Manufacturing > Manufacturing > The Customize Dialog Box > To Create a Follow Sketch Motion
To Create a Follow Sketch Motion
Follow Sketch motions let you sketch the tool path that the tool will follow. You can change the tool axis orientation at selected points along the sketch for 4-  and 5-Axis NC sequences.
1. Choose Follow Sketch from the drop-down list in the Customize dialog box, and click Insert.
The Follow Sketch dialog box opens.
2. Edit the Tool Motion parameters, if desired, using the Feed, Spindle, and Coolant buttons in the top portion of the box.
3. Click Sketch to sketch the tool motion. The sketching plane setup depends on the following selection:
If the Control Point option button is selected, you will be prompted to select or create a control point. The sketching plane will pass through the specified control point. The axis belonging to the control point will lie horizontally in the sketching plane.
If the Setup Plane option button is selected, use the regular sketcher setup technique to select or create the sketching plane and the Sketcher orientation reference.
4. Once the model is reoriented, sketch the tool motion. You will have two additional options, specific to sketching the Tool Motions:
Tool Kerf—Creates a construction circle with the diameter equal to the Cutter_Diam of the tool, centered at the location you select on the screen. You can reference this entity when sketching the tool path.
CL Command—Insert CL commands along the sketched tool path. You will be prompted to select location for the CL commands by selecting on a sketched entity. Then supply the contents of the CL command using the Sketcher CL Command dialog box. The system places a Sketcher point at the location of the CL command. If you later modify the sketch, the CL command placement will be determined by the new location of this point entity.
Sketcher CL commands are listed in the Customize dialog box under the Follow Cut motion they belong to. They are indented to show that their placement is controlled by the sketch. To modify placement of such a command, redefine the Follow Sketch motion and modify dimensions of the point entity corresponding to the CL command.
5. When the sketch is successfully completed, exit Sketcher.
6. If this is a 4- or 5-Axis NC sequence, you can also change the tool axis orientation at selected points along the sketch using the Specify Axis button.
The AXIS DEF menu then opens with the following options:
Add—Add an axis orientation definition.
Remove—Remove an axis orientation definition.
Redefine—Respecify the axis orientation at an existing location.
Show—Display existing axis definitions. The SHOW menu appears with the listing of existing axis definitions (Axis Def #1, Axis Def #2, ....). Placing the cursor over a definition name in the menu displays the corresponding axis definition as a cyan vector, which disappears once you move the cursor away from the menu item.
To add an axis definition, click Add and select a point on the sketched tool motion where you want to specify the tool axis orientation. Once you selected a point, you will be prompted to enter a parameter value along the entire sketch (with the start point of the sketch 0.0 and the end point 1.0). The parameter value corresponding to your selection will appear as an option in the selection menu, or you can click Enter and enter another value.
Once you specified the location, the DEFINE AXIS menu will open with the following options:
Along Z Dir—The tool axis will be parallel to the Z-axis of the Machine coordinate system.
Datum Axis—Select or create a datum axis that the tool axis will be parallel to, then specify the axis direction using Flip and Okay options.
Enter Value—Specify tool axis orientation by entering i,j,k values with respect to the Machine coordinate system.
7. The Preview button allows you to preview the tool motion defined. Click OK if satisfied, Cancel—to quit creating the tool motion.