Using the WCS and Tplanes to Set Up Toolpaths
This topic briefly discusses common machining situations and how you would use WCS or tool planes to set up your job. The general discussion here will help you decide when you need to create a new WCS to machine a part, or when you need to use Tplanes.
Keep in mind this general rule: program whatever the machine can get to in one setup with one WCS. If you have to manually change the part orientation in the machine, use a different WCS.
For most common milling applications on a 3-axis knee mill or VMC, leave the WCS aligned to the Top view and use the Top plane (Tplane) for your work. If you have a rotary axis, do the following:
- if the fixture will rotate continuously while you are cutting the part, leave the WCS and Tplane alone, and use the Rotary options from the Toolpath parameters tab, or the Rotary Axis Control page for tree-style toolpaths.
- if you need to rotate a fixture to a fixed position before the toolpath starts, and then machine a regular 2D or 3D toolpath, set the Tplane to the desired plane before creating the toolpath.
For 5-axis machines and Multiaxis toolpaths, use tool planes to work on the various faces.
If you are machining a block on the B axis of an HMC, set the Tplane equal to the Front, Right, Back and Left views with respect to the WCS to work your way around the block for each toolpath—for example, from the Planes Manager, choose Front (WCS).
In this type of application, you need to machine a part lying flat on the table, but the drawing in the Mastercam file is oriented in a non-standard plane. You cannot rotate, transform, or move the geometry in the file.
First, create a new view aligned with the part geometry. Use the New Plane dialog box to select a name, locate the origin at a suitable point, and, optionally, assign a work offset for the plane.
Select it for the WCS, and then align the Tplane and Cplane to it. Then create a 2D toolpath as you normally would. When you post the part, you will see 2D tool motion commands dimensioned from the part origin, just as if it was lying flat.
In this type of application, you would like to create operations to machine two different parts. Each part is mounted on a different fixture on your table.
To accomplish this, you would assign a different work offset to each fixture. When you create the toolpaths for each part, include the offset number in each toolpath. By basing each toolpath on an offset number instead of a coordinate position, your operator can run the job without worrying about how the fixtures are positioned on the table. All they need to do is touch off the parts properly before running the job to set each offset’s position in the control.
In the Planes Manager, create a new plane for each fixture. To create each plane, click the Top system plane, and choose Duplicate. Name the new plane and enter the offset for the fixture. Then define the origin for each plane by choosing Select in the Origin section, and touching a point on the fixture.
Before creating operations for each part, select the plane you created for the proper fixture. Mastercam will automatically output the correct offset codes when you post the operations and create tool positions relative to the origin that you specified for each fixture.





