Creating a Wire Toolpath
Mastercam includes toolpaths (referred to as wirepaths) for EDM machines. These wirepaths contain advanced tapering in both 2-axis and 4-axis, automatic corner filleting, synchronization, tab creation, and more. You must have a Wire product license to use these toolpaths and it also depends on the capabilities of the active machine definition.
-
Choose a Wire machine definition from the Machine tab.
-
From the Wire Wirepaths contextual tab, select a toolpath.
-
Mastercam displays the Chaining dialog box or Toolpath Hole Definition function panel depending on the type of wirepath selected.
-
Select one or more chains of entities in the graphics window, based on the toolpath requirements. Then choose OK to close the dialog box and continue.
For more information about wire chaining, refer to the drop-downs in this topic or use the Chaining Overview Help topic to learn more about general chaining.
-
Use the additional properties pages to enter the toolpath parameters and complete the toolpath.
For more information about the page and its parameters, click the Help button.
Mastercam uses two types of power settings libraries. These libraries have either a *.power or *.tech extension. Both libraries store the power settings (such as the wire diameter or condition code) values.
- The *.power libraries are legacy files that store the power setting values in a binary file. For more information on these libraries, refer to the Wire/Power: POWER Help topic.
- The *.tech libraries are modern files that store the power setting values in a xml file. For more information on these libraries, refer to the Wire/Power: TECH Help topic.
Mastercam supports Agievision, which is a control system for ED machining. Agie machines require a different set of information. To accommodate that, when you are using an Agie machine definition, the Mastercam dialog boxes look similar to what you would see on their controls.
Compared to regular wirepaths using the power or tech libraries, you specify the desired finish and the Agie control decides the power settings and how many passes are needed to obtain that finish.
| Contour Wirepath (Agie) | Contour Wirepath (Generic) |
|---|---|
|
|
For more information about using Agievision, refer to the Agievision Overview Help topic.
Mastercam also includes the AgieReg Add-In, which provides a way to enter information for the Agievision control. For more information about AgieReg, refer to the AgieReg Help topic.
| Toolpath Name | Gallery Image | Description |
|---|---|---|
| General | ||
| Contour |
|
Creates a toolpath with the same general shape in both the XY plane and UV plane. |
| 4-Axis |
|
Creates a toolpath with geometry that is different in both the XY plane and the UV plane. |
| No Core |
|
Pockets out areas of material without producing a slug. |
| Point |
|
Creates rapid moves that can be used to avoid a clamp or fixture. |
| Canned |
|
Select points and send them to the post processor with custom cycles. |
| Agie | ||
| Collar |
|
Creates a chamfer at the top, bottom, or both edges of the selected geometry. |
| Manual | ||
| Manual Entry |
|
Directly inserts text, comments, or G-codes into your NC programs. |
Wirepath chaining differs slightly from chaining for Mill or Lathe toolpaths. When chaining a wirepath, you must establish thread and cut positions before you chain the geometry. If you do not set these positions before chaining, you will receive a message as follows:
If you create a wirepath using the Window chaining method, Mastercam sets the order of items to be chained. However, if you manually select items to be chained, you must select them in the following order:
- Thread
- Chain
- Cut
A common method of setting up an operation to cut multiple contours requires that you set chaining options and create a point entity for the thread/cut point for each contour.
- Create the contours to be cut. Both closed and open contours can be part of the same operation.
- Create a thread point inside or outside of each contour. When window chaining contours, which you will do later in this procedure, Mastercam automatically uses each point entity for the thread position for each contour.
-
Select a wire toolpath from the Wire Wirepaths contextual tab.
- The Chaining dialog box displays.
-
Select Options in the Chaining dialog box.
-
Select the Break closest entity to thread point chaining option in the Chaining Options dialog box.
This is because the lead in should be perpendicular to the wirepath and Mastercam starts a wirepath only at an entity endpoint. When you chain the contours, Mastercam automatically breaks the entity that is closest to the thread point and creates a break that is perpendicular to the thread point. This provides an entity endpoint for the start of contour that is perpendicular to the lead in.
- Using the Window chaining method, select the contours and points, used for the thread points, in a single window.
- (Optional) You can change
the default search order (next closest) by choosing
different Nested chain options from
the Chaining Options dialog box.

- Make parameter selections for each of the dialog box pages. The parameter selections are applied to all of the contours in the operation.
- To have the point entity serve as both a
cut and thread point, use one of the following methods:
- Select Auto position cut point on the Leads page.
- Leave the Lead distance set to 0 (zero) on the Lead Distance page. Mastercam uses the point entity as the thread position. Entering a value for thread distance moves the thread points.
- Choose OK to generate the wirepath.
You can set non-vertical thread/cut positions for each contour of the operation on the Tapered Thread page. Mastercam uses the thread/cut position of the first contour to set up a non-vertical thread/cut. It then uses the same non-vertical thread/cut for the remaining contours.
Mastercam supports Window chaining of relief cuts in your material workpiece. Mastercam recognizes these single lines as relief cuts and chains them as such. The wire travels up those lines and back down and continues on around the closed geometry.
Several conditions must be met in order for Mastercam to recognize these relief lines when window chaining:
- The part must be a closed contour; open chains are not supported.
- You must create a Contour wirepath.
- The relief lines have to be single line, arc, or spline entities placed at the endpoints of the entities in the closed chain. If a single relief line is placed at a midpoint, it will be recognized as a separate chain.
You should deselect Infinite look ahead on the Compensation page or the relief moves will be filtered out of the wirepath.
- The start positions default to the same position as the thread position. To set the start position different from the thread position, you must deselect Set start position to thread point on the Leads page. You can then set the start position in the Start Position page.
- If you set a thread position but not a separate cut position, Mastercam automatically uses the thread position as both the thread and cut positions. You can also select Auto position cut point on the Leads page to have Mastercam automatically set your cut positions to the most efficient cut point for each contour.
- When chaining multiple contours, you can set one start position, and then set thread and cut positions for each contour. The start position can be the same as the thread point on the first contour to be chained.
- Toolpath Transform—Creates copies of operations in different orientations by transforming them, trimming them, or wrapping them around a cylinder with axis substitution. For more information, read the Transforming Toolpaths Help topic.
- Nesting—Efficiently spaces toolpaths to save time and material when machining. For more information, read the About Toolpath Nesting Help topic.
- Trim—Trims selected toolpaths to one or more closed chains. For more information, read the Trimming Toolpaths Help topic.
- Autosync Rails—Creates geometry to assist with wirepaths on models. For more information, read the Creating a 4-axis Wirepath From a Solid Using Autosync Rails Help topic.
The Generate toolpath option automatically generates the toolpath when you click OK. This option is on the pages and tabs of Mastercam's toolpath dialog boxes, and is on by default for new and edited operations. By selecting this option, you no longer need to select Regenerate dirty operations in the Toolpaths Manager after editing your toolpath.
For more information on how this option functions, refer to the Accepting and Generating Toolpaths Help topic.





