VERO UK TRAINING MATERIAL

Version 20

2 Axis Wire Cutting

2 Axis Wire Cutting using Line/Arc data

Things that will be covered in this section.

• Creating Profiles and Manual Features

• Creating a 2-axis toolpath

• Editing Technology

• Path-Lab simulation

From the menu select file > Open

Open the file - 2ax_lines.wkf

The file includes 2D geometry in the form of lines and arcs.

First it is necessary to create profiles* from the geometry on the screen.

*NOTE

The profile data can be 2D or 3D and can include closed or open profiles

The data given consists of 1 outer and 5 inner areas that need converting to profiles. In this case it is possible to use a single command to create all the profiles.

Select the “Quick Profile” icon

Ensure that the intersection icon is active from the left-hand side of the screen and pick using the left mouse anywhere in between the outer and inner geometry to create profiles.

Note:- Anytime time that the system requires input, there will be a prompt message displayed at the bottom lefthand corner of screen

The quick profile command works by automatically looking outwards and inwards from the point selected, looking at the geometry to find closed loops. These closed loops will be generated as profiles.

6 profiles will be created in the default colour yellow. Next, select Machining > CAM Navigator from the menus at the top of the screen

The screen will now split vertically and the CAM Navigator will appear in a separate panel on the right hand side. *NOTE - Features tab must be selected

Inside of the CAM Navigator you will see there are 3 tabs, Features, Mill and Wire. The Mill tab can be ignored during this training course.

The Features page is used to control all of the geometry that is being machined. eg. Pockets, Profiles, Holes, Piece Material, Stock Model and Obstacles.

The Wire page is where all of the tool-path data is stored. Inside of this window it is possible to select the machine tool and edit tool-path parameters e.g. wire type/size, cut technology and post processor.

From inside the Features page, righthand click on the Model Manager option and select Add tapered manual feature

With this option selected the system will ask you to pick a profile. Only the Profile selection icon will be active, window all the profiles as shown below or use the “Select all elements” icon

You will now be presented with a dialog showing the Profiles that are to be made into Features. Inside of this dialog box it is possible to add and remove geometry that has been selected or miss-selected

Select OK from the dialog box

With the profile selection now confirmed the system will now open the Feature parameters dialog box

Inside of this window it is possible to define what kind of manual feature you wish to create by changing the feature subtype drop down box

Pease note that this list can vary in length depending on the shape of the feature that has been picked.

Ensure that the feature subtype is set to Pocket and the height is 25 and select OK to exit the dialog box

The system will now prompt for the Features Orientation (bottom left of the screen)

Confirm each profile using mouse button 2 until all profiles have been given a downward direction, if the direction is wrong, use the spacebar to change the feature direction.

The CAM navigator will now show the features that have been added to the Model Manager tree

You will see from the list that all of the features have been defined as Pockets but we require the outer feature to be a Boss. Left hand click on each of the features until the outer feature is highlighted

Righthand click the feature and select Convert pocket <> boss from the drop down list, a new Boss feature is then added to the tree. Righthand click on the original feature and select Delete

With the features now added it is possible to add our first toolpath.

Highlight all the pocket/boss features in the features tree, right hand click and select Add Operation

The system will now open the Operations dialog box. In the Operations window, select Wire erosion operations, and on the right hand side select 2 axis and click the OK button.

Note - If the system does not already contain a default machine, a new dialog box will automatically appear where you can select your machine type, select a machine icon and click the OK button. You will now be presented with a new dialog box that will contain the Project details.

Select the Piece material icon on the right-hand side
highlight a part material and click the OK button

NOTE:- Materials shown will differ from machine to machine

Select the Wire icon from the right-hand side
highlight the 0.25 wire diameter and click the OK button then the OK button on the project parameters dialog.

NOTE:- Wire types shown will differ from machine to machine

The system will now automatically build the project, select the machine and add a machining operation for these profiles.

Note - In the model manager tree the pocket and boss features text has gone from green to purple. This is to indicate that a toolpath has now been added to those features.

Select the Wire tab on the CAM Navigator to see your machining.

Inside of the operations tree, it is possible to control all of the parameters of the toolpath

and simulation options.

Righthand click on the CAM-setup and select the properties option from the menu.

Activate Use manual strategy and click OK

Righthand click on the wire operation and select the properties option from the menu.

Tip - You can also left hand double click the wire operation to get the properties

You will now be presented with a new dialog box that will contain all of the operation

parameters for the toolpath

Select the Cut method tab

Pockets - Preferred cutting direction for parts cut from the inside (dies, dowels holes etc.)

Bosses - Preferred cutting direction for parts cut from the outside (punches)

Offset - Use above options (auto) or manually select to cut on the left or right of the toolpath

NOTE:- If auto direction is selected, cutting direction has no bearing on which side of the toolpath the wire is offset.

No core (pocket) first cut - Progressively profiling the aperture from the start hole until all material is removed.

Stepover distance - The wire overlap or step over distance for successive passes (usually half the wire diameter).

Pocket mode - Specifies for round holes whether to cut out concentrically or to spiral out.

Automatically control wire cut/thread - Post processor will automatically output thread wire and cut wire commands or stop command on machines without auto-threading.

Erode between features - Move to next feature with wire threaded and power on.

Thread at angle - Allow machine to stop for manual threading at a non-vertical start position.

Vectorisation tolerance - Maximum allowable deviation from true toolpath position.

Select the Technology tab

Cuts 1-20 - Select the required offsets and technology for each cut.

Approach distance - Allows the user to select a different technology from the cut start for a set distance into the profile.

Retract distance - Allows the user to select a different technology from a set distance from the end of a profile to the end of the cut.

Reverse cutting required - Alternate the cut direction for each pass, usually used on parts that remain tagged until completion.

Offset in geometry - Modify the NC output by the values in the cuts boxes and suppress cutter compensation on the machine tool.

3D offset - Re-calculate the offsets in the cuts boxes to compensate for cutting at extreme angles.

Modify internal corners - Modify the internal corners of a profile/feature so that they are greater than the offsets in the cuts boxes (to compensate for controls that don't allow cutting of sharp corners).

Additional clearance - Apply an additional offset without editing standard offsets and technologies.

Note:- If the machining operation is a “Taper”, an extra tickbox will be visible, this allows the option of disabling the taper on a cut by cut basis.

Select the Tagging tab

Tag position - Use distance from end of feature/profile or retract point for stop position in NC output.

Tag distance - Positive value for use in above option.

Tag removal method - Options to remove the waste material. On first cut, end of operation, none etc.

Stop at end of cut - Insert an additional stop at a distance after the standard stop.

Distance - Value above stop (must be smaller than tag distance).

Use single cut for tag - suppress trim cuts on tagging operation.

Additional clearance - Leave extra stock on feature/profile when removing the tag.

Select the Approach/Retract tab

Lead on mode - Move onto the feature/profile with straight line or line followed by an arc.

Arc radius - Value for above arc

Entry point increment - Move start point of each cut by given amount

Lead off mode - Move off the feature/profile with straight line or arc followed by a line

Arc radius - Value for above arc

Equal to lead on - Lead off distance is to be same as lead on distance

Lead off distance - Lead off distance if not equal to lead on

Lead off direction - Lead off parallel or at an angle to the lead on

Lead off angle - Angle relative to lead on

Rapid lead off - Output rapid move in NC for lead off

Cut wire before lead off - Cut wire while still on feature/profile.

Select the Programming planes tab

Use feature - Use the extracted features to define the reference and secondary planes.

Secondary plane - Manual input of plane if use feature is un-ticked.

Reference plane - Manual input of plane if use feature is un-ticked.

Use project settings - use the settings defined at the project level

Upper nozzle - Height of the upper nozzle on the machine tool.

Lower nozzle - Height of the lower nozzle on the machine tool. (Usually zero)

Use feature - Get angles from selected feature.

Taper\ Land - sets the system to apply a taper or define this operation as a land cut.

Taper angle - Manual input of angle if use feature is un-ticked.

Square corner type - Corner type in sharp corners.

Round corner type - Corner type in radius corners.

Select the Miscellaneous tab

This dialog allows the user to input up to:-

5 header and 5 footer pre-set commands

5 header and 5 footer user insert commands and

5 header and 5 footer comments

Dependent on the machine control, these commands will then be output in the NC code

1. Model Manager - This option allows you to check, add or remove geometry. It is also possible to change start, approach, retract and end points.

2. Auto Rebuild - If selected, this option will automatically rebuild the toolpath as soon as you select OK.

3. Create Custom operation - This option will allow you to save all of the operation parameters as an external file.

4. Load Custom operation - This will allow you to load a previously saved custom operation.

5. Create custom settings for active tab only - save the settings of the current tab.

6. Load custom settings for active tab only - load settings into the current tab.

7. Save defaults - This option will save the current parameters as default.

8. Select Technology from Database - Load in machine specific technology and offsets etc.

9. Select Quality Target - This option is for AgieVision controls only and allows the user to input desired “surface finish and accuracy” as an alternative to direct use of Technology

Use the following parameters in the Wire operation.

Cuts 1,2 and 3 ticked

Use distance for tag with tag distance of 1mm

Tag removal method - stop then cut wire on first cut

Upper nozzle 40mm

Lower nozzle 0mm

Select OK on the dialog

The toolpath should now have been re-built with the parameters you have defined.

We can now simulate the toolpath with the Toolpath Laboratory option

Right click on the Wire operation and scroll down the option list and select the Path-Lab option

1. Play - This icon will start the simulation

2. Move point backward - This option will allow you to step back through the toolpath

3. Move point forward - This option will allow you to step forward through the toolpath

4. Stop Simulation - This icon will stop the simulation

5. Level Backwards - This icon will allow you to step backwards through the toolpath level

6. Level Forwards - This icon will allow you to step forwards through the toolpath level

7. Draw modality - This option enables the icons immediately below this list

8. Simulation Speed - This slider bar will allow you to speed up or slow down the simulation

9. Invert direction - This is icon will reverse the toolpath direction for the simulation only

10. Right clicking on the toolpaths will enable the toolpath edit options (see below) (10a)

No criteria - this option will remove any visualisation option that has been set

By element type - this option will show the type of elements that make up the toolpath e.g. segments, arcs, and helixes in a colour band option.

Same Feed - this option will colour band the toolpath relating to different speeds and feeds across it.

Show points - this option will show the physical toolpath points

Show Rapids - this option if enabled will show the rapid movements on the toolpath

Show links - this option will show all linking moves in the toolpath

Show normals - this option will show the toolpath normal points

Show helixes - This option will show all helixes in the toolpath

Set Colours - this option will allow you to control all of the colours that's are used for all of the banding options, feed rate ranges, etc

Show diameter compensation - this option will add the cutter compensation to the simulation if it has been added in the operation parameters.

Set tool transparency - this option will control the toolpath transparency of the tool and the holder itself when the transparent shading is enabled.

(10a) NOTE:- The majority of the following options apply to Milling toolpaths only.

1. Edit toolpath - this option will allow you to edit or delete a specific point on a toolpath

2. Edit entry/exit - this option will allow you to edit the entry and exit plane Z height

3. Tool path trimming - this option will allow you to trim an area of a toolpath back to a profile

4. Sub path trimming - this option will allow you to delete levels of the toolpath

5. Feed reduction management - this option is used for milling toolpaths

6. Points Equalizer - this option is used for milling toolpaths

7. Move tool on point - this option will allow you to move the tool to a specific point on the toolpath and also see the XYZ position and speed and feed at that specific point.

8. Show Links - this option if enabled will show the linking movements of the toolpath

Once the simulation has been run, Close the Toolpath laboratory by clicking on the x in the top right hand corner of the path-lab area.

You have now completed your first part.

Addendum to part 1

In the previous example, the line/arc data was made into Profiles, then into Features, then machining's were added to the Features.

We recommend the use of features in Visi because this is in line with data extracted by Visi from Solid models

For customers who prefer to use profiles only (missing out the creation of features), the following procedure can be used.

From the menu select file > Open

re-open the file - 2ax_lines.wkf

The method used to create profiles is the same as used previously but this time we will be adding a thickness (CAM attribute) to the profiles

Select the “Quick Profile” icon

Ensure that the `Quick profile attributes' icon and the `Delete original geometry' icon on the left of the screen are selected

You will now be presented with the following dialog, this is where you define the thickness of the profile and whether is a Pocket (Material side outside) or a Boss (Material side inside)

Enter the values above and click Ok, the profiles are created with attributes.

Open the CAM navigator Features tab.

In the previous example, we used, Convert pocket <> boss to correct the definition of the outer Feature, as we have not created any Features this time, we need to use a different method.

Right hand click on `CAM profile repository' and select `find profiles, click the outer profile and the CAM navigator will highlight the profile in the list, right hand click on this and select `properties'

The attributes dialog will appear, leave the thickness's at zero and select `Always inside' to change the profile from a Pocket to a Boss

Next, highlight all the profiles in the CAM navigator, right hand click and select `Add operation', at this point we have reached an equivalent position to that which we were at on page 9 when we were adding operations to Features.

Additional Examples

Open the file Punch_plate.wkf

Try creating profiles using the Close profile command

Try creating Tapered features

Try alternative machining settings

Open the file Stat-rot.wkf

Try using quick profiles to generate the profile.

Define the manual features

VERO UK

21

VERO UK

Click inside this area

Window / Select all Profiles

Selecting this icon will allow you to add more geometry to the tree

This icon will allow you to remove geometry from the tree.

9

.

8

.

7

.

6

.

5.

4.

3.

2.

1 .

6.

5.

4.

3.

2.

1 .

77.

1007.

97.

87.

17.

27.

37.

47.

57.

67.

77.

87.

Click inside this area

---