Manufacturing > Manufacturing > Wire EDM > To Create a 4-Axis Wire EDM NC Sequence in Head1/Head2 Format
To Create a 4-Axis Wire EDM NC Sequence in Head1/Head2 Format
To create a 4-Axis Wire EDM NC sequence with CL data output in Head1/Head2 format, follow the procedure below.
1. Click Wire EDM > Taper Angle. The SEQ SETUP menu appears with options for 4 Axis Wire EDM selected.
2. The SEQ SETUP menu will include the following commands:
XY Plane—Specify the bottom plane for Head2 output.
UV Plane—Specify the top plane for Head1 output.
The XY Plane and UV Plane settings are modal. That is, you have to specify the top and bottom planes for the first 4-Axis WEDM NC sequence in the manufacturing model; for subsequent sequences, the system will automatically use the previous top and bottom planes unless you explicitly change them.
The CTM DEPTH menu will appear twice to allow you specify both planes. Use:
Specify Plane—To select or create a plane.
Z Depth—To locate the plane by entering a value for depth with respect to the NC sequence coordinate system.
Use Prev—To use a top or bottom plane from one of the previous NC sequences. Select the sequence name from a namelist menu.
3. Click Customize, then select Automatic Cut from the drop-down list in the Customize dialog box, and click Insert.
4. The INT CUT menu opens with Cut already chosen, causing the CUT ALONG menu to open as well, with Drive Surf already chosen. The following commands are also listed:
Thread Point—Select or create a datum point as the loading point for the wire and starting location of the tool path.
Approach Point—Select or create a datum point as the alternate starting location of the tool path. The system will load wire at the Thread point, move it directly to the Approach point, and then start cutting from the point on the contour closest to the Approach point.
Contour1—Sketch or select the first contour in the cut.
Contour2—Sketch or select the second contour in the cut.
When creating the cut motion, the system will attempt to synchronize the entities in the two contours in the order they were sketched or selected: the first entity of the first contour with the first entity of the second contour, and so on. Keep this in mind when sketching or selecting the contours, or supply manual synchronization.
Side Surfs—Indicate the contours of the cut by selecting side surfaces. This command is used in place of the Contour1 and Contour2 commands.
Synch—Opens the SYNCH menu for specifying points to synchronize the positions of Head1 and Head2.
Direction—Indicate the direction the tool will travel in to make the cut.
Offset—Specify the direction in which the cut motion will be offset.
5. On the CUT ALONG menu, click Done to begin specifying the cut.
6. Select or create a datum point to use as the Thread point. If you selected Approach Point as well, select or create another datum point to use as the Approach point.
7. The TRAJ OPT menu will open in turn for contour1 and contour2; choose Sketch or Select to indicate the contour.
8. If you are creating synch points, the SYNCH menu opens with the following commands:
Add—Select a location on a contour to place a synch point.
Remove—Select an existing synch point to delete.
Show—Display existing synch points.
Done/Return—Close the SYNCH menu and return to defining the cut motion.
9. An arrow appears, originating at the start point that you created in step 7. Choose Flip or Okay to indicate the direction of the cut motion.
10. The SLOT OFFSET menu opens with the options None, Left, and Right. Choose an option to indicate the direction of the tool offset.
11. The INT CUT menu reappears; click Show to display the cut motion.
If you get an error message "Cut motion cannot be created" try adding more synch points.