4. Wire EDM V20 - 2axis from linearc

VERO UK

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

VERO UK

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.

Click inside this area

VERO UK

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.

VERO UK

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

Window / Select all Profiles

VERO UK

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

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

This icon will allow you to remove
geometry from the tree

VERO UK

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

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

VERO UK

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

VERO UK

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

VERO UK

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.

VERO UK

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

VERO UK

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

VERO UK

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.

VERO UK

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.

VERO UK

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.

VERO UK

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.

VERO UK

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.

VERO UK

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

VERO UK

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

VERO UK

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)

VERO UK

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.

VERO UK

(

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.

VERO UK

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

VERO UK

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.

Click inside this area

VERO UK

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.

VERO UK

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