Visi Machining Manual

INTRODUCTION

INTRODUCING

The following examples show how each of the 2D machining strategies are used and gives an explanation of how they work. All 2D machining is performed on profiles, you should be familiar with profile creation from day 1 of the basic modelling course. A brief explanation of profile creation will be given at the start of the machining course. Included within the 2D machining we will cover basic drilling and point sets.

BASIC 2D MACHINING

V12.x Revision 1

VERO INTERNATIONAL SOFTWARE

1

Select WIREFRAME/PROFILES/CLOSE and pick one of the elements that make up

Profile Creation

Select the FILE/OPEN command and open the file 2D Milling Example.wkf from the training folder.

the outer profile (See Fig 3.0). Select the automatically close the profile.

A from the icons presented on the left to

You should see the following part. (See Fig 1.0)

Select ‘A’ for Automatic Figure 3.0 This will join all elements, travelling in the direction of the arrow, to become one profile. Select ‘Yes’ to confirm the profile creation Figure 1.0 : 2D Milling Example Select the WIREFRAME/ PROFILE/QUICK command Make sure the intersection icon is selected and pick anywhere inside the centre slot. This will create a profile for the middle slot (See Fig 2.0).

We now have created profiles for all of the provided geometry. Now we must define the required thickness for each profile. “NOTE’’ All profiles must have a thickness and material side before any 2D machining can be performed on them. Pick inside centre profile

Select MACHINING/PROFILE CAM ATTRIBUTES and pick the outer profile (See Fig 4.0).

Pick inside profile

Outer Profile Arrow pointing outwards Figure 2.0 : 2D Milling Example

Select again outside the two slots (as indicated above), this will automatically create all profiles apart from the outer rectangle (See Fig 2.0). Figure 4.0

VERO INTERNATIONAL SOFTWARE

2

VERO INTERNATIONAL SOFTWARE

3

The direction in which the arrow is pointing on the highlighted profile is an indication of the material side. When the arrow is pointing out then it is indicating that the material is on the outside and all machining will be calculated on the inside (a pocket). For this example, the outer most profile will have the material side pointing outwards.

Profiles - PF1, PF2, PF3, and PF4 (CIRCULAR SLOTS) all material sides to be outside (arrows pointing outwards) and the thickness to be as follows (See Fig 5.0).

‘The material side can be changed by pressing the space bar’ When the arrow is pointing inside then it is indicating that the material is on the inside and all machining will be calculated on the outside (a boss). Once the required material side has been selected hit the right hand mouse button and you will be presented with the following dialogue box. Profiles - PF5, PF6, PF7, PF8 and PF9 (CIRCLES & LARGE LINEAR SLOT) all material sides to be outside (arrows pointing outwards) and the thickness to be as follows (See Fig 5.0).

Enter the values as in the box above and select ‘OK’

We have now assigned a material side and thickness to one of the profiles.

Profile - PF10 (SMALL LINEAR SLOT) material side to be outside (arrow pointing outwards) and the thickness to be as follows (See Fig 5.0).

Repeat the procedure for the remaining profiles with the values shown on the next page.

PF1

PF2 PF5

Profile - PF11 material side to be inside (arrow pointing inwards) and the thickness to be as follows (See Fig 5.0).

PF6

PF10 PF9 PF8

PF4

PF7

PF3

‘The material side can be changed by pressing the space bar’

PF11

NOTE : The colour of a pocket and a boss are different

Figure 5.0

We now have all the profiles set ready for machining

VERO INTERNATIONAL SOFTWARE

4

VERO INTERNATIONAL SOFTWARE

5

10. Expand/Collapse all Tree items – This will expand all the tree items of all the operations and active projects. 11. Copy – Copies the selected toolpath. 12. Operations Ordering – Here you can re-order the toolpath into the sequence that you require. Operations can be ordered using different methods, at any time the original order can be re-instated. 13. Edit Toolpath – This allows the user to edit the toolpath completely. Points on the toolpath can be edited or even deleted if necessary. 14. Toolpath Trimming – With this option a toolpath can be trimmed to a profile or a set of profiles. The internal or external part of the trimmed toolpath can be retained. A copy of the original toolpath can also be kept. 15. Tool Length Check – This allows the user to calculate the minimum presetting length of the current tool. 16. Geometrical Tools – Provides a set of tools that allow the creation of boundaries (profiles) using 5 methods and tessellated fillet surfaces. Both of these can aid in the creation of new programs. 17. Sub-Path Trimming – This is similar to toolpath trimming but differs in that you can remove individual levels or areas of a toolpath. 18. Edit Approach/Retract – The approach or retract distance of the toolpath can be altered here. An absolute or relative position can be used. 19. Pick Operation – If there are many toolpaths visible on the screen then this icon will let you pick an operation and automatically highlight which toolpath you selected within the operations manager. 20. Paste – Will paste the copied toolpath. 21. Jobs Manager – This is where all the information is gathered and set-up for the batch processing of multiple operations outside the system using the Visi-Batch Scheduler. 22. Show/Hide log window – When activated this will show/hide the log window of the last calculated toolpath in the current working session. The log window gives information such as: - start and finish calculation time, total calculation time and whether or not the calculation was performed successfully. 23. Edit parameters – Allows the parameter editing of the selected item in the operations manager. 24. Delete operation – A selected operation can be deleted using this icon (as opposed to the whole project). 25. Change attribute – This allows the user to change the attributes of the selected toolpath. 26. Verify Toolpath – Using this icon, the toolpath is simulated more graphically. Individual or sets of toolpath can be simulated at once from a 3D solid block. Will not handle multiple origins, inclined tools etc. Runs quicker than icon 27. 27. Simulate Toolpath – This is where the toolpath is simulated with more features. Multiple origins, inclined tools etc. are all handled. Runs slower than icon 26. 28. Change NC – Different post processors are selected here and the selection will post the programs using the selected post for the current session only. 29. New Project – New projects are created via this icon. Projects allow the grouping together of machining operations. 30. Batch Build – This is where the toolpath is calculated. Once all the values have been set within the machining parameters then the toolpath must be calculated.. Multiple toolpaths can be selected and calculated sequentially.

VERO INTERNATIONAL SOFTWARE

8

Select – NEW OPERATION New Operation

First select ‘2D Operations’

Pocketing Spiral

Select ‘OK’

VERO INTERNATIONAL SOFTWARE

9

You will now be presented with the tool library.

Now we are presented with the following dialogue box.

Operation Parameters

Select tool number 2 - the ‘10mm End mill’. The islands have automatically been recognised so all we need to do now is to set up the operation parameters.

Select ‘OK’

Double-click on operation parameters. You will then be presented with the following form. We are now prompted to select the profile to machine. Select the outer rectangular profile and any islands will be automatically selected. These can be shown from within the operations manager

VERO INTERNATIONAL SOFTWARE

10

VERO INTERNATIONAL SOFTWARE

11

Machining Form Distance between passes - This is the distance between each pass needed to machine the pocket. The default is half of the cutter diameter. Bottom/Lateral Oversize - This is the amount of material left on for finishing. The bottom and side values can be different. NOTE – This is not the amount of material left on the islands, this is set using a different switch. Safety Distance - This is the distance from the profile (incremental value) at which the tool will start its approach at feed rate, after the initial rapid move. Starting Z - This is the value at which machining movements begin at feedrate. The default value is the top of the profile. Max Depth of Cut - This is the value set for each Z level pass. This value is calculated automatically, be default it is displayed as the same value as the diameter of tool. Last Pass Z - This value will be automatically calculated to identify the depth for the final cut or last pass. It may be used to generate a later smaller depth finishing cut to clear the bottom of the profile. Use Clearance Plane - This switch allows you to avoid unnecessary rapid movements to the Clearance Plane. If switched off, a movement to the clearance plane will be forced between each machining level.

Islands/Approach/Retract Form Approach Mode

Clearance Plane - This is the default Z plane defining the final Z level relative to the top of the profile at which all rapid moves are made.

Feed

-

If selected, it defines that the descent to the start point is made in feedrate mode.

Final Z Plane - This is the plane defining the Z level where the tool will return after each operation. It is normally the same as the clearance plane but may also be set to a different value where an obstacle is to be avoided or where the tool should return to a specific height between consecutive toolpaths.

Rapid

-

If selected, it defines that the descent to the start point is made in rapid mode.

Use Bottom Radius/Bottom Radius - This will allow a radius to be roughed out at the bottom of a pocket when the flag is active, the size of the radius is set by the value entered in ‘Bottom Radius’ dialogue box Use Draft Angle - This switch allows you to set a Draft Angle to be applied on the profile during the machining. This does not apply to the draft angle of islands, this can be set with another switch. Residual Profiles - Lets you automatically generate any residual profiles showing where the current tool has not removed any material. This material may normally be removed by a subsequent operation using a smaller tool. Auto Rebuild - If this flag is active, the system to automatically re-calculate the machining once you select OK.

Descending -

Zig Zag

If selected, it defines the approach will be an angular move. When used, the starting point will be automatically selected. -

If selected, it defines a ZigZag approach. When used, the starting point will be automatically selected.

Descending Angle - This parameter is available only if the Descending Approach Mode has been selected. It represents the tool-descending angle. Descending Step - This parameter is activated only if a ZigZag Approach Mode has been selected. It represents the maximum Z step to reach the right depth. Islands Face Mill - When active this will allow the user to specify a top oversize on the islands. The islands will be automatically cleaned during the pocketing operation. Top/Lateral Oversize - This is the value that represents the amount of stock that you want to leave on the top and sides of each island. Use Draft Angle - This is the value of the draft angle to be machined on the islands.

VERO INTERNATIONAL SOFTWARE

12

VERO INTERNATIONAL SOFTWARE

13

Fill the values into the Machining form the same as the values below

Cutting Condition Spindle Speed - This is the spindle speed of the tool displayed in RPM The Approach should be ‘Descending’ Plane Feedrate - This is the Feedrate of the tool or the cutting feed displayed in mm/min

Select ‘OK’

Feedrate into Material - This is the plunge feed of the tool when feeding down to each cut and is displayed in mm/min.

The Machining will calculate automatically and the result should be similar to the picture below but you will only see one view. Press ‘F2’ to see the other views…

*Length Compensation Number - This is the number that is read by the post processor for any Length Compensation Number that might be needed for the program. *Cutting Side - This is where you specify where the tool should be climb or conventional milling. *Coolant - This is where the type of coolant can be specified. *User Remark and PP info - are specific for the post processor. Ask your instructor for a more detailed explanation.

NOTE : All of the flags marked * will not effect the calculation in any way and the values will only become visible when the program has been post processed.

VERO INTERNATIONAL SOFTWARE

14

VERO INTERNATIONAL SOFTWARE

15

We have now calculated our first 2D machining strategy. Simulate the toolpath to see the results.

After we have simulated the toolpath, clear the toolpath and then select ‘New Operation’ to create our second toolpath.

Select the ‘Toolpath Simulated display’ icon Select ‘Quick Pocketing’

Select ‘Quick Pocketing’ The system will now show the first level of the toolpath onscreen and a new set of icons will appear on the left: Select tool number 2 - the ‘10mm End mill’. These icons control the display and animation of the toolpath. You can: See individual levels. See all levels. Move to the first or last level. Simulate the tool in shaded or wireframe mode (VISI must be in ‘shaded display mode’ for a shaded tool to be available). Set the tool transparency. Exit back to the Operation Manager

10mm End Mill If you click the ‘show tool’ icon, the animation icons will also appear as shown below:

These icons control the animation of the toolpath. You can: Play, pause and stop the animation. Jump the animation to the next point in the toolpath. Speed up or slow down the animation. (Note: the animation speed can also be set with the keyboard + and - )

VERO INTERNATIONAL SOFTWARE

16

Select ‘OK’

VERO INTERNATIONAL SOFTWARE

17

We now have to select the profiles we want to machine. Select the 4 circular profiles and the large linear slot profile in the centre of the model. (PF5, PF6, PF7, PF8 and PF9) Use Block control to pick more than one at any time.

The results will be as follows: -

Simulate the toolpath to see the results. We have now completed our second 2D machining strategy. Most of the 2D strategies are very similar to those shown and are easy to follow.

Double click the ‘Operation Parameters’ and fill in the values as the picture below.

Quick Pocketing will apply the same values set in the operation parameters to all of the profiles selected, regardless of depth, shape or material side. The rest of the operation parameters are almost identical to the previous operation. Refer to the previous operation for an explanation of the commands.

VERO INTERNATIONAL SOFTWARE

18

VERO INTERNATIONAL SOFTWARE

19

Clear the toolpath and then select ‘New Operation’ to create our next toolpath.

We are now presented with a selection of tools from the Visi-tools database of milling tools. It is from here where we can select the desired tool.

Select ‘Quick Milling’

Quick Milling

We are now going to select a tool that is not in the current library.

Select to create a tool from the Global Library

Create tool from Global Library

Select the second 4mm-end mill

Select this end mill

Select ‘Mill’ and ‘OK’

VERO INTERNATIONAL SOFTWARE

Select ‘OK’ to the speed and feed defaults

20

VERO INTERNATIONAL SOFTWARE

21

We now have to select the profiles we want to machine. Select the 4 circular slot profiles PF1, PF2, PF3 and PF4. Use Block control to pick more than one at any time.

PF1

The option differences between pocketing and milling operations in 2D are as follows: Machining Form

PF2

PF4

PF3

Double click the ‘Operation Parameters’ and fill in the values as the picture below. Diameter Compensation – This section allows you to apply the DIAMETER COMPENSATION NUMBER that is used on the CNC control as a corrector for any adjustments needed on the size of the piece. The LENGTH COMPENSATION NUMBER which works in a similar way to the diameter corrector and calls values from the CNC control. Toolpath Offset These parameters apply different offset strategies according to your requirements. None – This means that the system will leave the centre of the tool on the selected profile with no offset applied. Profile Offset – When this flag is activated the toolpath is offset by half of the cutter diameter and also allows the use of the diameter compensation switch. Profile Corrected – This allows the centre of the tool to be left on the profile although the toolpath is adjusted and extra circular moves are added where necessary.

Quick Milling will apply the same values set in the operation parameters to all of the profiles selected, regardless of depth, shape or material side.

VERO INTERNATIONAL SOFTWARE

22

VERO INTERNATIONAL SOFTWARE

23

Select ‘OK’ and display the toolpath. The result will be as follows

Approach/Retract Form

Profile Approach Direct – The tool moves directly away from the last tool position to the start point in a straight line. Perpendicular – This allows a perpendicular approach to the start point of the selected profile. The approach point is projected perpendicular from the start point. Circular – This will create a circular approach from the selected starting point on the profile. Helicoidal - This will create a tangential approach to the selected start point but uses a 3 axes helical move to perform the approach.

Simulate the toolpath to see the results. We have now completed our third 2D strategy. Most of the 2D strategies are very similar to those shown and are easy to follow. You should now be at a stage where you can start to understand the principle of how 2D machining works.

Approach Radius – This will let the user enter the required radius for the approach and is only active with the circular and helicoidal approach mode selected.

Profile Retract Direct – The tool moves directly away from the last tool position to the retract point in a straight line. Perpendicular – The tool moves away perpendicularly form the end machining point to the retract point. Circular – This will move the tool circularly away from the machining end point to the retract point. Retract Radius – This will let the user enter the required radius for the retract method and is only active with the circular retract mode selected. Material Approach Feed or Rapid determines whether or not the descent to the start point is a Feed or Rapid move.

VERO INTERNATIONAL SOFTWARE

24

VERO INTERNATIONAL SOFTWARE

25

We will now machine the final slot profile.

Clear the toolpath and then select ‘New Operation’ to calculate our next toolpath.

Select ‘Milling’

PF10

Select ‘Milling’

For the last operation we will select a tool from the current library. Select the small centre profile ‘PF10’ We are now asked to select the start and finish machining points for the final profile. Select the mid-point of the long bottom edge of the profile as both the start and end machining point.

Start and end point

Select ‘6mm End Mill’

We could now change the machining direction from climb to conventional milling if we needed*. For this profile we will accept the default so select the right hand mouse button to confirm the machining direction.

Select ‘OK’ to confirm the tool selection

*NOTE By pressing the space bar we can change the machining direction from climb to conventional.

VERO INTERNATIONAL SOFTWARE

26

VERO INTERNATIONAL SOFTWARE

27

We have now machined our first 2D job and the same principles applies to all 2D machining strategies on any job.

Double click the ‘Operation Parameters’ and fill in the values as the picture below

Go through the following examples using the strategies you have already learned and apply your own parameters to the strategies. You will be given the depths of the profiles and the rest is up to you. Example 1 Select the workfile ‘Example 1.wkf’

Select ‘OK’ and display the toolpath. The result will be as follows

The profiles should have the following values.

Outer profile = Material pointing inwards

4 off large circular profiles = Material pointing outside (pocket) 50mm thickness

This operation is almost the same as quick milling and all the parameters in the forms are identical. Refer back to the quick milling operation for an explanation of all the parameters on each form.

VERO INTERNATIONAL SOFTWARE

28

VERO INTERNATIONAL SOFTWARE

29

4 off circular slots = Material pointing inwards (bosses) 30mm thickness

Example 2 Select the workfile ‘Example 2.wkf’

Larger inner circular profile on datum = Material pointing outside (pocket) 20mm thickness PF1

PF3

PF4 PF2

Small inner circular profile on datum = Material pointing outside (pocket) 50mm thickness

The profiles will have the following values. PF 1 = material pointing outside (pocket)

Using the information given create the machining for the above file.

PF 2 = material pointing inside (boss)

VERO INTERNATIONAL SOFTWARE

30

VERO INTERNATIONAL SOFTWARE

PF 3 = material pointing inside (boss)

31

Open the file ‘Profile and section1.wkf’ PF 4 = material pointing outside (pockets)

4 off circular profile = material pointing outside (pockets)

The model consists of one ‘closed’ shape profile and one ‘open’ section profile. NOTE Only one section profile can be used at any one time. Open ‘Operation manager – New operation – 2D operations – Profile Section’

VERO INTERNATIONAL SOFTWARE

32

VERO INTERNATIONAL SOFTWARE

33

Select ‘T3 – 6mm Ball Nose tool’

Change the settings to match the following : -

Select the bottom planer shape profile and pick a point on that profile to indicate the start and end machining point. Confirm the machining direction using the ‘RHM’ button Now select the ‘section profile’ and use the ‘RHM’ button to confirm the machining direction. Open the ‘Operation Parameters’ Select ‘OK’

The result will be the same as shown above.

VERO INTERNATIONAL SOFTWARE

34

VERO INTERNATIONAL SOFTWARE

35

Open the file ‘Revolution Example.wkf’ Open ‘Operation manager – New operation – 2D operations – Revolution’

There is only one ‘open’ profile present. The first thing that must be done is the profile must have a machining side attached to it. This is necessary to determine whether or not the cutter will class the machining as inside or outside. NOTE There is no need to assign any thickness to the profile as no thickness is need for this particular strategy, but giving the profile thickness will not affect the machining. Select ‘T3 – 6mm Ball Nose tool’ Select ‘Machining – Profile CAM attributes’ and pick the profile. Make the material side ‘Inside’ as shown below: -

NOTE Only Ball Nose tools can be used on this strategy Select the profile and confirm the default machining direction using the ‘RHM’ button. Use the ‘RHM’ button to confirm that there are no machining boundaries.

No thickness is needed on the profile

VERO INTERNATIONAL SOFTWARE

36

VERO INTERNATIONAL SOFTWARE

37

We now have to inform the system where the machining centre will be and what will be the machining axis.

Open the ‘Operation Parameters’

Enter ‘X0, Y0 and Z0’ for the machining centre

And ‘X’ as the revolution axis. Confirm using the ‘RHM’ button

Change the ‘Constant Step’ to 1mm and calculate the machining.

The result will be as shown above.

VERO INTERNATIONAL SOFTWARE

38

VERO INTERNATIONAL SOFTWARE

39

The toolpath in our case has machined above the profile when the ‘Start and End angle’ were 0° and 180° respectively and the profile was above the revolution axis. If the profile was below the revolution axis but the ‘Start and End angle’ was the same the result would be different. This is shown below.

Open the file ‘Extra 2D operations.wkf’

Profile above Revolution axis

Switch on the layers ‘Layer 1 and Open Pocket Profiles’

Profile below Revolution axis, same settings used

VERO INTERNATIONAL SOFTWARE

40

VERO INTERNATIONAL SOFTWARE

41

Open ‘Operation manager – New operation – 2D operations – Open pocket

Select the top one of the 2 profiles and select the straight end segment as the open part

Select this edge as the open segment

Confirm the profile and edges using the ‘RHM’ and ‘confirm selection’ Select ‘T2 – 10mm End Mill’

We now must select the profile to be used for this strategy and also select the open edges from the profile we have just selected. The open edges are where the tool will cut outside and are confirmed using the ‘RHM’ button and ‘confirm selection’. Open the operation parameters and set up the parameters as laid out on the next page. You will notice that all the parameters are very similar in this strategy to the existing pocketing strategy. An explanation of these settings and parameters has already been given earlier in these notes. Please refer to those for an explanation of the parameters.

VERO INTERNATIONAL SOFTWARE

42

VERO INTERNATIONAL SOFTWARE

43

Please setup the parameters as follows for this strategy: -

The result will be as shown above and the machining goes outside the selected open edge. Select ‘OK’

Repeat the process for the lower profile

Next, the system will ask you to ‘Indicate the approach point’

Clear the toolpath from the display.

Press ‘F2’ until you have a top view.

Switch on the layers ‘Layer 1 and Helical Milling Profiles’

Note: the outer toolpath pass is shown to aid selecting the approach point (you would normally approach from outside the pocket) Select a point (intersection free point) similar to the one shown below: -

VERO INTERNATIONAL SOFTWARE

44

VERO INTERNATIONAL SOFTWARE

45

Open ‘Operation manager – New operation – 2D operations – Helicoidal Milling

Use the ‘RHM’ button to confirm the cutting direction. Open the operation parameters and you will be presented with the following form. Once again you will notice that all the parameters are very similar in this strategy to the existing pocketing strategy. An explanation of these settings and parameters has already been given earlier in these notes. Please refer to those for an explanation of the parameters. An explanation of the different parameters is given below. Pitch This is in effect the depth of cut. It is the distance the tool will travel in Z from one complete circular tool movement to another. Final Contour This option ensures that there is an extra circular pass added to the bottom of the toolpath. This makes sure that when you are machining into a blind hole, the bottom of the hole will be flat. Change the parameters to the ones show below and select ‘OK’

Select a 20mm tool from the global library

Select ‘OK’ Now select one of the 2 circular profiles. The system will now ask for the start\end machining point and the direction. Select the ‘Centre point’ icon and pick the centre of the profile.

VERO INTERNATIONAL SOFTWARE

46

VERO INTERNATIONAL SOFTWARE

47

Open ‘Operation manager – New operation – 2D operations – Mill Thread

There are no thread mill tools in the default library, so we will have to create one manually: -

The result will be as shown above. Notice the extra pass at the bottom of the hole. Repeat the process for the other profile Clear the toolpath. Enter the tool parameters as shown below: Switch on the layers ‘Layer 1 and Thread Milling Profiles’

VERO INTERNATIONAL SOFTWARE

48

VERO INTERNATIONAL SOFTWARE

49

Open the operation parameters and fill in the following parameter as laid out below.

Select ‘OK’to create the tool Thread Milling can be done either from profiles or points. We will mill the thread using profiles

Select the 2 profiles and confirm the selection using the ‘RHM’ button

Once the operation parameters dialogue box is open you will be presented with the previous form. Once again you will notice that all the parameters are very similar in this strategy to the existing pocketing strategy. An explanation of these settings and parameters has already been given earlier in these notes. Please refer to those for an explanation of the parameters. An explanation of the different parameters is given on the next page.

VERO INTERNATIONAL SOFTWARE

50

VERO INTERNATIONAL SOFTWARE

51

Nominal Diameter

This value relates to the actual thread diameter and the value is taken from the size of the profile selected, or a default value is entered if a point is selected. Internal Diameter The internal diameter is the internal size of the thread and this value will change depending upon whether an internal or external thread is selected. Thread Length The depth of the thread is determined here and this value indicates the depth to machine. The value is taken from the attributes assigned to the profile selected, or a default value is entered if a point is selected. Start Machining Angle This value is the angle about the Z-axis where the machining will start around the thread Number of Pitches This is the complete number of threads taken from the tool parameters that will be machined on the component. For example if the value is set to 5 and the pitch is 2 then the system will machine the full depth of the thread in a series of 10mm cuts. Threading type – Internal and External Internal or External thread type determines where the tool will produce an internal or external thread form on the component.

The result will be as shown above. Try to changing the values and options within the operation parameters to see the different results that can be achieved.

Clear the toolpath Pitch type – Left or Right This flag defines either a left or right hand thread. When these switches are activated the machining will be from either the top to the bottom of the thread or vice versa depending on whether conventional or climb milling is used.

Switch on the layers ‘Layer 1 and Blending Profile’

Change the parameters to the ones show on the previous page and select ‘OK’

VERO INTERNATIONAL SOFTWARE

52

VERO INTERNATIONAL SOFTWARE

53

Now select the open profile near the radius on the top of the open pocket and the start and end machining point on the profile as opposite ends of the profile.

Open ‘Operation manager – New operation – 2D operations – Blending

Select the profile

Select the start and end point for the machining

Select ‘T3 – 6mm Ball Nose’ Open the operation parameters and you will be presented with the form shown on the following page. Once again you will notice that all the parameters are very similar in this strategy to the previous strategies. An explanation of these settings and parameters has already been given earlier in these notes. Please refer to those for an explanation of the parameters. An explanation of the different parameters is given below

This strategy is very similar to the profile and section strategy that was explained earlier on in the notes. The difference is the following parameter.

*NOTE: - Only Ball Nose/Bull Nose and Corner rounding tools can be used for this type of strategy.

Fillet Radius This is the size of the radius to be machined

Select ‘OK’

VERO INTERNATIONAL SOFTWARE

54

VERO INTERNATIONAL SOFTWARE

55

Change the parameters to the ones show below and select ‘OK’

Now select the open profile near the radius on the top of the open pocket and the start and end machining point on the profile as opposite ends of the profile. Open the operation parameters and you will notice that the machining form is different because of the different tool that we selected. Once again you will notice that all the parameters are very similar in this strategy to the existing strategies. An explanation of these settings and parameters has already been given earlier in these notes. Please refer to those for an explanation of the parameters. An explanation of the different parameters is given below Guide point – High and Low This flag determines where the application point for the machining will be calculated from with regard to the tip of the tool and the profile. The High flag assume the machining to be calculated from the top of the profile and the Low flag the machining to be calculated from the bottom of the radius defined on the tool. If the profile top and bottom were set to 0 and –20 respectively, and the radius on the tool was 5mm, then if the flag was set to be low the machining would not go lower than –5mm. Change the parameters to the ones show below and select ‘OK’

On this particular strategy the operation parameters form will change depending on the tool that is selected. Repeat the procedure but create and use a corner-rounding tool with the following parameters.

VERO INTERNATIONAL SOFTWARE

56

VERO INTERNATIONAL SOFTWARE

57

Open ‘Operation manager – New operation – 2D operations – Chamfering

The result of each toolpath will be as below: -

Select ‘OK’ Clear the toolpath We now need to create a tool manually with the following parameters Switch on the layers ‘Layer 1 and Chamfering Profiles’ Select ‘Create tool manually’

Create a chamfering tool with the following parameters

VERO INTERNATIONAL SOFTWARE

58

VERO INTERNATIONAL SOFTWARE

59

Now select the open profile and also the start and end machining point on the profile Select the profile

Radial and Axial

These 2 options define what type of multiple passes will be created on the toolpath. The Radial option defines a number of vertical steps to clear material to the chamfer and the Axial option defines a number of horizontal passes to the chamfer. Approach/Retract Disengagement type – Radial and Axial This defines the disengagement type of the tool from the chamfer. The Radial option represents a retraction towards the tool centre by the distance entered in the Input value and the movement type is radial from the cut on the profile. The Axial option represents a retraction towards the tool axis by the distance entered in the Input value and the movement type is axial from the cut on the profile. The Preset diameter allows the user to enter a diameter in the Input value and this is the diameter that the toolpath will offset to when disengaging the toolpath.

Select the start and end point for the machining

Change the parameters to the ones show below and select ‘OK’

Open the operation parameters and you will be presented with the form displayed on the next page. Once again you will notice that all the parameters are very similar in this strategy to the previous strategies. An explanation of these settings and parameters has already been given earlier in these notes. Please refer to those for an explanation of the parameters. An explanation of the different parameters is given below Chamfer Depth and Chamfer width The values entered here are the vertical and horizontal sizes of the chamfer to be machined Angle Is the angle of the chamfer with respect to the vertical axis Depth Mode This determines whether the chamfer will be machined by entering a value for the depth and width or the width and angle Multiple Passes This option defines the approach type to the first pass on the profile and is used in conjunction with the number of passes and the Radial or Axial option. Number of passes This defines the number of passes used to use with the Radial or Axial option when the toolpath is generated.

VERO INTERNATIONAL SOFTWARE

60

VERO INTERNATIONAL SOFTWARE

61

The result of the toolpath will be as set out below: -

Open ‘Operation manager – New operation – 2D operations – Extrusion

Clear the toolpath

Switch on the layers ‘Layer 1 and Extrusion Profiles’

Select ‘OK’

Select ‘T3 – 6mm Ball Nose’

VERO INTERNATIONAL SOFTWARE

62

VERO INTERNATIONAL SOFTWARE

63

Perpendicular Mode When this flag is activated it will create the machining toolpath perpendicular to the vertical profile that was originally selected.

Now select the curved profile on the model.

Change the parameters to the ones show below and select ‘OK’

Use the space bar to select the machining direction and confirm the selection with the ‘RHM’ button (In this case, we will machine in the downwards direction) Open the operation parameters and you will be presented with the form displayed on the next page. Once again you will notice that all the parameters are very similar in this strategy to the previous strategies and in particular the Profile and Section strategy. An explanation of these settings and parameters has already been given earlier in these notes. Please refer to those for an explanation of the parameters. An explanation of the different parameters is given below: -

Left\Right Extrusion Distance This is the machining extrusion distance to the Left/Right of profile (looking along the direction of the profile) Left\Right Cut Depth The values entered here refer to the depth of cut that is applied to the extruded machining to the left and right of the profile. Although these parameters actually seem to be the same and give the same results they are in fact different and can be used to in different ways to machine only a section along the profile. An example of this is given below.

VERO INTERNATIONAL SOFTWARE

64

VERO INTERNATIONAL SOFTWARE

65

The results should be as below: -

Try some different settings yourself on all the strategies explained in these notes. You may have noticed that in the ‘Operation Manager’ the colour of text of the strategy name changes based on its status. The colours are as follows: x

A GREEN strategy means that the toolpath is new and has yet to be calculated.

x

A PURPLE strategy means that the toopath has been calculated but some parameters have been modified and the toolpath needs to be recalculated.

x

A BLACK strategy means that the toolpath has been calculated successfully

x

A RED strategy means that the toolpath cannot be calculated with the parameters you have supplied. Look in the ‘CAM log window’ for an indication as to the problem.

Congratulations! Open the operation parameter again and change the values to the following and select ‘OK’ Right Extrusion Distance Right Cut Depth

= =

This completes the basic 2D milling tutorial

-70 20

The result will be the same as below and only a 20mm section of the profile has been machined but away from where the original profile is positioned.

VERO INTERNATIONAL SOFTWARE

66

VERO INTERNATIONAL SOFTWARE

67

Drilling Select the file ‘Drilling Example1.wkf’

Open the ‘Operation Manager’

Open up the type of cycle you require, for this example we will choose ‘Drilled Hole’

Select here to open drilling cycles

Select ‘New Drill Cycle’

You will now be presented with the following form.

VERO INTERNATIONAL SOFTWARE

68

VERO INTERNATIONAL SOFTWARE

69

We now have to choose what type of hole we are going to drill, whether the hole is to be a through hole or a blind hole.

Geometry selection means we can pick up the required information about the diameter and depth of the hole from a 3D model if available.

Select ‘Through Hole’ from the drop-down Cylinder selection allows the diameter and depth to be defined by selecting a cylinder from the 3D model. The information from that cylinder is then transferred from the model to the correct D and DP values.

Circle selection allow the diameter to be defined by selecting a circle from the geometry and the information from that circle is then transferred from the data to the values of D. The depth must be entered manually

Through Hole

Select ‘Circle info’

Click “Apply”

We now have to pick a circle from the drawing provided. We now have to give a size and depth for the holes we are going to drill. Select one on the 12 circles from the drawing.

Select a circle

This is the main form where we enter the sizes and depths for the holes. You will now see the diameter of the hole is entered in the dialogue box Value D = Diameter of the hole in question Value DP = Depth of the hole* *NOTE The depth of the hole is taken from the land of the drill and not the tip.

VERO INTERNATIONAL SOFTWARE

70

VERO INTERNATIONAL SOFTWARE

71

We now have to select the holes that we want to drill. Holes can be picked from points on model e.g. Midpoint, Endpoint, Intersection, or centre point. It is also possible to select pre-defined points already created. We will select the points already created. Select the point’s environment selection method.

Enter a value of 40 in the DP dialogue box (this will then drill the hole 40mm deep)

Select ‘OK’

Now select one of the points at the centre of one of the diameter 12 holes. You will automatically be taken back to the form above and probably think that noting has happened. Now select ‘OK’ The cycles will be created and placed in the ‘Operations Manager’ and will disappear from the ‘Fixed Cycle’ panel. NOTE : The system automatically picks up the correct drill, in this case a centre drill is also selected.

The ‘Fixed Cycle’ panel is still active and is waiting to carry on with more drilling routines as required. Select ‘Cancel’ to exit.

Each cycle is different and trying different cycles will select different tools assigned to each cycle. The ‘TOOL PARAMETERS and CYCLE PARAMETERS’ can be edited here or at a later stage. We will accept the defaults for this example.

VERO INTERNATIONAL SOFTWARE

72

VERO INTERNATIONAL SOFTWARE

73

The result will be as follows.

Machining Form Drill Type: Normal – This is the standard drilling type, this will force the tool to drill straight to depth and then rapid back out of the hole. Chipping – This is where the drill stops at a set depth and rapids back off by a few mm and then starts to feed again to the drill depth and does this all the way to the full depth of the hole. Pecking – This is similar to chipping but will rapid all the way out of the hole and rapid back to a safe distance from the last Z value and continues to work in this way until the full depth of hole is reached. Param1, 2 & 3 – These parameters are only used for ‘chipping’ and ‘pecking’ cycles. Param1 allows you to set the ‘Z’ increment. Param2 allows for the dwell time to be set and Param3 is post-processor dependant.

If we now enter the ‘Operations Manager’ you will now see there is 2 drilling cycles, one for centre drilling and one for drilling. All the operation parameters are now just like any other cycle and are fully editable. An explanation of the operation parameters are as follows.

Depth Management Set Depth/Set Diameter - Only applies when using a CNC type combined centre drill and chamfer style tool. You can select to go to a specific depth or diameter. Depth - This is the calculated drill depth to the point of the drill. (You set the depth to the shoulder and the system automatically calculates the depth to the point). Mark Diameter - This value is only applicable for the centre drill and works from either the depth or the distance across the diameter of the centre drill. See below. Starting Z – This is where the drill starts to drill to the depth you set (relative to the ‘Z’ position of the point(s). A positive value will start drilling the holes that distance BELOW the point(s) you select. A negative value will start drilling above the point(s)

You must first activate the ‘Set Diameter’ switch and then when a value is entered in the ‘Mark Diameter’ you can then compute the correct depth from the value entered.

Compute Depth value

Optimise Toolpath* – This will allow the user to view different ways in which the tool will travel between holes. Different variations can be tried here, which include No optimization, Min X or Y distance, shortest toolpath and minimum distance. *NOTE This is not applicable on sets of points.

VERO INTERNATIONAL SOFTWARE

74

VERO INTERNATIONAL SOFTWARE

75

NOTE: It is also possible to set the machining attributes for groups of profiles rather than just individually as detailed on the previous page.

Select - MACHINING/OPERATIONS MANAGER

On the Machining menu you will see the command ‘Quick Profile attributes’

Using this command, you are able to pick multiple profiles and apply machining attributes to them NOTE: The same attributes will apply to all profiles picked at the same time using this method….. i.e. The material side and heights will be the same for all profiles picked at the same time.

You will now be presented with the dialogue box shown above. The icons within the Operation Manager dialogue box are explained below: -

If you use this command, the panel shown below will appear: -

Notice that the second box has the legend ‘Negative thickness’. This means that a negative value is implied in this box and therefore a minus sign is not required…. i.e. If the bottom of a pocket is at Z-50.0mm then you would enter a value of 50

1

2

3

4

5

6

7

8

9

10

11

12

13

14

15

30

29

28

27

26

25

24

23

22

21

20

19

18

17

16

1. 2. 3. 4. 5. 6. 7. 8.

We will now create the required toolpaths for this part.

9.

VERO INTERNATIONAL SOFTWARE

6

New Operation – This selects the type of operation or template file to use. New Drill Cycle – This selects the drilling options. Post Process – Select this to post process the calculated toolpath. Toolpath Simulated Display – This is where the toolpath is simulated within the model view environment. Display Toolpath – This displays the completed toolpath on the screen. Clear Toolpath – This icon hides the toolpath. Delete – This deletes the selected item. (Including the whole project if selected). Save template file – This is where the operations are saved into a template file and can be used on any other job. Print – Allows an HTML (or .xls) machining report to be produced of the calculated operations.

VERO INTERNATIONAL SOFTWARE

7

Rapid Management Clearance plane – The tool retracts to the clearance plane after every hole. The value of the clearance plane is set on the ‘Cutting conditions’ tab Safety distance – The tool retracts the safety distance after every hole. The value of the safety distance is set on the ‘Cutting conditions’ tab Absolute Z obstacle – Allows you to enter an absolute ‘Z’ value that the tool will retract to after every hole. However, the first and last moves will be at the clearance plane. Set Relative Z Obstacle – Allows you to dynamically ‘drag’ the ‘Z’ height of the toolpath between holes. i.e. To edit the toolpath to make it ‘jump over’ an obstacle. Obstacle Manager (icon) – This icon brings up the Obstacle Manager. With this icon you can select solids and nominate them as obstacles (clamps etc.) The system will automatically make the toolpath jump over the obstacles. Check collisions – Activates the checking of the solids (clamps) as selected in Obstacle Manager.

Select ‘Drilling Example 2.wkf’

Obstacle Manager

Refer to previous 2D operations for an explanation of the cutting conditions form. Complete the examples on the following pages using the information given and choose you own cycles and depths for the holes.

VERO INTERNATIONAL SOFTWARE

76

VERO INTERNATIONAL SOFTWARE

77

Select ‘Drilling Example 3.wkf’

Try different cycles on the files given to see the results. Use Tapping and Counterbore cycles to see how they work.

VERO INTERNATIONAL SOFTWARE

78

INTRODUCTION

This training document is intended to give an explanation of how to create, edit and manage both the Machine Tool definition and Cutting Tool Libraries. We will learn how to use both of these and how they can aid in the manipulation of machining components. A Machine Tool definition is needed for the creation of NC programs for fixed 3, 4 and 5 axis-machining centres. (The default is set as a standard fixed 3-axis milling machine.) Tool libraries are used to create a list of specific tools available for either all or specific machine tools.

ToolLibraries

You will be presented with the following form

Select the menu item > Machining > NC-machines manager.

The standard installation comes with a few machines already configured. The one’s apart from the ‘Standard 3 Axis Milling’ are configurations for continuous 5-axis milling machines. We will step through the procedure of creating a new 3-axis machine in this tutorial: -

Select ‘New NC Machine configuration’ New NC Machine On this form, general information about the machine can be set. Edit NC Machine Delete NC Machine

Machine Description – We give a description of the machine here and you can enter anything you like. The type of machine is usually entered here e.g. Bridgeport, HAAS, Huron etc.

Copy NC Machine

Comment – Here you may enter some comment of you own, maybe the workshop where the machine is situated.

Show NC Machine Details

NOTE: - If you check ‘Set as default machine configuration’ then this machine will be used as the default machine when the system starts up. The post processor and library assigned to this machine will also be used. Default Local Library – Here you assign the tool library to be used with this machine. This box will allow a specific library to be assigned to a specific machine. Post Processor Configuration File – This is where you select the post processor to be used with this machine. You can always change the post later if required, but this will be the default post processor assigned to this machine.

For our training purposes, enter ‘Bridgeport’ in the Description and ‘Toolroom’ in the comment dialogue boxes.

Single Horizontal - In this case we have a horizontal 4-axis machine tool. The post processor considers it as an XYZ, plus an extra rotation around a primary axis.

Specific Configuration - To identify a machine tool with more axes you can select Leave the ‘Set as default machine configuration’ un-checked Leave the ‘Default local library’ set at none (we will create a new tool library next, then come back and attach it to our new Bridgeport machine)

the number of axis (1 or 2) after setting the specific configuration flag. If you select 2axis (i.e. 3-axis + 2-axis = fixed 5-axis) then the secondary axis portion of the panel will become available. Primary and Secondary Axis.

Next, we will set the default post processor for our new Bridgeport. Click the browse button, and then select the ‘Fanuc0m.cfg’ file. A large range of postprocessors is available. For this training example, we will stick with the Fanuc. Select the ‘Axes Parameters’ form. NOT PRESENT

Table, Divisor or Head – These options are for future implementation. With this version, selection of any of these three will not affect the NC output. Rotation Axis - When the post processor calculates new axis orientations, there is usually more than one way to achieve the desired result. Generally, there will be more than one potential combination of a primary and secondary axes rotation. The post-processor will always select the combination that can be effected with the minimum rotation. The initial axis angles may be defined as part of the configuration. When the configuration file is loaded, the contents are checked, and you will receive a warning message if the parameters are invalid. Rotation Axis On both the primary and secondary axis, you need to specify the tool axis and the letter for the rotation axes. The axis can be rotated A around X, B around Y or C around Z. Rotation Direction Bi-Directional – This flag means that the rotation of the fourth or fifth axis can be in either direction. Clockwise – This means that the rotation of the fourth or fifth axis can rotate only clockwise. Counter-Clockwise – This means that the rotation of the fourth or fifth axis can rotate only counter-clockwise. The user can specify the minimum and maximum angles of rotation around each axis.

This form is where we specify the way in which 4 and 5 axis positional machining will be handled when we post process a file that has machining on multiple faces. The default is ‘None’. If we change to Single Vertical, Single Horizontal and Specific Configuration we can then specify the type of 4th and 5th axis.

Rotation axis type None - In this case a classic 3-axis milling machine is set up and the post processor considers the machine as a simple XYZ axis machine. Is not important in this case if the machine is vertical or horizontal, the post processor will take care of the format output and the corresponding axis system will be used.

Single Vertical - In this case we have a vertical 4-axis machine tool. The post processor considers it as an XYZ, plus an extra rotation around a primary axis.

It is of course possible that you may create a machining operation that takes place in an orientation that is unachievable in your particular machining environment. In this case, the system will output an error message during post-processing.

Now we will create a new tool library, and then assign it to our new machine.

Select the ‘Extra Parameters’ form NOT PRESENT

Select > Machining > Local libraries manager.

The parameters here are used to configure a continuous 5-axis machine and are not described in this document The system supplies one default local library with a few tools already added. A sample tool-holder library is also provided. We will step through the procedure of creating a new tool library.

Select ‘New Local Library’ New Local Library

Tool Change This option allows you to select the tool change type (Automatic or Manual). This parameter will be used by the post processor, which will then output the correct information to the NC file. Change Position If the machine needs a special tool change reference point it is possible to define the correct tool change co-ordinates here (normally left at X0, Y0, Z0). Tool Axes This parameter is connected only to the rotary axes setting. If you have a machine tool with more than 3 axes, the tool axes identify the default tool direction in respect to the absolute co-ordinate system. In our case we are just defining another 3-axis machine. We will leave all the default settings set, apart from the ones we have already altered within the ‘General Parameters’ form. Select ‘OK’ and ‘OK’ We have now created a new machine.

Edit Local Library

Delete Local Library Copy Local Library

Copy Tools from Local Library

Display Library Details

We now presented with local library editing panel: -

Select ‘Create Tool from Global Library’

Select the type of tool to create.

Select ‘Mill’ and ‘OK’

Next, we will start to fill out our new library. Enter the Name of your new library in ‘Local Library Description’ (Use Bridgeport)

Now we need to start adding tools to our library. Tools can be created in 3 ways; they can be selected from a global library of tools, created manually or copied from one local library to another. New tools can also be made during the creation of a cutting operation. So even if we need a new tool on a job that is not in any library, we can always create them on the fly. The first tool we create will be copied from the global library. The global library is a list of tools that come as standard with the system.

We now have a list of tools available in the global database of milling tools and we can choose the tool we want to add to our new local library.

For our first tool we will select a 12mm End mill.

Click on the ‘Tool Holder parameters’ tab

This panel (shown on the next page) allows us to define a tool holder (or holder assembly) that will be associated with this tool. If a tool holder is added to a tool, collision avoidance and gouge detection are possible during 3D cutter path creation.

The tool holder must be defined as an assembly and can be made up of: 1. A tool holder 2. An extension 3. An adaptor Any combination of the above components can be included in the assembly. Select the 12 mm End mill with the 111 mm overall length and click ‘OK’ There are very few restrictions on how the tool assemblies can be added together, however, 1. Different Assemblies cannot be saved using the same name 2. You cannot save an empty assembly

The picture below shows the normal relationship of holder+extension+adaptor

Now we are presented with the cutting parameters form where we can set up the speed and feed for the selected tool. The parameters here will be explained when we create a manual tool.

A few example assemblies can be found in the ‘Default Tool Assembly Library’

Allows you to save the selected component(s) into the database. You have a choice to save the component(s) into either the tool holder, holder extensions or holder adaptors database .

Allows you to remove the selected component(s) from the assembly.

Removes all components from the assembly.

The values here control the relationship of the holder assembly to the machine spindle nose. They are only used during 5-axis (continuous) simulation A description of the Tool Holder parameters follows: The ‘Assembly Description’ box is used to name the assembly you are creating. You must provide a name before you click the save icon or the OK button.

Allows access to the holder’s database. From here you can create, modify and delete holders.

Allows access to the holder extensions database. From here you can create, modify and delete holder extensions.

Displays the presetting length. By default it equals: “Flute length + (Overall lengthFlute length)/2)” If a tool holder assembly has been added to the tool, the user can input a value that is different to the default. However, if a tool holder assembly has not been added, the default-preset length will remain in effect.

If enabled, this button will run the automatic tool length checking computation.

Allows access to the holder adaptors database. From here you can create, modify and delete holder adaptors. The system is able to automatically compute the minimum tool preset length based on a particular tool+holder assembly+tool-path combination. At this point in time, the auto calculate will be greyed out as we have no tool-paths computed. Allows you to bring in a pre-defined assembly.

Below is the Holder Definition panel: Remove the selected slice

Delete all displayed slice data.

Note. The user must supply a name for the holder before clicking on the OK button. The other panels for Holder Extensions and Holder Adaptors work in the same way. We will not add any tool holder data for this tool. Select ‘OK’ We have added one tool to our library.

Holder definition This user interface allows the user to define a slice of tool holder by inserting the top, bottom diameter and height.

Slice Z height

Slice bottom diameter

Slices editing These buttons allow the user to move and reorder the slices to define the required shape of the tool holder. NOTE: The “undo” button allows only one level of undo.

Add a slice under the selected position

These buttons allow the user to add a slice, remove a slice or remove all the slices.

Notice that there is no tool position assigned to this tool. We can set this at any time. We can set the tool position when we create the tool, after the tool has been created or even when we post process the program.

Other options on the local library form are: -

A red tick This means that this tool has already been used

Filters Tool Source, Type, Subtype and Diameter – These filters can be used to filter the display of tools. Each filter is activated by the check box to the right of that filter box.

A red bounded tick This means that this tool is the currently used tool A tool holder overlaid in the top right hand corner of the icon This indicates that this tool has a tool holder attached to it

Create a tool from a Global Library Create a tool Manually

We will now create a tool manually. Select ‘Create Tool Manually’

Edit a Selected Tool Delete the Selected Tool Change the Tool Position Manually

Select ‘Mill’ and ‘OK’

Automatically Assign Tool Number Display Selected Tool Details

The icons in the ‘Pos.’ column indicate how the tool was created and it’s usage status. See the description below: -

The different icons here indicate a tools current usage and how it was created. You can also see if a tool holder has been attached to the tool.

A green cylinder This means that this tool comes from the global library. A white cylinder This means that this tool comes from the local library A green hand This means that this tool has been defined manually in the local library A white hand This means that this tool has been added and it was not selected from any library

Open up the ‘Subtype’ and select ‘Ball nose’

Enter ‘7’ in the Diameter (D) box and then select the Tool Parameters, ‘Enhanced Editing’ flag.

Diameter (D) - This is the main diameter of the tool. 2nd diameter (d) – This is a second diameter setting, and is only active on certain tool types. It relates to the diameter (d) on the tool image. Tip Angle – This is the angle of the cutter on milling tools (where applicable) and the angle of the tip on drilling tool. Corner Radius – This is the corner radius of the tool. It is dependent on the type of tool selected and is only active on bull nose, ball Conic and corner rounding tools. Tool Length – This value applies to the overall length of the tool

The various flags and options are explained below. Usable Length – This value applies to the overall cutting length of the tool. General Parameters Form Num. of Teeth – This is the number of teeth, inserts or number of flutes for the tool. Tool Rotation – This is the direction the tool is rotating for normal cutting. Coolant – This is the type of coolant that will automatically be turned on when this tool is used. Tool Position – This is the tool number or carousel position. It can be set manually, left un-set by entering a question mark or set automatically.

Cutting Parameters Form

Lock database tool settings This flag is for unlocking the link to an external database. If the tool has been selected from an external database then we can unlock the link to the database by de-selecting this flag and then all the parameters of that tool then become editable. Database type – This is the name of the database from where the tool has been selected. If the box says ‘NONE’ then there is no link to any database and the tool has been created manually. Database reference code 1 and 2 – These are internal codes of the tool and do not affect the machining in any way. During the creation of a tool, text can be entered here to help identify the tool e.g. Tool supplier or meaningful reference code. Subtype – This is where you select the specific sub-type of tool. For example, an end mill and a ball nose are both sub-types of a milling tool whilst a centre drill and a flatbottomed drill are both sub-types of a drill. Tool Parameters Enhanced Editing – When this flag is active, more options are available for the user to define the tool.

Materials Tool/Insert Material and Piece Materiel – Here the type of material can be defined and must be used in conjunction with the correct type of piece material. When selected the correct speeds and feeds for the selected tool and material will be selected and input into the Cutting Conditions form and the Feed Speeds dialogue boxes *.

Cut Mode – This is the type of cutting the selected tool is actually doing and the relevant cutting conditions will be entered into the Cutting Conditions form and the Feed Speeds dialogue boxes *.

Cutting Conditions – This is where we can directly enter the cutting conditions for this tool. The Vc[m/min] is the cutting speed of the tool in Metres per minute and Fz[mm] is the feed of the tool in mm per tooth. If we have access to this information (from a cutting tool catalogue for example), then we can compute the correct feed and speed by entering the ‘metres per minute’ and ‘feed per tooth’ then clicking on the Compute feed speeds icon (shown below): -

Feed Speeds – This is the actual spindle speed in revolutions per minute S[rpm] and the cutting feed in mm per minute F[mm/min]. Cutting Parameters Step Over – This is the default step over of the tool. Step Down – This is the default step down of the tool. Safety Distance – This the safe distance of the tool above the top of the workpiece. Length and Diameter Corr – These values represent and length and diameter compensation numbers that are applied to the tool and will only be seen in the post processed output. Normally these are left blank, as the post-processor will use the tool station number for these values instead.

Select ‘OK’ and ‘OK’

*NOTE To cover all combinations of speeds, feeds, cutting material and piece material, Visitools will need to be used to input the correct information into the relevant databases. This is further than the scope of this document and, suffices to say, most customers ‘bracket’ the speeds and feeds entered here for other materials. Enter the following information into the ‘General Parameters’ form and the ‘Cutting Parameters’ form.

We have now created two tools within our new library and this demonstrates the process needed to create a complete new local library. We have illustrated how to create a tool from the global library and manually creating a tool.

Using the information you have been given, continue to enter a few more new tools into our Bridgeport library. Make sure you try different types. Try to create tools that are relevant to your workplace. Finally, once you have finished adding tools to your new tool library, we need to link the new library to the Bridgeport machine we created earlier. If any of the local library manager panels are on screen, click ‘OK’ to close them. Select Machining > NC-machines manager Highlight ‘Bridgeport’ then click ‘Edit NC machine configuration’

Edit machine configuration icon

Highlight ‘Bridgeport’ from the ‘Default local library’ drop down selector box then click ‘OK’ on both panels

Default local library selector box

This has linked the Bridgeport tool library to the Bridgeport machine configuration. Now, if the Bridgeport machine is selected when creating tool paths, the new tool library and post-processor will be used automatically.

This concludes the tutorial on Tool Libraries and Machine configuration

Welcome to VISI-Machining In this training documentation, the first type of toolpath (Roughing Spiral- Cavity) will be explained in detail, while all subsequent toolpaths will be explained in more general context. Once you have created the first toolpath, you will notice that the dialog boxes remain consistent for all toolpaths, which considerably reduces the learning process.

3DCAMRoughing

Agenda: Roughing Roughing Spiral Rest Roughing Spiral Roughing Against a Stock Model Roughing Spiral – Cavity Pre Drilled Point Roughing Spiral - Core Roughing Zig-Zag Roughing – Checking Collisions

Let’s create our first Roughing Spiral strategy.

Roughing Roughing Spiral - Cavity

Click the New Operation icon to create a new strategy.

Open the file “Cavity-123.wkf” From the following dialogue window select the Roughing Spiral strategy and then pick ‘OK’ to confirm this.

Once the model is loaded into the software we can begin to define the various cutting strategies required to manufacture the part. The first strategy we will apply will be a Roughing Spiral cut which will clear the bulk of the material away. To do this we need to begin by opening the Operation Manager, this is the place where the entire project can be managed and organized. Go to the menu Machining > Operation Manager to start up the operation manager.

You should now see the operations manager appear on the right hand side of the screen containing an empty project.

Now create a tool appropriate for roughing out this job. Click the Create Tool Manually icon to create a new tool. Choose the tool type Mill from the next dialogue box.

From the “General Parameters” page create a “Bull Nose” tool subtype using the parameters shown on the dialogue box below. The parameters you will need to adjust are ringed.

Info: - The Enhanced editing switch allows access to the extra tooling parameters that are otherwise frozen if this box is not checked. Automatic numbering allows the system to allocate a tool position in the library normally in the first available position. It is possible to have 2 tools with the same position no. if one has been created manually and one has come from Global tool library.

Now switch to the “Cutting Parameters” page to assign some default Speeds and Feeds for this tool. Click on the tab as shown

Assign the feeds and speeds using the parameters shown on the dialogue box below. The parameters you will need to adjust are ringed.

Info: - Clicking the Cut Mode button to “Rough” allows the entry of Roughing Speeds and Feeds. Here we use the “Feeds speeds” input to manually assign our values. icon to assign Click the “Set tool defaults” defaults for the Cutting parameters such as Step Over, Step Down and Safety Distance.

Finally let’s assign a “Tool Holder” for this tool. We will select one of the default holders from the library that comes as standard with the software. Click on the “Tool Holder Parameters” tab as shown below.

Select a holder from the standard library. From the list of Available holders select the ISO50 type and then select ‘OK’ to confirm the choice. Click the Holders Database icon to pick a holder from the default library.

Selecting the Machining Geometry Immediately after confirming the Toolholder parameters it is now required to select the model for machining. Using the standard VISI controls pick the model from the screen area. The Edit Model geometry dialogue will appear. A fuller description of the Piece Manager, detailing its features and function can be found in the document “Piece Definition”. Please ask your tutor if you do not have a copy of this document. All we need to do here is click on the green tick

The resulting dialogue box will now display the tool and holder together. Give the Assembly Description a name and select ‘OK’ to continue.

Info: -We are in fact creating a Triangulated mesh representation of the model for machining purposes. These values represent the accuracy of the mesh. The values here (0.1 and 10) are perfect for a Roughing Model. Now we have decided the cutting strategy and tool, we have to set the relevant machining operation parameters for this tool path. Your Operation manager should now look like this and contains a default machine tool, the origin for the toolpath, the tool and a cutting strategy (Roughing Spiral).

Double Click with the Left Mouse button on the Roughing Spiral strategy to access the cutting parameters.

Setting Up the Machining Strategy The dialog box will appear, and will have 7 different tabs, each containing different parameters which control the toolpath. The first tab “Machining”, represents all the fundamental parameters for the cutting strategy. Use the values shown below in the Dialogue Box.

Step Over Adjust This flag will only become active when bull nose tools are used for roughing. When the flag is active the step over is adjusted to always compensate for any extra material left on planar areas because of the step over used and the size of the radius used. Corners management Smooth corners: This option optimises the toolpath for high speed machining (H.S.M). For this type of machining it is necessary to remove any sharp corners in the toolpath allowing the tool to run at a higher feedrate and reduce cutter wear. Activating this option will add radii to all sharp corners within the toolpath. Max radius: This value represents the maximum radii value that can be added to the corner of the toolpath. Profile tolerance: Each Z level consists of a contour profile (where the piece is cut) and a set of concentric offset profiles. The profile tolerance controls the amount of smoothing to add to the corners when machining a profile. The value is the maximum distance that the smoothed profile will diverge from the actual contour profile.

Offset tolerance: The value is the maximum distance that the smoothed profile offset will diverge from the inner (offset) profiles. In essence, this parameter is identical to the Profile Tolerance, except that it refers only to the inner (offset) profiles and not to the outer profile.

Smooth stepover: This option optimises the toolpath for high speed machining (H.S.M). For this type of machining it is necessary to remove any sharp corners in the toolpath allowing the tool to run at a higher feedrate and reduce cutter wear. Activating this option will add an S-shaped transitional movement between each step across.

What’s happening here? An explanation of the Parameters in use on this page. Stock Oversize 0.5 mm This means that we are leaving 0.5mm of material on sidewalls of the component for finishing. Step Down 2mm This is the size of step between each Z level of the toolpath. Step Over This is the distance between the passes on each level of the toolpath and can be set to a percentage of the tool diameter or entered directly. Here we are using 40 percent of the tool diameter to define the step over distance.

Now we can move on to the Approach / Retract page. Click the tab to open this dialogue panel.

Approach / Retract Settings The approach and retract settings will dictate how the cutter will move onto and off the machined piece. There are many parameters that have subtle effects on the approach and retract type, most of which are set to sensible values based on the cutter geometry. Please reproduce the settings shown below.

Ramp/helix angle: The angle that the tool will move down into the material, in our case we are ramping using a 2 degree angle. Ramp min. diameter: A toolpath which would produce ramps smaller than this size (diameter span) will not be processed in our case we will eliminate any toolpaths that are below 66mm span. Vertical movements Approach: This is the size of a (vertical) radial movement added to the top of the approach ramp. Retract: This is the size of the (vertical) radial movement in the retract move. Horizontal movements Approach: This is the size of the horizontal component in the approach ramp. Retract: This is the size of the horizontal component in the retract move. Retract angle: This is the angle of the retract move. Plunge Area: The plunge area allows the user to input a physical X, Y value to force an area at where the toolpath should approach the part. If for example, the roughing strategy was being applied to a multi cavity block. Selecting an area close to one cavity would force the toolpath to start inside that cavity. It is also possible to select a point using the pick starting area icon. Fitting options Choose how the lead in and lead out arcs of the retract movements fit to the machining pass.

This dialog contains the following information: What’s happening here? An explanation of the Parameters in use on this page. Plunge mode = Ramp: If selected, the approach will follow the contour of the part as it ramps down to the next Z level. When this option is selected a ramp angle is required for computation. Ramp/helix height/offset: 3mm The ramp height offset is an extra height used in the ramping motion. It ensures the tool has fully slowed down from rapid speed before touching the material so that it enters the material smoothly at the ramping angle and ramping federate, here we are using a value of 3mm.

Machine all of pass: The path of the cutter will match the surface, including vertical surfaces and the corners. An arc will only be inserted at the end of the pass, and then only if it can be done so safely without hitting the job. Minimise trimming: In use here. The path of the retract will be as close to the surface as possible, maintaining a minimum distance from the surface to fit the arc of the set radius. Fully trim pass: In cases where it is crucial to prevent over-machining, this is a good and cautious strategy modification. The pass is trimmed back so the entire arc fits into it, but no nearer than a full machine pass link would be. Maximum trimming distance: The size of the pass trimming can be no greater than this distance. All of the values on the Approach/Retract tab are set to sensible default values based on the tool, strategy, depth of cut etc. Normally, it is not necessary to alter these values.

Transitions

In our example we are using the method By Depth, although due to the shape of the part either method would probably yield similar results.

Here we can set various parameters that control specific aspects of the tool Step Down and lift off. Click the “Transitions” tab to open this dialogue panel and reproduce the parameters as shown.

Min. Step over without Lift Off: This value allows the user to specify the maximum distance between two different passes where the system is allowed to create a connecting feed movement. If this value is set to zero, all the connecting movements will be executed in rapid mode at the rapid height. Small pockets management: This is a very important option when trying to avoid small pockets not to be machined. This function can be used to avoid the tool machining down into pockets that are only a little larger than the tool diameter. This can be used to preserve the tool life as it prevents the tool making small ramping moves and ‘bottoming out’. It is also linked to the ‘Ramp min. diameter’ function. Boundary What’s happening here? An explanation of the Parameters in use on this page. Step Down Management

The step down management allows the user to control the Z step down for the roughing strategy. In our example we are using :Constant: The system will remove the stock material using the fixed Z step down value of 2mm in our case. Using this method, any planar areas that fall between two levels will not be machined. Transition method: Using this option the user can decide if cutting multiple pockets, whether each pocket should be cut sequentially, or if thin walls are present, cut them level-by-level.

The Boundary page allows us to fine tune how the toolpath is constrained to any selected boundaries and also controls the Z start / end depth limits within the toolpath. Now we can move on to the Boundary page. Click the tab to open this dialogue panel.

On the “Boundary” page reproduce the parameters as shown below. Most of the values will be fine as default, the only one to change is highlighted.

Batch Build the Roughing Spiral toolpath Toolpaths can be calculated in 2 ways. They can be processed automatically when exiting from the machining parameters tabbed dialogue box, or alternatively they can be calculated using the “Batch Build” technique. This in theory allows a user to stack several un processed toolpaths in the operations manager and batch calculate them in one hit. In our case we only have one toolpath so far but can still calculate it with the batch build technique. Highlight the Roughing Spiral strategy inside the operation manager and click the batch process icon as detailed in the image below. Click with the Left Mouse button on the batch process icon to begin processing the toolpath..

Make sure the Roughing Spiral is selected in the Operation Manager.

Now that the toolpath has been calculated lets display it on the screen, this can be done from the operation manager. Click next to the Roughing Spiral strategy to display the toolpath. A red tick will appear. Next we will calculate the toolpath P.T.O The resulting toolpath.

Now we have a toolpath displayed on the screen the cutter can be animated to show the tool movement at each Z level.

Roughing Rest Roughing Spiral

From the Operation Manager click the Toolpath Simulated Display toolpath. In this example we will continue with the previous model which should now have 1 roughing cut applied to it.

Click the Toolpath Simulated Dislpay icon to animate the toolpath.

Use the controls on the left side of the screen to control the various display properties of the toolpath. Click the Show Tool icon to show the tool moving on the screen.

Enable the Shaded Tool icon to show the tool in shaded representation. This icon will display all the Z level steps. These 2 icons show only the top or bottom levels respectively.

Rest roughing is done after at least 1 toolpath has already been created, the option for Rest Roughing will not appear in the New Operation list until this condition has been met. Rest Roughing removes the material left by the previous cutter, and can be repeated several times with different size cutters. Although similar to finish rest machining, Rest Roughing recognizes large amounts of material that still remain and adjusts the passes accordingly in order to plunge safely into material, and approach safely from outside the material. You will get different results, depending on what values you enter. Now create a new Rest Roughing Spiral strategy. Click the New Operation icon to create a new strategy.

These 2 icons allow the stepping up and down through each Z level. From the following dialogue window select the Roughing Spiral strategy and then pick ‘OK’ to confirm this. The image to the right shows the tool displayed using the icon to step down the Z levels.

In this example, use a 20mm diameter cutter with a 5mm corner radius. Enter the cutter parameters as shown in the dialogue below. Note: - If you are unsure how to access the cutter parameters please refer to the Roughing tutorial or the Tool Libraries guide.

Let’s edit the parameters for this toolpath by double clicking on the Rest Roughing Spiral strategy in the operation manager.

Double click here to access the parameters for this strategy.

Enter the parameters shown on the Machining tab in particular adjust the Stock oversize and the Step Down.

Add some default feeds and speeds from the “Cutting parameters page” and set the tool defaults. An example is shown below.

Now click onto the Remachining tab, this is one of the most important pages for this strategy as this is the place where the user can reference previously calculated roughing toolpaths.

The system will now create a stock model (not seen by the user) based on the reference toolpath(s). The Rest Area passes will be based on a comparison between the actual model and the stock model. From the remachining tab there are several parameters that will effect the quality of the stock model and toolpath behaviour. Tolerance: The amount the cutter can move above or below the surface. The smaller the value the more accurate the calculation.

Click the Reference Operations icon to begin to add the roughing cut to reference against. Select the previous roughing cut as the reference operation, this should be the only one available.

Resolution: This is the granularity of the calculation - the smaller the value, the finer the detail, but the calculation is slower. Using a larger resolution will decrease detection time, but may lead to very small features being missed. Stock offset: This is an extra thickness that can be temporarily applied to the cutter and can be set when editing passes using a stock model. Use of the Stock Offset parameter can help to create better-trimmed passes. A negative value will cause the system only to select passes that are below the surfaces of a stock model by the specified amount, while a positive value will select all passes that are within the specified distance from the surfaces of a stock model.

Click the transfer button to pass the Roughing Spiral cut to the right hand column so it can be referenced.

Before confirming the machining parameters go to the Boundary tab and make sure ‘Use defined boundary’ is checked.

Select OK to confirm the choice of the Roughing Spiral strategy. The reference operations box should now be displaying 1 to indicate only 1 item is being referenced.

The resulting toolpath will now only attempt to machine areas left over from the previous referenced operation.

Roughing Against a 3D Stock Model

In this example, Select ‘T5 – 26mm R5 Bull Nose’ from the available cutters list as shown below.

The process of roughing against a stock model is very necessary when machining castings. More than often the casting model needs to be machined down to a finished component size. To avoid excessive cuts and moves when roughing away the casting it is important to be able to reference the actual rough casting model as a stock model rather than roughing to a generic bounding profile. Open the file pump.wkf Now create a new Roughing Spiral strategy. Click the New Operation icon to create a new strategy.

From the following dialogue window select the Roughing Spiral strategy and then pick ‘OK’ to confirm this.

Make sure that you have filtered the Mesh selection so that the stock mesh(casting) cannot be picked from the screen. Now pick the purple solid model as the machining piece. Disable the mesh filter and then pick the purple solid for the machining piece.

Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.1 for a Roughing type of cutting Strategy.

Now add the geometry using the same dialogue window. Click on the Add Geometry icon to begin the selection of the geometry from the screen. Note: - It is possible to select Meshes, Solids and Surfaces when using the By Solid stock definition.

Adding the Stock Model Now we need to select the Roughing Stock model to limit our roughing cuts against. Look at the operation manager and double click on the Stock Geometry item nested under the Roughing Spiral strategy.

Double click the Stock Geometry item to begin adding the casting model.

The Stock offset determines the material to be removed or retained from the surfaces of the stock. The same value is also used for the machining of semi-finished components (typical of die casting), when the "stock offset" value is set. Select the mesh model from the screen as the stock model item. Make sure that you filter only the Mesh when picking the geometry from the screen to avoid picking the solid model. Enable the mesh filter and then pick the grey mesh for the stock model.

From the next dialogue window make sure you use the drop down window to select the correct geometry stock type. Click on the drop down arrow to select stock type and select the option By Solid

The strategy should now contain 1 Model and 1 Stock model as shown below.

Let’s edit the parameters for this toolpath by double clicking on the Roughing Spiral strategy in the operation manager.

Double click here to access the parameters for this strategy.

Now click on the Approach / Retract tab and use a plunging type of approach.

Now calculate the toolpath by clicking OK from the dialogue box. The calculation takes a little longer when trimming back to a stock model. As you can see the toolpath is now trimmed back to the stock model the down side of this kind of process is that there are more rapid moves introduced into the toolpath.

Enter the parameters on the machining as shown below, the values that need to be changed have been highlighted.

Trimmed toolpath with rapid moves shown.

Trimmed toolpath with rapid moves hidden for clarity.

Roughing Roughing Spiral - Predrilled point

Enter the parameters of the Roughing Spiral toolpath and go to the Approach / Retract tab. Click on the Use Drill Points checkbox to enable the selection of drill points, and then press the selection icon as indicated below.

To prevent a cutter from plunging into hard material at a given point sometimes it is preferable to have the cutter enter into a hole that has previously been created by a drill. The roughing strategies in VISI-Machining allow us to do this by specifying pre-drilled points. Open the file Rcavity-predrilled.wkf The file already contains a Roughing Spiral toolpath where the system has calculated the current plunge point. Switch on the toolpath display using the operations manager to see the current toolpath.

Click here to begin the selection of drill points from the screen graphics area.

Also note that the Helix ramping parameters are disabled once we use the drill points option.

Select the drill point as indicated in the image below. Select this point as the pre drill entry point.

Click here beside the Roughing Spiral strategy to enable the red ‘tick’. This will display the toolpath in the graphics area.

Click OK from the Add / remove points dialogue box

Also from the Approach / Retract tab make sure the plunge co-ordinates are closer to the drilled entry point to avoid making the cutter have to travel a long way across from the drill point to the plunge co-ordinate area. This move is performed as a cutting feed move and would mean the cutter traveling across the job whilst cutting at full width.

Open the file multiple drill points.wkf

Using what you have learned from the previous example open the machining parameters for the toolpath that already exists and add the 6 points for each cavity.

This co-ordinate represents the centre of the machined piece adjust your values to suit. Now recalculate the toolpath using either Auto Rebuild from the machining tab form or Batch Build from the operation manager. The image below shows the cutter now vertically approaching the preset drilling point.

This diagonal move represents the cutter travelling from the pre drill position to the plunge co-ordinate influenced start point.

Note: - It is not possible to use a Plunge Point that is outside of the model geometry. USING MULTIPLE DRILL POINTS In the previous example only one drill point was used as a pre drilled entry point. However if your file contains multiple cavities, each requiring the tool to enter at a specified drill point then more than one point can be picked.

Remember, the Plunge area coordinates dictate which pocket the tool will start in first and ultimately the machining order.

Roughing Roughing Spiral - Core Core roughing is almost identical to Cavity roughing, except for a couple of toggle switches that need to be checked, in order to get the result we are looking for. As the name suggests this type of roughing strategy is suited to Core types of model geometry where the tool will machine the part from the outside to the inside.

Now create a tool appropriate for roughing out this job. In this example, use a 30mm End Mill cutter. Enter the cutter parameters as shown in the dialogue below. Note: - If you are unsure how to access the cutter parameters please refer to the Roughing tutorial or the Tool Libraries guide.

Open the file core-roughing.wkf Now create a new Roughing Spiral strategy. Click the New Operation icon to create a new strategy.

From the following dialogue window select the Roughing Spiral strategy and then pick ‘OK’ to confirm this. Add some default feeds and speeds from the “Cutting parameters page” and set the tool defaults. An example is shown below, you can enter feeds ands speeds that you feel appropriate.

Now select the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.1 for a Roughing type of cutting Strategy.

Enter the parameters on the Machining tab as shown below. The important area to note on this form is the Core Management area. Make sure that the Detect core areas is flagged.

Let’s edit the parameters for this toolpath by double clicking on the Roughing Spiral strategy in the operation manager.

Horizontal link clearance

Double click here to access the parameters for this strategy.

For core roughing, the cutter enters the materially horizontally from outside the part. This parameter defines the distance outside the part from which the cutter will start. Note that this parameter is only active if detect core areas is switched on. Now switch to the Boundary tab and make sure the box is checked for the parameter Use defined boundary. This will ensure that the toolpaths will be constrained to the X and Y bounding box for the part.

Select OK to calculate the toolpath and then run the toolpath simulated display from the operation manager.

Points to NOTE about Core Roughing The very first Z level is the only level at which the user can influence the entry point for the cutter. The parameter that effects this position is shown below. Go to the Approach / Retract tab and look at the Plunge area coordinates.

Use this icon to pick an area for plunging. Here is the full Core Roughing Toolpath result.

Now use the simulated display to check the result. Click the Toolpath Simulated Display to animate the cutter at each level. Select the icons shown below.

It must be stated that this coordinate is not an EXACT coordinate point but is used to define the general area of the plunge, the software will then dictate the exact position of the plunge.

Here is the plunge point on the 1st level of our example, influenced by the plunge area coordinates 0, 106.

On subsequent Z levels of the toolpath the system will pick the entry points and these points should always be from outside of the part. Try experimenting with the Plunge Area Coordinate to see how it influences the position of the tool. Tool approaches from outside of the part and works inwards to wards the core form.

Roughing

In this example, Select ‘T5 – 26mm R5 Bull Nose’ from the available cutters list as shown below.

Roughing Zig-Zag Zig-Zag roughing is an effective strategy for cutting softer materials such as aluminium, graphite, copper and various types of modeling board. It is also a very good strategy to employ if the machine tool being used cannot process too many circular movements as this strategy has a lot of liner point to point movements and fewer arcs. Open the file Zig-Zag-Rough.wkf Start the Operation Manager and begin by adding a Constant Z toolpath. Machining > Operation Manager Select the “New Operation” menu to create the new operation.

Pick the New Operation “Roughing Zig-Zag”

Now select the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.1 for a roughing type of cutting Strategy.

Let’s edit the parameters for this toolpath by double clicking on the Roughing Zig-Zag machining strategy in the operation manager.

The Offset value represents the distance between the ZigZag path and the contouring passes within each level of the toolpath. This parameter is necessary to clean up the cusps left on the part after the Zig-Zag passes have removed the bulk of the material. The default value is [flat radius tool] * 0.45 for flat and bull nose cutters, while it is forced to equal zero on Ball tools. In our example(26 R5 tool) this equates to 8 x 0.45 = 3.6

Double click here to access the parameters for this strategy.

Now switch to the Boundary tab and make sure the box is checked for the parameter Use defined boundary. This will ensure that the toolpaths will be constrained to the X and Y bounding box for the part.

Enter the parameters on the Machining tab as shown.

Click OK to calculate the passes. The image below shows one Z level pass of Zig-Zag roughing. You can see in the images here, the effect of the offset parameter.

In this example we are using a Stock oversize of 0.5mm and a Step Down value of 5mm with a Step Over percentage of 45 percent.

Contour pass added around the model to clean up the cusps left from the Zig-Zag passes.

The Resulting Toolpath – The extra levels have been added where required.

Step Down Management - Auto So far all the roughing strategies have used a Constant Step down in the Z axis. The last thing we will change on this example is the type of step down used. Go back to the machining parameters and click on the Transitions tab. Change the values to represent those in the image below. Click the Auto button. Auto: - Using this option, the system will automatically add extra Z slicing levels in between the main roughing levels. These extra steps are part of the roughing operation and cannot be closer together than the value specified in the minimum step over. This method is very useful when the part being machined contains many shallow faces at different Z levels. Precision This value controls how accurately the system finds the appropriate Z height at where to insert a new Z level slice. Extra Pass This value relates to the maximum horizontal distance between two adjacent Z level slices. If the horizontal distance between the two Z level slices is greater than the specified value, an extra Z slice is added. Using this parameter you will be able to control how many extra slices are required on the ‘flatter’ areas to ensure a constant stock volume is left for secondary machining operations. The smaller the value for extra pass the more Z slices will be calculated by the system. Now rebuild the toolpath and check the results. If you zoom into the toolpath you can see that there have been extra levels introduced. P.T.O

Extra Z levels have been added into the toolpath where the conditions are met.

Roughing Checking Collisions

Double click on the Roughing Spiral strategy to access the machining parameters for this strategy. Go to the General tab and look at the ‘Consider Tool Holder’ parameter this needs to be checked to enable holder collision detection.

When creating a set of machining toolpaths it is critical to check that the selected tooling and holder assembly can machine the passes without collision. If you choose to make use of this functionality any collisions that are detected are automatically trimmed out from the areas the tool and holder cannot access. Open the file roughing with toolholder.wkf Open the Operation Manager and you will see a pre calculated toolpath.

Display the toolpath by enabling the Red Tick.

If you animate the toolpath using the ‘Toolpath Simulated Display’ and step down to the lower levels of the toolpath you can see a tool holder collision.

Important Info About Holder Clearance Holder clearance Defines the safety distance between the holder and the model geometry.

Tool holder shown gouging with workpiece.

The Roughing operation fully gouge checks the Tool holder against both the part model and the un-machined stock model. For Finishing paths please note that this value represents ONLY the distance between the holder and the model geometry. Any stock oversize is not considered. Therefore this value must always be larger than any stock oversize value.

Now rebuild the toolpath to see the effect of Toolholder collision checking.

Tool Presetting Length

With tool holder collision detection applied.

A second method of preventing a collision with the workpiece is to calculate the ideal length of tool required for currently applied toolpath. Again open the file Open the file roughing with toolholder.wkf From the previous example we already know that there will be a collision with the holder and workpiece, but we do not know how long the tool should be if we wanted to adjust the tool to a length that will cut the part without problems. Open the Operation Manager and you will see a pre calculated toolpath.

Toolpath has been trimmed away where there would be a collision between holder and the workpiece. No Tool holder collision detection applied.

Select the Roughing Spiral strategy from the operation manager.

Now click the Tool Length Check icon from the Operation manager Toolbar.

Toolpath has machined to the very bottom of the cavity which will introduce a collision.

Click the Tool Length check icon.

The tool length dialogue box will now appear.

If you now perform a tool path simulation you will see that the tool is now detached from the holder, this is because the presetting length has been adjusted (the amount the tool is out of the holder) but not the overall length of the tool. Details of the current tool.

This is the current length that the tool is protruding out the holder.

Notice that the Tool appears detached from the holder.

Represents a specified tolerance around the tool holder and tool shank which is taken into account when checking for collisions. No collision will be considered if the interference will be in this tolerance.

Leave the settings as shown in the image and now calculate a new presetting length. Click the Compute Presetting to begin the tool length optimisation.

Take a look at the prompt bar in the bottom left corner as it displays the amount of collisions detected during the calculation.

Notice that the Tool Presetting length has now been adjusted.

Now edit the Tool and make the total length suitable as shown below.

Take a look at the Tool holder parameters to check the tool and holder assembly, now everything seems to be in order.

After editing the tool select OK to confirm and select YES to update the operation parameters and cutting conditions.

Tool Holder now misses the part with the preset length of 100mm.

Welcome to VISI Machining 3D In this training documentation it is assumed that the user is familiar with the basic navigation of VISI Machining and the Operation Manager, so only parameters relative to the machining strategy will be explained in detail. Once you have created the first toolpath, you will notice that the dialog boxes remain consistent for the majority of the toolpaths, which considerably reduces the learning process.

Semi&Finish

What is Covered in this Chapter? Semi & Finishing Constant Z Parallel Plane Parallel Plane Cross Machining Planar Face Machining 3D Stepover Radial True Spiral Contour Projection Tracing 3D ISO Machining

Semi & Finishing Constant Z Open the file Waterline.wkf

In this example, use a 12mm diameter cutter with a 3.5mm corner radius. Enter the cutter parameters as shown in the dialogue below. Note: - If you are unsure how to access the cutter parameters please refer to the Roughing tutorial or the Tool Libraries guide.

Start the Operation Manager and begin by adding a Constant Z toolpath. Machining > Operation Manager Select the “New Operation” menu to create the new operation.

Pick the New Operation “Constant Z”

Add some default feeds and speeds from the “Cutting parameters page” and set the tool defaults. An example is shown below.

Now select the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.05 for a finishing type of cutting Strategy.

Enter the parameters on the Machining tab as shown below.

Let’s edit the parameters for this toolpath by double clicking on the Constant Z strategy in the operation manager.

Significant Parameters Used Here Double click here to access the parameters for this strategy. Notice that the dialog box is very similar to the ones used during roughing. This strategy is most effective on steeper surfaces. This is because the spaces between the passes are calculated from the stepdown value, and on surfaces where there is little z-level change, the spaces between the passes are greater and you may get unsatisfactory results. You can therefore limit the work area to surface angles between, for example, 40 and 90 degrees. Limit your passes to work within an angle range, to get the best results for the tool.

Stock Oversize: - We have set a value of zero here so the piece is finished to component size. Step Down: -Each Z level pass will be calculated at constant 0.5mm depth increments Machining Strategy Unidirectional: - The cutting strategy will be moving in one direction only as opposed to changing direction at the end of each pass. Step Over Mode Constant: - The passes will be calculated at a constant Z pitch of 0.5mm with no intermediate passes calculated. Auto Rebuild: - With this switched checked and when the ‘OK’ button is clicked the toolpaths will be calculated straight away. Now switch to the Boundary tab to change some of the machining limits.

Look at the parameters shown below and change those that are marked in the red box.

As you can see from your toolpath the Z steps stay a constant pitch all the way down the job and the motion is in one direction only. Parameters To Change. Let’s make some subtle changes to the toolpath by adjusting the parameters of the strategy. Ramping Between Levels Open the machining parameters again and go to the Transitions tab. In this instance we will make the tool ramp between each Z level to try and eliminate a constant witness line down the part. Adjust the parameters as shown below and select ‘OK’ to calculate the toolpath.

You can visibly see the ramping between each level around the part.

Tangential Link Min Z Level: - Here we have set the Z level for the passes to fall between 0 and 29, this ensures that the passes are calculated around the main form and do no machine around the outside of the part base and do not drop below a Z depth of 29. Without changing any other parameters click the ‘OK’ the first set of passes.

Try checking this option to see the difference between this and a standard ramping option. The ramp will blend in and out of each Z level with a smooth tangential motion.

button to calculate

Trim to ramp

Finally try checking this option and again compare the difference. You should see in areas where it is achievable , that Z level passes are trimmed back to meet the start and the end of the ramp transition. Ramp trimming occurs in this area and helps eliminate witness marks.

Constant Z with Adaptive Stepdown When using a Constant Z strategy with a constant step down on a part that is not completely steep or completely shallow, it is very likely that in the shallow areas there will be large gaps between passes. To combat this problem and create some intermediate passes we can use the “Stepover Mode” Adaptive. Open the file AdaptiveZ.wkf Looking at the passes already applied to the part it is clear to see that using the “Constant” step down method does create areas where the passes are widely spaced horizontally and would result in a poorer surface finish. Open the cutting parameters for this strategy and go to the Machining tab.

Go to the “Step Over Mode” drop down and switch it to Adaptive, this will open up 3 new parameter boxes, enter the values as shown below. Click OK to calculate.

Minimum Step Over: - This specifies the minimum stepdown value to be used for the in between passes, meaning passes will be no less than this distance from each other. Precision: - This controls how accurately the system finds the appropriate height to insert a new slice. Extra Pass: - This parameter relates to the maximum change in the surface profiles for two adjacent z-levels. Having calculated the surface profile at a given z-height the profile at the next z-value is provisionally calculated. The maximum value of the shortest horizontal distance between adjacent points on the two profiles is then calculated. If the change in profiles from one z-level to the next is greater than the Profile Step-in, then the provisional profile is discarded. An adjustment is then made to the z-level so that an extra profile is inserted. This process is repeated until a profile

that meets all requirements is found. The smaller the number here, the more likely extra passes will be found. Let’s look at the results in our example. As you can see extra passes have been inserted into the areas where there were previously large horizontal voids between each Z level. You can experiment with the 3 parameter values to obtain different results.

Constant Z with Drive Curve Another good solution for creating “intermediate” passes on parts that have a combination of steep and shallow areas is to use the Step Over Mode Drive Curve. Here is an example of how this option works. The information on the file for the boundaries and the drive curves has already been generated and the information needs to be present before the options can be used. Open the file “Multiple Curves no machining.wkf”

If you need assistance in generating these curves or profiles then please ask for assistance.

Pick the model and confirm

Generate a new machining operation using the “Constant Z” strategy using a “6mm Ball Nosed Tool”

Select the 3 yellow profiles as machining boundaries. If you are unsure how to do this please ask your tutor for more help.

SELECT THESE 3 PROFILES

Open the operation Parameters and change the “Step-Over Mode” to “Drive Curve”

The step on the curve is calculated as shown in the diagrams below: -

Constant Z step

Z levels using drive curve

The next step is to choose the drive curve/s Select the “Pick Drive Curves” icon.

NOTE Single or Multiple drive curves can be used for this option. Select the 3 blue curves highlighted below: -

Once the drive curve option is selected then the “Step on curve” becomes active and the “Step down” is now unavailable.

The “Step on curve” now relates to the step along the curve and not the step in Z, as is the default option.

The option of having the step along the curve allows greater control of the slices along the model and this is particularly useful for components that have a shallow angle.

SELECT THESE 3 CURVES

Select “OK” to accept the curves

Constant Z Helical The last option to investigate within the parameters of the Constant Z strategy is another Transition based parameter, Helical. Let’s see its effect with an example. Open the file Helical Machining.wkf

Activate the “Auto Rebuild” flag (Machining Tab) and switch on the option for the rapid management from the Boundary tab to “Safety Distance” and generate the toolpath. HINT!!!!

Start the Operation Manager and begin by adding a Constant Z toolpath. Machining > Operation Manager Select the “New Operation” menu to create the new operation.

The result will be as below with the Z levels adjusted to the drive curves, shown here with the Rapids hidden from the display.

Pick the New Operation “Constant Z”

In this example, Select ‘T3 – 6mm Ball Nose’ from the available cutters list as shown below.

Let’s edit the parameters for this toolpath by double clicking on the 2 Leading Curve Machining strategy in the operation manager.

Double click here to access the parameters for this strategy. Enter the parameters on the Machining tab as shown. Add a Step-down value of 1mm in the Stepdown box.

Now select the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.05 for a finishing type of cutting Strategy.

Now switch to the Transitions tab and focus on the Transition method parameters. Switch the Transition method option to Helicoidal as shown in the image. From the Boundary tab make sure that the Min Z Level values are set as shown below so that the toolpath will not fall over the edges of the main rectangular base area of the part, i.e we are restricting the Z limits to which the toolpath can be applied.

Constant Z Helical – Removing the toolpath “lifts”. As you can see from the image and the toolpath itself, where the part has a totally vertical wall the Helical transition can produce some anomalies. This can be solved by reducing the machining tolerance slightly. Go to the General tab and slacken off the machining tolerance to a value of 0.03 as shown below.

This should solve the problem and produce a better quality toolpath with out the small spikes.

Now click the OK button to calculate the toolpath. The result is shown below. The toopath motion should be totally Helical, in this case there is one approach and one retract move. This option ensures that there are no marks left on the part and if necessary will automatically switch to a normal Constant Z transition if a Helical transition cannot be achieved. There will also be a clean up pass applied on any flat areas of the part. Check out the very bottom pass on this part, this is a horizontal clean up pass. Note: - You will instantly notice some strange toolpath “lifts” at the near vertical area of the part. P.T.O for advice.

Semi & Finishing Parallel Plane

In this example, use a 12mm Ball Nose diameter cutter. Enter the cutter parameters as shown in the dialogue below. Note: - If you are unsure how to access the cutter parameters please refer to the Roughing tutorial or the Tool Libraries guide.

Open the file raster.wkf

Start the Operation Manager and begin by adding a Parallel Plane toolpath. Machining > Operation Manager Select the “New Operation” menu to create the new operation.

Pick the New Operation “Parallel Plane”

Add some default feeds and speeds from the “Cutting parameters page” and set the tool defaults. An example is shown below.

Now select the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.05 for a finishing type of cutting Strategy.

Enter the parameters on the Machining tab as shown below and select ‘OK’ to calculate a basic toolpath. Later other options will be changed to see the differences.

Let’s edit the parameters for this toolpath by double clicking on the Parallel Plane strategy in the operation manager.

Significant Parameters Used Double click here to access the parameters for this strategy.

Raster Passes are spaced perpendicularly to the tool axis. Consequently, this machining strategy is most effective on shallow (nearing horizontal) surfaces. The zheight of each point along a raster pass is the same as the z-height of the triangulated surfaces, with adjustments made for applied thickness and cutter definition.

Stock Oversize: - We have set a value of zero here so the piece is finished to component size. Step over: -Each pass will be calculated at a constant horizontal pitch of 0.5mm between each pass. Machining Strategy Zig-Zag: - The cutting strategy will be move the cutter in two directions changing direction at the end of each pass, moving back and forth across the piece. Stroke Angle: - The passes will be calculated at 45 degrees across the job, this is sometimes good way of ensuring a better overall finish where surfaces may be otherwise parallel to the machining direction e.g zero degrees. Auto Rebuild: - With this switched checked and when the ‘OK’ button is clicked the toolpaths will be calculated straight away.

Let’s look at the results in our example. As you can see, passes have been calculated at the desired pitch moving back and forth across the job at a 45 degree angle.

Parameters To Change. Let’s make some subtle changes to the toolpath by adjusting the parameters of the strategy. Go to the Machining tab and switch the direction to Unidirectional and click OK to calculate the passes.

Zoom into the top left or bottom right corner of the job and you will notice that there is a strange ZIG ZAG movement in a small portion of the toolpath. To remedy this undesirable movement we need to tweak another parameter. Go to the Transitions tab and look at the parameter “Min.Step-over without lift off”. Currently set at a value of 12mm. This value sets the minimum acceptable toolpath length before the tool will lift off the job. In this case the length of the passes in these areas falls below the 12mm limit. Look at the dialogue below and change the value as shown. Click ‘OK’ to calculate the toolpath.

Once calculated the toolpath should now lift off from the job at the end of each pass as shown in the image. The value of 0 ensures that this will happen in all areas where there a small pass lengths. Note: - The rapids have been hidden to help clarify the image.

Parallel Plane – Pass Extension One very useful feature inside the parallel plane strategy is the ability to extend the toolpaths beyond the limits of the machined piece without the need to provide run off surfaces. Now note that each toolpath lifts of at the end of each pass to maintain motion in one direction.

Open the file pass extension.wkf

Add a new Paralell Plane toolpath to the project in the operation manager and select a tool from the existing default library. Choose T4 – 10mm Ball Nose cutter.

On the Machining tab enter the basic parameters a shown below, adjusting the Step Over and the Stroke angle values as indicated.

From within the Operation Manager enter the machining parameters for the strategy. From the Transitions tab change the Pass Extension value so that the toolpath will be extended beyond the boundary. Next, move to the Boundary tab to constrain the toolpath to the XY bounding rectangle of the piece.

Double click here to access the parameters for this strategy.

Take a look at the result of the standard pass extension, as you can see the passes are extended but will start to drop down the sides of the part as the toolpath is extended.

Semi & Finishing Ÿ Parallel Plane Cross Machining

To see an alternative result, try using the Tangential option. Go back to the Transitions tab change the Pass Extension value so that the toolpath will be extended further.

This strategy builds on a set of existing Parallel Plane passes. It creates a new set of passes at right angles to the original set. The new passes can be used to machine gaps left in the original passes, e.g. where the surfaces and the passes were approximately parallel.

The toolpath now extends beyond the machined piece but this time the extension is tangent to the surfaces.

Click OK to calculate the toolpath with the new extension Parameters.

Open the file cross-raster.wkf

Start the Operation Manager and begin by adding a Parallel Plane toolpath. Machining > Operation Manager Select the “New Operation” menu to create the new operation.

Pick the New Operation “Parallel Plane”

In this example, Select ‘T3 – 6mm Ball Nose’ from the available cutters list as shown below.

Next add a restriction boundary to the strategy to stop the tool rolling over the edges of the part. From the lower split panel in the Operations manager double click on the Boundary List item nested under the Parallel Plane strategy. Double click the Boundary list item to add a restriction boundary to the part.

Now pick the boundary from the screen as shown in the image below. Select the Profile boundary from the screen

Now select the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.05 for a finishing type of cutting Strategy.

The profile should now be added as a Cut Boundary under the Boundary list item.

Profile has now been added as a cut boundary.

Let’s edit the parameters for this toolpath by double clicking on the Parallel Plane strategy in the operation manager.

Cross Machining Passes. Go to the Machining tab and focus on the Cross Machining part of the form. Change the option from “None” to “Standard” and click OK to calculate the passes.

Double click here to access the parameters for this strategy. First let’s create a standard Parallel Plane toolpath on the part. Go to the Machining tab and adjust the parameters as shown.

If we Zoom in to the same corner again you will notice that there are now extra passes perpendicular to the original passes where the spacing of the tool path was sparse. What do the options mean ? Please try changing the options to see the results!

Here we will use a Step Over of 1mm and a Stroke angle of 45 degrees, select OK to calculate the basic passes. Zoom into the corner of the part and take note that the passes a quite sparsely spaced as the toolpath becomes almost parallel with the machined surfaces.

The regular Parallel Plane passes are calculated, and then the Cross Machining passes are added at the end of the strategy.

The cross machining passes are calculated before the original Parallel Plane passes.

Only the Cross machining passes are calculated. (See image)

Let’s edit the toolpath to apply some cross machining passes and see how they can help this situation.

Semi & Finishing Planar Face Machining

In this example, use a 30mm diameter End Mill type cutter. Enter the cutter parameters as shown in the dialogue below. Note: - If you are unsure how to access the cutter parameters please refer to the Roughing tutorial or the Tool Libraries guide.

When you select Horizontal Area Passes, VISI Machining will find all the flat areas of the geometry and put passes at the z-level of each area. Horizontal Area Passes act only upon completely flat areas – if a surface has even a small gradient, it will not be detected. However, you can use Axially Offset Passes with Horizontal Area Passes. Axially Offset Passes machine the same passes a number of times, offset along the tool axis. Open the file horizontal area.wkf

Start the Operation Manager and begin by adding a Planar Face Machining toolpath. Machining > Operation Manager Select the “New Operation” menu to create the new operation.

Pick the New Operation “Planar Face Machining” and select ‘OK’

Add some default feeds and speeds from the “Cutting parameters page” and set the tool defaults. An example is shown below.

Now select ALL the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.05 for a finishing type of cutting Strategy.

Here are the parameters for the Planar Face machining toolpath set in the Machining tab.

Let’s edit the parameters for this toolpath by double clicking on the Planar Face Machining strategy in the operation manager.

Significant Parameters Used Double click here to access the parameters for this strategy.

Enter the parameters on the Machining tab as shown on the next page and select ‘OK’ to calculate a basic toolpath.

Stock Oversize: - We have set a value of zero here so the flat areas are finished to component size. Step over range: -This is the range of the size of spaces between the passes, defined by the minimum and maximum value you set here. VISI Machining will pick the largest value possible within that range that does not leave unwanted upstands between the passes. You can lower the min and max range value to have narrower passes. Auto Rebuild: - With this switched checked and when the ‘OK’ button is clicked the toolpaths will be calculated straight away.

The result of the Planar Face Machining should be similar to the image shown below.

Open the file 2Leadingcurves.wkf

In fact there are not so many parameters that will influence this type of path so no further parameter changes will be discussed.

Start the Operation Manager and begin by adding a Parallel Plane toolpath. Machining > Operation Manager Select the “New Operation” menu to create the new operation.

Pick the New Operation “2 Leading Curves”

Semi & Finishing 2 Leading Curves 2 Leading Curve passes are passes that "flow" across the surface and are virtually parallel to each other, rather like raster passes, but the shape and direction of the passes are controlled by the boundaries around them. Each pass echoes the shape of the preceding one but also takes on some characteristics of the following pass, and so the paths "morph" or gradually change shape from one side of the boundary to the other. This machining strategy is most effective on areas that include shallow surfaces as the passes are spaced along the xy-plane (stepover), and not the z-plane (stepdown).

In this example, Select ‘T3 – 6mm Ball Nose’ from the available cutters list as shown below.

Using the ‘Block Control’ icon to pick the 2 Leading curves needed for the machining.

NOTE : Block control

It is also possible to depress the control (CTRL) key instead of using the ‘Block control’ icon.

Select the 2 curves starting with the curve on top of the radius and then the curve around the bottom of angled walls.

Pick this curve first

Now select the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.05 for a finishing type of cutting Strategy.

Pick this curve second

NOTE : The order in which you pick the curves is important, as this will determine the machining direction. The status of the curve is also very important when using this strategy. If the start and end points do not coincide on both curves and the curves do not travel in the same direction, then the toolpath will not give the required result. Some of the common problems will be described later.

Let’s edit the parameters for this toolpath by double clicking on the 2 Leading Curve Machining strategy in the operation manager.

Some Useful Tips to consider before calculating a 2 Leading Curve toolpath. Some common problems encountered with this strategy are shown below. All problems are due to the condition of the curve. I.e. Start points and direction.

Double click here to access the parameters for this strategy.

Both curves OK Start points OK, Curves in same direction Perpendicular flag in-active

Enter the parameters on the Machining tab as shown below and select ‘OK’ to calculate a basic toolpath. Later other options will be changed to see the differences.

Both curves OK Start points OK, Curves in same direction Perpendicular flag active

Both curves OK Start points OK, Curves in different direction Perpendicular flag active Many of the parameters on this dialogue are common to some of the strategies already used. Here we will explain parameters unique to this strategy.

Both curves OK Start points are different, Curves in different direction

Both curves OK Start points OK, Curves in different direction Perpendicular flag in-active

Both curves OK Start points are different, Curves in different direction

Both curves OK Start points are different, Curves in same direction Perpendicular flag in-active

Once all the options are set to obtain the correct result, select ‘OK’ to calculate the toolpath. Display the toolpath and see the results. Use the Display and Clear Toolpath icons to show the toolpath. The result will be as shown below.

Toolpath morphs from one curve to another and flows around the shape, parallel to the drive curves. Both curves OK Start points are different, Curves in same direction Perpendicular flag active

Investigating the options

We are now going to use the segments to synchronise the toolpath

Go to the Machining tab and activate the option Perpendicular mode.

Expand the option in the ‘Drive curve’ option from within the operations manager and double click on ‘Synchronisation Lines’

Perpendicular Mode With this option flagged the system will calculate the machining perpendicular to the 2 drive curves. The difference can be seen in the image opposite.

Toolpath morphs from one curve to another and but is now orientated perpendicular to the curves

Synchronisation Lines If we look at the toolpath from the plan view, you will see that the toolpath looks OK. However it is possible to improve the quality of the toolpath using ‘Synchronisation Lines’. Currently the toolpath between the upper and lower curves is moving diagonally to & from the points along the curve. This is shown below Gradual diagonal movement

Double Click the Synchronisation lines item under the drive curve node.

Now select the 8 segments. It does not matter what order these lines are selected.

Select the 8 lines Once selected use the right hand mouse button to ‘Confirm Selection’

After defining the synchronisation curves, you will notice the toolpath has turned purple within the operations manager. This means that something has changed and the toolpath needs to be re-calculated.

Click the Batch Build icon to recalculate the toolpath using the Synchronisation Lines. The operation is coloured purple to indicate modifications have taken place and recalculation is required.

Semi & Finishing 3D Stepover Constant Surface Stepover passes are 3D passes. The passes are at a constant distance from each other along the surface of the job (regardless of the direction). This is an ideal strategy to use on the boundaries generated by rest machining, or in any circumstances where you want to ensure a constant 3D distance between passes. Open the file constantstepover.wkf Start the Operation Manager and begin by adding a 3D Step Over toolpath. Machining > Operation Manager Select the “New Operation” menu to create the new operation.

Display the toolpath and see the results. Use the Display and Clear Toolpath icons to show the toolpath. Pick the New Operation “3D Step Over”

The toolpath is now constrained between the Syncronisation lines and flows around the corner in a more controlled manner.

In this example, Select ‘T4 – 10mm Ball Nose’ from the available cutters list as shown below.

Next add a restriction boundary to the strategy to stop the tool rolling over the edges of the part. From the lower split panel in the Operations manager double click on the Boundary List item nested under the Parallel Plane strategy. Double click the Boundary list item to add a restriction boundary to the part.

Now pick the boundary from the screen as shown in the image below. Select the “RED” Rectangular Profile boundary from the screen

Now select the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.05 for a finishing type of cutting Strategy.

The profile should now be added as a Cut Boundary under the Boundary list item. Profile has now been added as a cut boundary.

Let’s edit the parameters for this toolpath by double clicking on the 3D Step Over strategy in the operation manager.

Here we have adjusted only the Horizontal Step Over and the Vertical Step Over to 0.5mm respectively. Toolpath is stepping over at a constant pitch and follows the rectangular boundary shape.

Double click here to access the parameters for this strategy.

Enter the parameters on the Machining tab as shown below and select ‘OK’ to calculate a basic toolpath. Later other options will be changed to see the differences.

As you can see from the result, the toolpath maintains a constant 0.5 mm step over regardless of the contours on the machined piece. Also note that the shape of the toolpath follows the rectangular boundary shape. Inverting Step Over and Direction Continuing with the toolpath already created it is possible to edit the parameters and change the direction of the toolpath in several ways. To see this effect more clearly change the Machining Strategy from Zig-Zag to Uni Directional. Go to the Machining tab and change the setting, then re-calculate toolpath.

Animate the cutter motion using Toolpath Simulated Display

Cutter Direction, Anti Clockwise

Try calculating the remaining cutter direction / step over combinations from the Approach / Retract tab.

.The toolpath now icon maintains a constant direction and can clearly be seen moving Anti clockwise, from the inside of the part. You can also see the step over link moving downwards towards the bottom of the part. Step over direction, inside to out.

Cutter Direction, Clockwise

Step over direction, outside to inside. Click on the Approach / Retract tab and now adjust the following options, check the invert direction box, now recalculate the toolpath.

And finally the 4th combination

Step over direction, inside to out.

Cutter Direction, Anti-Clockwise Cutter Direction, Clockwise

Step over direction outside to inside.

Options to change the shape of the toolpath. Using Drive Boundaries Using the Operation manager it is possible to add a Drive boundary(s) to influence the shape of the toolpath but also place restrictions on the toolpath. Let’s see how this works.

Double click on the Drive Boundaries item to add a new Drive boundary.

Now select the Green Profile boundary as the Drive boundary definition. Click on the Green Profile Boundary item to add this as a new Drive boundary.

Recalculate the passes by clicking the Batch Build icon from the Operation Manager, it is not necessary to go back into the machining parameters. Click on the Batch Build icon to recalculate the toolpath.

Notice that the toolpath now follows the definition of the Drive boundary shape. Even though we still have the rectangular boundary selected as a cutting boundary, it is ignored because the Drive is inside of the Cutting boundary (limit boundary).

Here is another scenario using a combination of Limit and Drive boundaries that will control the shape of the toolpath. We will be using a different set of Limit Boundaries and Drive Boundaries. From the operation manager perform the following modifications:-

Double click on the Drive Boundaries item to add a new Drive boundary and select the Green profile.

Double click the Boundary list and then select the smallest yellow boundary in the centre.

Now recalculate the toolpath using the batch build icon from the operation manager. Click on the Batch Build icon to recalculate the toolpath.

The result of this Limit and Drive boundary combination can be clearly seen in the image below. The toolpath is now restricted to the Yellow limiting boundary but it is taking on the shape of the Drive boundary even though the Drive boundary is clearly outside of the cutting boundary.

Semi & Finishing Radial Radial passes converge on a central point. The stepover is calculated along the circumference of the circle of a radius you define. This machining strategy is most effective on areas that include shallow curved surfaces and circular areas as the passes are spaced along the xy-plane (stepover), and not the z-plane (stepdown). The z-height of each point along a radial pass is the same as the z-height of the triangulated surfaces, with adjustments made for applied thickness and cutter definition. Open the file radial.wkf Start the Operation Manager and begin by adding a Radial toolpath. Machining > Operation Manager Select the “New Operation” menu to create the new operation.

Pick the New Operation “Radial”

In this example, Select ‘T4 – 10mm Ball Nose’ from the available cutters list as shown below in the default library.

Let’s edit the parameters for this toolpath by double clicking on the Radial strategy in the operation manager.

Double click here to access the parameters for this strategy.

Enter the parameters on the Machining tab as shown below and click ‘OK’ to create a toolpath.

Now select the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.05 for a finishing type of cutting Strategy.

Significant Parameters For this Strategy

Take a look at the calculated toolpath. It looks a bit messy as some of the passes are creeping over the edge of the part.

Stepover Editing the Options The stepover is the spacing between the passes along the circumference of the circle. The maximum radius you set on this dialogue page defines the circle. The stepover is calculated from the blue line in the diagram - passes are evenly spaced by the amount that you set in the stepover field.

Centre You must specify the xy-position of the centre-point of your circle. The Radial passes will start or end at this centre-point. To help you to work out the coordinates, you can zoom in, and look at the position of your cursor from the xy information fields on the status bar and use the geometry picker to define the centre point.

To make the toolpath significantly tidier the end radius value can be adjusted so that the toolpath is limited from falling over the edge of the part. Open up the operation parameters and go to the Machining tab. Focus on the “Geometrical Definition” area of the form.

Angle The minimum and maximum angles act as limits to your passes. They control the angle span of the operation, that is, how much of a complete circle will be machined. Each radial pass starts at the centre point and ends at the circumference of your circle, unless changed in the radii field (below). Looking down your cutter axis (zview), a line with an angle of 0 is parallel to the x-axis, and a line with an angle of 90 degrees is parallel to the y-axis. An angle of 360 degrees is a full revolution around the circle, and the line is parallel with the x-axis. Any angle of a value in between 0 and 360 degrees will be a rotation pivoting anticlockwise from the centre point The minimum angle is the first radial pass to be created, and the maximum is the last radial pass to be created. A range of 0 to 360 will give the full circle, a range of 0 to 180 will give half of a circle, and so on

0° min, 90° max:

80° min, 200° max:

Click the Maximum radius button to enable picking from the screen.

Use the Quadrant point icon to pick the point on the model that defines the maximum radius.

Pick a Quadrant Point on this edge. The Maximum radius should measure 54 as shown below.

The toolpath should look like the one in the image shown here.

Semi & Finishing Spiral

If you display the toolpath simulation you can see that the tool starts in the centre of the job and the tool moves in an anti clock wise direction.

This machining strategy is most effective on areas that include shallow curved surfaces and circular areas as the passes are spaced along the xy-plane (stepover), and not the z-plane (stepdown).

Open the machining parameters again and go to the Approach/Retract tab.

Open the file spiral1.wkf

Click the Invert Step-over checkbox to machine the part in a clockwise direction. Invert direction is only in use if the toolpath motion is Unidirectional so will have no influence in this case.

Start the Operation Manager and begin by adding a Spiral toolpath. Machining > Operation Manager Select the “New Operation” menu to create the new operation.

Specify a Plunge area co-ordinates as shown below, this will enable the toolpath to start from outside of the cavity. Toolpath now moves clockwise and starts from the outside.

Pick the New Operation “Spiral”

In this example, Select ‘T3 – 6mm Ball Nose’ from the available cutters list as shown below in the default library.

Let’s edit the parameters for this toolpath by double clicking on the Spiral strategy in the operation manager.

Double click here to access the parameters for this strategy.

Enter the parameters on the Machining tab as shown below and click ‘OK’ to create a toolpath. Notice that the dialog box is very similar to the one used in creating radial passes. Fill in the parameters as shown and click OK.

Now select the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.05 for a finishing type of cutting Strategy.

We should now have a toolpath that machines to the exact outer edge of the part as shown below.

The result should look like this image: Significant Parameters used in this machining Strategy.

Here we can set the maximum radius to be considered by the spiral path. Editing the Parameters

Here we can set the centre point for the spiral toolpath. Value = 0, 0

If you look closely at the passes, the default settings have not rendered an optimal result. In this example we will alter two of the parameters in order to achieve a better result. The first parameter we must change is the maximum radius of the part. The system as a default uses the extents of the surfaces and places the value in the Radii dialog box.

In order to find the correct radius value to use, we will have to measure one on the part. Now in order to re-calculate our existing passes, we must re-generate them using this new value and a new contact angle. Click on the Spiral Passes 1, right click and select Properties. Select the pick point icon to allow picking of a point from the screen. Pick a Quadrant Point on this edge. The Maximum radius should measure 34.5 as shown below.

Semi & Finishing Contour Projection A Contour Projection pass is created by dropping the cutter onto the surface and running it along a single boundary or a set of boundaries to produce the effect of engraving. Open the file boundary.wkf

In this example, we will generate boundary passes on existing geometry. The curve geometry that exists in the file was generated in a CAD system, and is a typical example when doing cavity engraving. Start the Operation Manager and begin by adding a Contour Projection toolpath. Machining > Operation Manager Select the “New Operation” menu to create the new operation.

Pick the New Operation “Contour Projection” and select ‘OK’

Add some default feeds and speeds from the “Cutting parameters page” and set the tool defaults. An example is shown below.

In this example, use a 1mm diameter Ball Nose type cutter. Enter the cutter parameters as shown in the dialogue below. Note: - If you are unsure how to access the cutter parameters please refer to the Roughing tutorial or the Tool Libraries guide.

Now select ALL of the model from the screen area. Check that you are using similar values to those shown below for the triangulation of the model for machining purposes, the chordal tolerance is set at 0.05 for a finishing type of cutting Strategy.

Now select the projection Curves to use in the strategy. Drag a window around the profiles inside the component.

Let’s edit the parameters for this toolpath by double clicking on the Contour Projection strategy in the operation manager.

Significant Parameters The engraving is required to be 0.3 mm deep into the cavity, we will input that as a negative value in the Stock Oversize parameter box.

Also here the Machining Strategy is Unidirectional meaning the cut will always be in one direction only. Double click here to access the parameters for this strategy.

Check the results of the toolpath, they should look like the following image. Remember that the passes are 0.3mm below the surface so shading the file will not be any help!

Enter the parameters on the Machining tab as shown on the next page and select ‘OK’ to calculate a basic toolpath.

Editing the Machining Parameters If this is very hard material and you would like the cutter to stepdown using a few passes, go back to the Machining Tab and focus on the Engraving Mode parameters. The stepdown we will use is 0.1mm and the number of offsets will be 3.

From the Approach / Retract tab set the approach and retract modes to Axial, so that the tool enters and leaves the job in a vertical motion.

Finally go to the Transitions tab to edit the retraction methods. Change the Rapids Management to Safety Distance. This will mean that the cutter only retracts to a minimum safety height and not back to the clearance plane every time it lifts off the job, this will reduce the machining time significantly.

Semi & Finishing Tracing 3D Open the file ‘3D Curve Example.wkf’ Tracing 3D is purely a Curve based machining strategy and does not require and solid or surface information. It can be useful for engraving or cutting round trim lines of components.

The file consists of one closed profile. Open the operations manager and select ‘New operation – Tracing 3D’ Select the “New Operation” menu to create the new operation.

Here is the result of the edited Contour Projection strategy showing the multiple levels, vertical entry and exit, plus the rapid moves at the safety distance.

Select ‘T3 – 6mm Ball Nose tool’

Let’s edit the parameters for this toolpath by double clicking on the Tracing 3D strategy in the operation manager.

Double click here to access the parameters for this strategy. Now select the profile START POINT

Enter the parameters on the Machining tab as shown on the next page and select ‘OK’ to calculate a basic toolpath.

END POINT

Select the middle of the top part of the profile as the start and end point of the machining Accept the machining direction, confirm using the RHM button. Flag the ‘Auto Rebuild’ check box and select ‘OK’

Check the result from the calculated toolpath. You should see only a single pass moving from the start to the end point in the direction specified. It should look like the image below. Editing the Parameters The ‘Engraving’ option works within this strategy and this is the same as the ‘Engraving option’ from the ‘Contour Projection’ strategy.

Go to the Machining tab and change the operation parameters to the following options and re-calculate the toolpath.

Semi & Finishing ISO Machining ISO Machining is the process of cutting individual surfaces which belong to a larger solid or surface model. Although the strategy is effectively cutting single surfaces the toolpath is still fully gouge checked against the machined piece. The following example shows some of the features and parameters used in the ISO Machining toolpath. Open the file “ISO-MACHINING.wkf” Create a new profile on the bottom face using the profile from face command.

The engraving option will allow the user to enter the depth of cut ‘Step Down’ and the number of cuts above and below the selected profile, ‘Levels on Surface’ and ‘Levels under Surface’ The toolpath should look like the one in the image below.

Double click here to access the parameters for this strategy.

Open the operations manager and select “New Operation – ISO Machining

The first area to look at is the Pattern drop down box accessed from the Surface paths tab. The “Pattern” options determine the toolpath shape and are as follows:Parallel cuts – Parallel option Parallel cuts

Select “OK” and then Select the “T3 – 6mm Ballnose” and select “OK”

We will now be presented with the new ISO machining layout. Parallel cuts – Constant Z option

Cuts along curve option

Morph between 2 curves option

The principle behind how the ISO machining works can be shown in the following flow chart.

Select the “Parallel” option to set the machining angle in Z to 90 and then select the “Drive Surfaces” option to pick up the surfaces to machine.

Click “OK” to confirm the list of selected surfaces. NOTE This list only contains the surfaces to machine and does not include any surfaces that are used for the gouge checking. The gouge check surfaces MUST be selected from the separate tab in the new interface

Select “OK” once more and then expand the tree in the operations manager and calculate the toolpath by highlighting in the tree and then selecting the “Toolpathbatch build” icon Pick the surfaces as shown in the image below.

The result will look like the following image. Next we will change some options to deal with the amount of lift off.

The toolpath will now lift with a portion of feed move and a portion of rapid move as shown in the image. The exact distances for the feed and rapid movements can be adjusted with the button from the Link tab as shown below.

To change the options for the lifting off along the passes the linking options need to be changed. Go to the Link tab and adjust the following options. Then rebuild the toolpath.

Changing the Pattern type – Cuts along curve Double click the operation parameters to change the settings for the second option and toolpath pattern.

Change the pattern type to “Cuts along curve” and we must now select the “Edit curves - Lead” icon and pick the profile at the top of the part.

Select “OK” on the main interface and then rebuild the toolpath, the result will be as shown in the image. To overcome lift-offs along the cut or in between the slices then the linking options need to be changed. Edit the parameters of the linking tab and change the following option from 110% to 200% and then recalculate the toolpath.

Enter the machining parameters and swith to the Link tab.

Select the Top Profile and then click OK.

Here is the result of changing the ‘Link between slice option’ as previously described. There are now no lifts between each toolpath link.

Here you can see that if the motion is bigger than the gap size the tool path is set to "broken". If the motion is smaller than the gap size the tool movement is "direct". The gap size is set to 50 % of tool diameter. The tool diameter is 20 mm so the small gaps are 10 mm and the big gaps are all gaps bigger than 10 mm.

LINK BETWEEN SLICES

Some Information about the linking and lifting options GAPS ALONG CUTS If gaps along a tool path are detected, then you have different choices how the tool should pass the gap and pursue machining. Depending on the size of the gap it is possible to set two different options on whether it is a big or a small gap. The value in the field "Small Gap Size in % of tool diameter" sets the threshold for small and large gaps along a tool path segment. The value is defined as the percentage of tool diameter. All gaps along tool path segment, which are smaller than this threshold value, are considered as small gaps and the action defined for small gaps is executed. All other gaps that are larger than this value are larger gaps and the action defined for large gaps is performed. E.g. if tool diameter is 20mm and the gap size is set to 10%, then the threshold is 10% of 20mm, which is 2mm. All gaps which are smaller than 2mm are considered as small gaps. All gaps greater than 2mm are considered large gaps. If you don’t want the gap size depending on the tool diameter just activate "as value" and set a value.

Similar to gaps along cut you differ between small and large links. This difference size is calculated as a percentage of the user given maximum step over value.E.g. if this value is set to 150% and the maximum step over value is 0.1mm the gap threshold is 0.15mm. That means, all step over moves from one tool path slice to the next slice are checked against this 0.15 mm and determined whether the gap is smaller or larger than this value. If you don’t want the gap size depending on the maximum step over just activate "as value" and set your value.

Toolpath Pattern – Morph Between 2 Curves The third and final toolpath pattern and the one where will add the collision control is “Morph between 2 curves” Double click the operation parameters to change the settings for the third option and toolpath pattern. Change the pattern type to “Morph between 2 curves” and we must now select the “Edit curves – First and Second” icons and pick the profiles at the top and bottom of the part.

For this operation we will also add more surfaces to machine. Click the “Drive surface” icon and from the dialogue box select the “New” icon to add additional surfaces.

Select the Drive Surfaces button to begin adding new surfaces.

Use this icon to add the new surfaces to the drive surfaces group. Pick the side walls as additional machining surfaces.

Select the Top Profile as the first curve.

Select the Bottom Profile as the second curve. Click OK to confirm the selection of the surfaces.

From the main dialogue window click “OK” and rebuild the toolpath, the result should be as follows:-

NOTE Although the toolpath looks fine there is no collision checking applied at present and this MUST be done to stop any gouging on the part. From the picture below, a section view of the above toolpath shows the collision when no checking is applied.

Double click the operation parameters and activate the “Gouge Check” tab.

Up to 4 sets of surfaces can be defined for gouge checking but we will use only 1. Activate the option for set 1 and pick the surface selection icon.

Any number of surfaces can be selected for gouge checking from only 1 additional surface to all the surfaces that make up the part model or from additional models if needed. Gouge Area

For this exercise we will select the whole model. Use the “Selection inside of a window” icon from the left hand side of the screen and drag a window around the whole model.

Drag a window around the whole part as shown below to select all the surfaces for collision checking.

Finishing Steep & Shallow Open the file steepshallow.wkf The purpose of this new strategy is to replace the operation “FINISHING COMBI” and to overcome the discovered problems and the limitations. This function machines in a synchronous manner switching between steep and shallow strategies based on the shape of the geometry. It is possible to define an angle (Reference angle) to split the Steep areas from the Shallow areas. Areas that lie between 0 degrees and the “Reference angle” are considered shallow areas and are machined using a “constant step-over” like strategy. Areas that are greater than or equal to the “reference angle” are considered steep and are machined using a “constant Z finishing” like strategy.

From the left menu, select the operations manager icon, and from the Operations Manager select NEW OPERATION,

Select ‘OK’ to confirm the check surface selection.

Click “OK” and recalculate the toolpath. The result will now have the collision detection applied and will not gouge the part as shown in the image.

Scroll down the list of strategies and select STEEP & SHALLOW, then select OK.

The toolpath will now be listed in the operations manager……..

Double click the operation, and the toolpath dialog box will appear.

Select a 6mm ballnose from the library, then select OK.

Select the geometry…..then confirm the selection.

The stepdown and stepover can be different values, in this example, we will use 1mm for both.

The stepdown can be constant, or adaptive.

If adaptive is selected as the step-down mode, you can adjust some parameters under the Advanced settings tab. The corners management is also accessed in this area.

As a default, the system performs the stepover as an increment. If Scallop mode is turned on, a Theoretical scallop value can be defined and will be used.

Adaptive parameters This reference angle splits the steep and shallow areas. Corner management

The angular control allows a minimum and maximum angle to be used. In this example, the system will ignore any areas less the 0.1deg. (ie: flat areas)

The shallow areas can be machined in the following ways: Unidirectional Zig-Zag Downward Upward

The steep areas can be machined unidirectional or Zig Zag.

NOTE:

The cutting mode can be climb or conventional.

If the upward or downward strategy is selected, the advanced settings tab will be available in order adjust specific parameters associated with those toolpath types.

Offset type: The following options are available:

Depending on which offset method is used, the system will render a completely different result. The type of offset that should be used is solely dependent on the geometry being machined. Below are some illustrations which will show the different types of behavior.

Upper type: the upper waterline pass is offset and trimmed to the lower waterline pass. Lower type: the lower waterline pass is offset and trimmed to the upper pass. Both type: both lower and upper passes are offset together. The offsets will be looped.

Once the parameters have been inputted, select OK. Select the toolpath, right click with the mouse, and select Toolpath Batch build.

If you turn on the toolpath display and zoom into some areas…..

You will notice the toolpath machines all areas using both a steep and a shallow strategy. Unlike the traditional strategies, this one will machine the part in a synchronous matter.

Upper Offset

Lower Offset

Both Offset

If the toolpath is animated, you will notice that the system is machining both steep and shallow areas at the same time. In older strategies, such as Finish Combi, the steep areas were completely machined first, then the shallow areas, which was not as efficient as this new strategy.

Welcome to Visi Machining In this training documentation it is assumed that the user is familiar with the basic navigation of Visi and only parameters relative to the machining strategy will be explained in detail. Once you have created the first toolpath, you will notice that the dialog boxes remain consistent for all toolpaths, which considerably reduces the learning process.

What is Covered in this Chapter?

RestMachining

Rest Machining Rest Material Corner Rest Machining Pencil Milling Theoretical Rest Areas Rest Material COMBI Rest Material contours

Rest Machining Rest Material

Open the file Rest material.wkf The term, rest machining, refers to one of several strategies used to calculate areas of the job where material remains after running previous toolpaths. Some of the rest machining strategies work out the areas where material will be left and create the toolpath to machine those areas.

From the left menu, select the operations manager icon, and from the Operations Manager select NEW OPERATION,

Once the local library appears, select a 4mm ballnose then select OK.

(NOTE: If a 4mm ballnose tool does not exist, one must be created)

Scroll down the list of strategies and select REST MATERIAL, then select OK.

The Rest material toolpath will now be listed in the operations manager…. The left/right distance is the amount the system offsets the initial pencil pass that is created at the surface intersections. In this example it will offset the original pass 1mm on either side.

Double click the operation, and the toolpath dialog box will appear

If you wanted to create additional passes in order to gradually machine the material, you could change the horizontal & vertical stepover to 0.2mm and leave this value set to 1mm and the result would look like the image below:

The system maintains a 1mm total offset on either side of the original pass but adds more offsets in between at 0.2 mm increments.

A steep/shallow angle can be enabled in order to avoid vertical or near vertical areas by checking the angular control box and applying the minimum/maximum angles. In this example we will set a minimum of 0 deg and a maximum of 89 degrees.

The vertical and horizontal stepover can be adjusted independently. In this example we will set them both to 1mm

The machining strategy can be changed:

The toolpath will now be calculated and the progress can be monitored when the process manager pops up.

In this example, Zig-Zag will be used.

The default computation method is set to the Quick method, which is what we are using in this example, but if required, if you can change this to the Rest area method which will use a reference cutter size:

When the toolpath calculation is completed, you can visually see the result by either clicking the box beside the toolpath or by selecting the toolpath display icon.

OR

The approach can be toggled to work from outside in, or , inside out. In this example the toolpath will run from outside in.

Once these parameters have been set, select OK. Select the toolpath, right click with the mouse and select Toolpath batch build:

Select a 6mm ballnose tool, then click OK.

Rest Machining Corner Rest Machining

Open the file corner rest.wkf This function allows the computation of a particular type of toolpath that will remove all the un-machined areas of a Theoretical reference tool. The strategy uses an internal pencil milling strategy which is computed using the theoretical previous tool diameter being programmed. This means that if, on the model, there are radii with a value greater than or equal to the “previous tool radius”, theses areas will not be machined.

Then, select the geometry to be machined, and confirm the selection.

Please note that for this release the “Reference tool” can only be a “Ballnose” type

From the left menu, select the operations manager icon, and from the operations manager select NEW OPERATION….. Scroll down the list of strategies and select Corner Rest Machining, then select OK. The Corner rest machining dialog page will appear……

The stepdown and stepover can be different values, in this example, we will use 1mm for both.

By default all areas are machined, but this can be toggled to output either Steep or shallow areas independently.

The previous tool is the Theoretical reference tool mentioned earlier. Once again, a BALLNOSE tool is only supported.

The angle used to identify and split the steep and shallow areas.

This will control the precision when searching for areas to be machined. If you reduce this value the system will begin to find many more areas due to the triangle variations, however this value is dependant on the piece been machined.

Setting 90° will machine all the rest material areas along the corner (image 3). Setting 0° will machine all the rest material areas will be machined across the corner (image 4). Setting 45° will machines areas between 0 and 45° along the corner, while areas between 45 and 90° will be machined across the corner (image 5).

It is very useful to solve situation where the blend radius of the model is more or less equal to the reference radius (so in theory there is no material to be removed). In this situation the system normally creates the pencil passes but the rest material passes will not be made in order to avoid any creation of unnecessary rest machining passes.

Image 3

Image 4

Image 5

(see Image A)

R tool = R blend

The Steep machining strategy can be toggled, but the Shallow machining strategy only supports climb milling at this time. In this example, it will be set to climb.

Image A

Image 2

This parameter allows the max Z height of material to be removed to be set. The tool is not allowed to machine the passes lower than this value on the theoretical areas found on the part. This parameter is very important to prevent tool brakeage when it is necessary to machine hard material. Situations, like that shown in Image2 can be dangerous for the tool life.

The default value should be 1/3 of the Tool radius. It is suggested not to set the “max depth of cut” larger then the tool radius.

Linear: allows the option to have direct movement between the passes Spiral: allows the option to have a smooth movement between the passes similar to a “spiral” Flying Spiral: The linking movements between the passes are not projected on the model. Linear Spiral

Allows the splitting of the rest machining passes if the angle deviation of the pencil passes is bigger than the programmed value.

This option allows the organisation of the pencil passes in the way to generate more connected and uniform passes.

Planar: The system looks at the pencil passes from the tool axis (from +Z) and connects the passes that have the angle deviation less than the value set in Max Angle deviation.

Max angle deviation =130°

Max angle deviation =136°

Angular: The system looks at the pencil passes from any directions (3D point of view) and connects the passes with angle deviation less than the value set in Max Angle deviation.

No Sorting: The system follows exactly the pencil passes. For any part of the pencil pass there will be a group of Rest machining passes. The risk in this case is that uncut material could be left in the corners or were more part of the pencil passes converge at one point.

Once the parameters have been inputted, select OK. Select the toolpath, right click with the mouse, and select Toolpath Batch build.

When the calculation is completed, you can animate the result by selecting the Toolpath Simulate icon.

Select “All Step” to view the entire toolpath.

Notice during the simulation the vertical areas on the part are being machined using a Constant Z strategy and the shallow areas are being machined using a 3d stepover strategy.

Rest Machining Pencil Milling

Open the file pencil.wkf This function will create a toolpath that will calculate a single pass on all corners of a part giving an excellent finish. The area to be machined is determined by the diameter of the tool selected. If there is a radius on the model and the radii value is larger than that of the tool diameter this area will not be machined.

Constant Z From the left menu, select the operations manager icon, and from the operations manager select NEW OPERATION….. Scroll down the list of strategies and select Pencil Machining, then select OK.

3d Stepover

From the local library select a 4mm ballnose tool, then click OK.

Select the geometry to be machined, then confirm the selection.

Toggling this parameter will limit the toolpath from 0 to 45 degrees. For this example use these values.

The machining strategy can be changed. If an UpWard or Downward strategy is used, the ADVANCED settings become available. In this example use Unidirectional.

Double click on the toolpath in the operation manager……..

The Upward milling strategy will force the tool to always machine in an upward direction, and conversely, when Downward is selected, the tool machines in a downward motion.

This utility can be used for roughing out the corners by stepping down in Z increments. In this example disable this option.

The Bi-Tangency control is a special angular tolerance that you can use to control the system precision while searching for areas to be machined. All machining operations have a tolerance and the smaller the value, the more accurate the calculation. This is an extra thickness that can be temporarily applied to the cutter in addition to the normal thickness. You can use Overthickness to make passes along fillets where the radius is greater than that of the cutter. For example, if you have a surface with fillets of corner radius 8 mm and you want to create a Pencil Milling along it with a 10mm ballnosed cutter, you can apply an Overthickness of 4 mm to it. The Pencil Milling will be made for a ball-nosed cutter of size 18 x 9 mm (which will detect this fillet), and then projected back onto the surface to make a toolpath for the 10 x 5mm cutter.

Rest Machining Theoretical Rest Areas

Open the file theoretical.wkf A set of 3D boundaries can be generated from rest areas left by an imaginary reference cutter. This gives good results when used for machining operations at the semi-finishing and finishing stages of a job. You can then use these boundaries to limit another set of passes made with a cutter of an equal or smaller size.

Once the parameters have been inputted, select OK. Select the toolpath, right click with the mouse, and select Toolpath Batch build.

From the menu, open the operations manager………………

Once the calculation is complete, you can animate the toolpath to view the result.

Inside the operations manager, there is an icon which will access the Geometrical tools in Visi……..

Once the “Theoretical rest boundaries” are selected, click OK. The Local library will then open and will require that a reference tool be selected. In this example, a 4mm ballnose tool will be used……….

The system will then prompt to use boundaries…….In this example we will create boundaries on the entire part, so press RHM

If you wanted to create boundaries only in specific areas of the part, you could use 1 or more profiles as “containment areas”. This is especially useful are large parts.

Select all elements, in order to create boundaries on the entire geometry…

The Theoretical rest area dialog box will then appear.

Define if the status of the stock

Set the min/max angles.

Define the Previous tool that was used. This can be either a ballnose or Toroidal type. Then confirm the selection………

On the advanced tab, other parameters can be adjusted……

If we remove the shading, and view the geometry in wireframe mode, you will see the new boundaries that were created……..

The smallest amount of material to be found in areas included in the rest area boundary prior to rest machining. If the reference cutter left parts of the job with less than this amount of material, those parts of the job would not be included in the rest area boundaries. This is the granularity of the calculation. The smaller the value, the finer the detail of the boundaries made, but the slower the calculation. The diameter is the span of the boundary, the distance between two points on either side. Boundaries that have a diameter smaller than this value are discarded The boundaries are offset outwards along the surface by this amount after they have been made.

Once all the parameters have been imputed, the system will begin calculating the boundaries……..

These boundaries can now be used as containment when creating the different toolpath strategies that are available…..

When the calculation is finished, a message will appear indicating the number of boundaries that we created……

Select a 6mm ballnose tool, then click OK.

Rest Machining Rest Material COMBI

Open the file restmaterialcombi.wkf This function allows the machining of un-machined areas left behind from a previous tool using different machining strategies for Steep and Shallow areas. The most important features are:

Then, select the geometry to be machined, and confirm the selection.

x Ability to machine the Steep areas using Constant

Z or 3D Step Over or Parallel Plane strategies. x Ability to machine the Shallow areas using 3D

Step Over or Parallel Plane strategies. Please note that the “Reference tool” can either be a Ballnose or Toroidal Type

From the left menu, select the operations manager icon, and from the operations manager select NEW OPERATION….. Scroll down the list of strategies and select Rest Material COMBI, then select OK. Double click on the operation……..the Rest material Combi dialog page will appear……

can be changed……… Define the reference tool. This can be a Ballnose or Toroidal type. In this example, we will use a 10 mm ballnose. The stepdown type can be toggled.

Corner smoothing can be enabled.

These parameters are identical to those explained in the theoretical rest areas section.

Defines the steep/shallow angle being used. An overlap angle can be used to avoid marks where the two different strategies meet.

From the the next.

tab, there are different ways the toolpath can move from one Z level to

In this section, it is possible to select different strategies to machine shallow areas. The 2 strategies are:

In this section, it is possible to select different strategies to machine steep areas. The 3 strategies are: Constant Z (most common) Parallel Plane (used in 3+2, shallow geo) 3d Stepover (used in 3+2, shallow geo)

Parallel Plane 3d Stepover

can be also changed for shallow strategies……..

tab, there are different ways the From the toolpath can be linked when it steps over.

A minimum pass length can be defined. This will discard any passes that are less then this amount.

Once the parameters have been inputted, select OK. Select the toolpath, right click with the mouse, and select Toolpath Batch build.

Constant Z strategy

3d stepover strategy

If we RHM on the toolpath and turn off the transition and rapid motions, we can see the different strategies used to machine the part.

The Geometrical tool dialog box appears, and unlike before, the Rest material contours option is now visible (this is because we selected an operation prior to selecting the icon).

Rest Machining Rest Material Contours

Open the file restmaterialcont.wkf Similar to theoretical rest areas, this strategy requires that one reference OPERATION be used instead of a hypothetical tool. The system will create a set of 3D profiles from rest areas left by the selected operation. It is possible use these profiles to limit another set of operations made with a tool of an equal or smaller size. Make sure it is selected, then click OK.

The profile manager will appear……….. From the left menu, select the operations manager icon. In the operation manager, there is a parallel plane toolpath we will use as the reference operation. Click on the toolpath, then select the Geometrical tools icon……..

Minimum thickness It is the smallest amount of material to be found. If the reference operation left parts of the job with less than this amount of material, those parts of the job would not be included in the Rest material profiles. The min material depth should be greater than the "scallop height" left by the reference operation. Contour type 3D profile: the rest area profile will be made in 3 dimensions. 2D profile: the rest area profile will be made on the current work plane.

Once the parameters have been set, select OK. The system will calculate the rest areas and a message will pop-up and display how many profiles (rest boundaries), were created.

If we look at the part we can see the boundaries………

If we toggle the reference toolpath display on………

You can zoom into areas were the boundaries were created.

In these areas the thickness exceeded 0.2 mm, and the boundaries were created.

Welcome to VISI Machining 3D

The geometrical tools presented in this document add an extra set of functionality to the creation of boundaries for machining purposes. The geometrical tools are not extra toolpath strategies but are profile/mesh creation type tools that can be used in conjunction with the machining strategies contained within VISI Machining 3D. The following guide will show you how and where these can be used with hands on examples. Familiarity with VISI Machining is assumed so every single step will not be documented.

What is Covered in this Chapter? Rest Machining

3DCAMGeometrical Tools

Rest Material Contours Theoretical Rest Boundaries Shallow Area boundaries Silhouette Boundaries Cutter Contact Areas Fillet Surfaces

The Geometrical tools can be accessed from the Operation Manager icon bar. The following is guide for each option available.

The results should be the same as below.

Rest Material Contours Open the file Rest Material Contours.wkf Make sure the Radial Strategy is selected from the operation manager before selecting the geometric tools icon.

The ‘Rest Material Profile Manager’ option will then appear.

The outer profile in this case is not needed and can be deleted. The rest of the profiles can be used individually or nested. These profiles can then be used as machining or limiting boundaries if required. Try different values to view the different results.

Enter ‘0.1 into the minimum thickness and 2D Profile’ into the Contour type. Minimum Thickness - This value relates to the minimum thickness of the scallops that the system will use when generating the rest material profiles. The system is using an imaginary reference toolpath on the component and generating the rest material profiles from the cusp height (Minimum Thickness) used on the toolpath. In practice the smaller the value the more rest material areas will be identified and more profiles generated. Contour Type - This option relates to how the profiles will be generated. After the rest material profiles have been generated the profiles will be created either projected onto the component and therefore 3D profiles, or the profiles can be projected onto the active workplane and therefore 2D profiles. Select ‘OK’

Theoretical Rest Boundaries This option allows the creation of 3D profiles from rest areas left by an imaginary tool. This gives good results when used for machining operations at semi-finishing or finishing stages of a job. You can then use these boundaries to limit another set of toolpaths made with a cutter of an equal or smaller size.

Resolution This is the granularity of the calculation. The smaller the value, the finer the detail of the boundaries made, but the slower the calculation time. Minimum diameter: The diameter is the span of the boundary, the distance between two points on either side. Boundaries that have a diameter smaller than this value are discarded

User interface This option is available in the following situations when the: x

Focus is on the project item

x

Focus is on the tool item

x

Focus is on the operation item

Step 1: Define your tool - the smaller, secondary one with which to machine inside the rest areas and create the boundaries. If previously the focus was on an already used tool, the system will use this tool. Step 2: Select the model geometry on which you want to find the rest material areas (using the same dialog box used for the geometry definition for 3D machining operations).

Offset: The Shallow Area boundaries are offset outwards along the surface by this amount after they have been made. Sometimes it may be advantageous to put in a small offset value; you can prevent jagged boundary edges where an area of a surface is at an angle similar to the Contact Angle Include corner areas: If switched on, the system will include in the areas detection also the areas were more the one edge meet together. See example: Holder clearance: Defines the safety distance between the holder and the model geometry. Please note that “Holder clearance” is automatically switched on if has been selected tool + tool holder.

Step 3: Select profiles as boundary limitation for the Theoretical rest areas profiles. Step 4: The system will display the following dialogue box: Stock oversize: The distance between the surface and the cutter (and the boundary) If you set the distance to be zero, the boundary will be based on calculating the movement of the cutter along the surface itself. If a positive number, it will be above the surface, if a negative number, it will be below the surface. Angle Max and Angle Min allows you to force the area detection only between the specified Max and Min angled you have entered. Using this option will allow you to isolate, for example, only the “shallow” areas of the whole model. Previous Tool : This allows you to specify a cutter with which the Theoretical Rest Areas will be calculated against. This cutter is usually larger than the cutter being used to cut the rest areas. The reference cutter represents the tool used in the imaginary toolpath.

Corner Areas= ON

Corner Areas= OFF

Try it out Open the file shallow_areas.wkf Use a 6mm Ball Nose Tool to as the actual cutter to be used. Set the Parameters as shown. P.T.O….

Theoretical Rest - Try it out cont………………….

Shallow Area boundaries This new option allows you to make profiles around the shallow (flat) areas of the selected model. The system produces 3D profiles User interface This option is available in the following situations when the: x

Focus is on the project item

x

Focus is on the tool item

x

Focus is on the operation item

Step 1: Define your tool - the tool that you will use to machine inside the Shallow area boundaries. If the focus was on a previously used tool, the system will use this tool. Step 2: Select the model geometry on which you want to find the Shallow area (using the same dialog box used for the geometry definition for 3D machining operations). Step 3: Select profiles as a boundary limitation for the Shallow areas boundaries. Step 4: The system will display the following dialogue box:

100 Rest Material Boundaries are detected.

Stock oversize: The distance between the surface and the cutter (and the boundary) If you set the distance to be zero, the boundary will be based on calculating the movement of the cutter along the surface itself. If a positive number, it will be above the surface, if a negative number, it will be below the surface. Use vertical oversize: If selected, this parameter allows you to specify an additional oversize value only on the vertical faces. Angle Max and Angle Min allows you to Set the contact angle range of your tool by setting the minimum and maximum contact angle. Boundaries will be drawn around areas where the angle is within that range. For Shallow Area boundaries, the range

should typically be between 0 and 30 degrees, but where surfaces are very close to the minimum or maximum angle, you may get an undesirably jagged edge so you may want to alter the range slightly. Alternatively, you can sometimes get rid of jagged edges by giving the boundary a small offset

Step 5: After computing, the system will display the following dialogue box and will create the Shallow area boundaries on the working layer as shown.

Max Z level: This is the highest positions of the tool along the z-axis Try it out Min Z level: This is the lowest positions of the tool along the z-axis Open the file shallow_areas.wkf Contact Areas Only: This option should be selected (ticked) to limit your boundary to the surface, with no major material clearance. If you want to create boundaries that include non-contact areas, then the option should not be selected (box not ticked). Resolution: This is the granularity of the calculation. The smaller the value, the finer the detail of the boundaries made, but the slower the calculation. Minimum diameter: The diameter is the span of the boundary, the distance between two points on either side. Boundaries that have a diameter smaller than this value are discarded Offset: The Shallow Area boundaries are offset outwards along the surface by this amount after they have been made. Sometimes it may be advantageous to put in a small offset value; you can prevent jagged boundary edges where an area of a surface is at an angle similar to the Contact Angle Holder clearance: Defines the safety distance between the holder and the model geometry. Please note that “Holder clearance” is automatically switched on if has been selected tool + tool holder.

Use a 6mm Ball Nose Tool to define the shallow area boundaries. Set the Advanced Parameters as shown. Shallow area boundaries created.

Isometric view

Silhouette Boundaries This new option allows you to create a profile that has as shape the perimeter that you see when you looking at the selected model from the Z axis. User interface This option is available in the following situations when the: x

Focus is on the project item

x

Focus is on the tool item

x

Focus is on the operation item

Step 1: Select the model geometry on which you want to find the Silhouette area (using the same dialog box used for the geometry definition for 3D machining operations).

Top view

Step 3: Select profiles as boundary limitation for the Silhouette areas boundaries. Step 4: The system will display the following dialogue box:

Resolution: This is the granularity of the calculation. The smaller the value, the finer the detail of the boundaries made, but the slower the calculation.

Try it out Use the reference material as a guideline for this exercise. Open the file littleman.wkf and create the boundary from the STL mesh file.

Please note that using a bigger value it is possible get a more smoother silhouette boundary Step 5: After computing, the system will display the following dialogue box and will create the Silhouette boundaries on the working layer as shown.

Cutter Contact Areas

Step 4: The system will display the following dialogue box:

This option allows you to make profiles around areas where the cutter is in contact with the selected model. The system produces 3D profiles. Please note that the Cutter Contact Area does not work on vertical or nearvertical surfaces. The steepest angle you should use for best results is 80 degrees. The following example shows how it is possible to set a clearance distance from the faces which you don’t want to touch (and mark) with the tool.

Yellow profile= working area limit. Green profile= cutter contact area profile computed inside the working area ( yellow profile) “D” = Clearance distant from the vertical faces. This distance has been made setting the vertical oversize on the parameters window. User interface The option is available in the following situations, when : Focus on project item Focus on tool item Focus on operation item Step 1: Define your tool - the tool you will use to machine inside the Cutter contact areas boundaries. If previously the focus was on an already used tool, the system will use this tool.

Stock oversize: The distance between the surface and the cutter (and the boundary) If you set the distance to be zero, the boundary will be based on calculating the movement of the cutter along the surface itself. If a positive number, it will be above the surface, if a negative number, it will be below the surface. Use vertical oversize: If selected, this parameter allows you to specify an additional oversize value only on the vertical faces. Constraint: Most machining operations or 3D boundary creation constrains or limits the tool centre to the edge of the boundary or surface; it can move no further than this. But when creating a boundary with Cutter Contact Areas, you can constrain or limit the tool contact point to the boundary instead, in effect the machinable area is offset by the radius of the cutter. Centre Point: The point where the cutter contacts the surfaces is always within the boundary

Step 2: Select the model geometry on which you want to find the Cutter contact area (using the same dialog box used for the geometry definition for 3D machining operations). Step 3: Select profiles as boundary limitation for the Cutter contact areas.

Contact Point: An edge of the cutter is always within the boundary.

Offset: The Shallow Area boundaries are offset outwards along the surface by this amount after they have been made. Sometimes it may be advantageous to put in a small offset value; you can prevent jagged boundary edges where an area of a surface is at an angle similar to the Contact Angle Holder clearance: Defines the safety distance between the holder and the model geometry. Please note that “Holder clearance” is automatically switched on if has been selected tool + tool holder. Step 5: Angle Max and Angle Min allows you to Set the contact angle range of your tool by setting the minimum and maximum contact angle. Boundaries will be drawn around areas where the angle is within that range. For Shallow Area boundaries, the range should typically be between 0 and 30 degrees, but where surfaces are very close to the minimum or maximum angle, you may get an undesirably jagged edge so you may want to alter the range slightly. Alternatively, you can sometimes get rid of jagged edges by giving the boundary a small offset.

After computing, the system will display the following dialogue box and will create the Contact area boundaries on the working layer as shown.

Try it out Use the reference material as a guideline for this exercise. Open the file cutter contact.wkf Use a 6mm Ball Nose Tool and the following settings

Max Z level: This is the highest positions of the tool along the z-axis Min Z level: This is the lowest positions of the tool along the z-axis Contact Areas Only: This option should be selected (ticked) to limit your boundary to the surface, with no major material clearance. If you want to create boundaries that include non-contact areas, then the option should not be selected (box not ticked). Resolution: This is the granularity of the calculation. The smaller the value, the finer the detail of the boundaries made, but the slower the calculation. Minimum diameter: The diameter is the span of the boundary, the distance between two points on either side. Boundaries that have a diameter smaller than this value are discarded

Should create 39 cutter contact boundaries.

Step 3: Select profiles as boundary limitation for the Fillet surface. In our case we can click the Right Mouse Button to continue.

Fillet Surfaces This option allows you to create fillet surfaces (mesh format) on all the edges of the selected model. Selecting mesh fillets entities in your model geometry definition, allows you to reduce sharp changes in cutter direction and machine more quickly. By adding curves to the internal corners, the cutter does not have to dramatically change direction while rotating, and this helps to prevent damage to tooling and the machined piece thus allowing for faster feedrates.

Step 4: The system will display the following dialogue box:

Tolerance: The tolerance to which the new fillet surfaces will be triangulated. A lower value will give more accurate results, but will increase the calculation time.

User interface The option is available in the following situations: x

Focus on project item

x

Focus on tool item

x

Focus on operation item

Resolution: This is the "granularity" of the calculation. Using a smaller value will give the finer detail but will increase the calculation time. Number of facets: This is the number of flat faces (triangles) across the radially curved section of the fillet.

Step 1: Define your tool – the system will use his shape to generate the fillet geometry. It is possible to select End mill, Ball nose, Bull nose (also tapered) and eventually a tool holder. Select the tool as shown below.

End Mill

Conic End Mill

Bitangency angle: This is the minimum angle required between the two contact point of the tools to find edges. If the contact points have an angle less than the “Bitangency angle”, the fillet surface will not be generated.

Ball Conic Cutter

Step 2: Select the model geometry on which you want to create Fillets (using the same dialog box used for the geometry definition for 3D machining operations).

Max Z level: This is the highest positions of the tool along the z-axis Min Z level: This is the lowest positions of the tool along the z-axis Holder clearance: Defines the safety distance between the holder and the model geometry. Please note that “Holder clearance” is automatically switched on if has been selected tool + tool holder.

Step 5: After computing, the system will display the following dialogue box and will create the Fillet surfaces on the working layer as shown.

Try it out Use the reference material as a guideline for this exercise. Open the file filletsurface.wkf

Use a 10mm Ball Nose Tool to define the fillet surfaces and the settings shown.