Mastercam’s Transform Toolpath

Often a program is required for a production fixture that contains multiple parts, all of which require the same machining operations. When programming for multiple parts, the transform toolpath can save you a great deal of time; however, before using the transform toolpath, you should first be completely satisfied with the machining operation(s).

The transform operation should be used in a way that minimizes the cycle time. This can mean that for your fixture and machine, you will 1) keep the tool in the spindle until all parts have been machined or 2) machine one part completely and then the next.

The parts to be machined could be for a horizontal or vertical mill, as shown by the fixtures in Figure 1.

• From the drop-down menu, select TOOLPATHS and Transform
• Set up the Type and Methods window similar to that shown in Figure 2.
  • The Translate type will be used for multiple parts clamped on one fixture plate in a rectangular pattern.
  • The Coordinate or Tool plane methods could be used for this type of fixture. This example will use the former method.
  • The source could also be NCI or Geometry.
  • In the Source operations window, select all operations of the initial or source part.
  • On the right side of the window, enable the options to Copy source operations and Disable posting in selected source operations.
  • By assigning new work offsets, we are telling the system to post out a new work offset for each part. In the case of a Fanuc-style controller, this will mean the first part has the work offset number G54, the second has the number G55, etc.

• Set up the Translate window as required. Figure 3 is set up for a fixture holding six parts on a 3 x 2 grid.

The number of instances is important, because it will determine how many work offsets and, therefore, how many parts will be machined. The rectangular values are included simply so we can visualize that all six parts are being machined. The work offsets on the machine will determine the actual machining locations.

• Accept these selections.  

Your screen should now look similar to Figure 4, which shows the toolpaths for the six parts as described. You should also notice a ghost icon next to the original toolpaths, indicating that the G/M code for these original toolpaths will not be sent to the machine. If the original toolpath code was posted, the original part would be machined twice because the transformation operation creates a copy of the original operation.

For a more detailed explanation, watch the video “Machining Multiple Parts the Easy Way.”

Transforming One Toolpath at a Time

Oftentimes the best method to create toolpaths for multiple parts is as follows. Create the code to place a tool in the spindle, use it on all parts and switch to the next tool. You would then use that tool on all of the parts and repeat for each needed tool until all parts are completely machined.

To accomplish this, repeat the steps above, but rather than selecting all of the operations as shown in Figure 2, only select one operation. Then repeat this toolpath for each operation.

To see the process in action, be sure to check out “Machining Multiple Parts the Proper Way.” 

This next example will explain how to translate the toolpaths for the four-sided tombstone fixture from Figure 1. Once again, create a toolpath that you are satisfied with. For this example, you will keep the tool in the spindle until all machining operations with it are complete. Next the tool will need to be retracted to a safe location so that the fixture can be rotated and not collide with the cutting tool. The easiest way to minimize the possibility of the tool and the fixture colliding is to move the tool to one or more of the machines’ home locations using the G28 command.

Here’s how to move the tool to a home position:

• From the drop-down menu, select TOOLPATHS   and Manual Entry. 
• As shown in Figure 5, click on As Code and enter the following code in the Manual Entry window:
• G28 G91 Z0
• G28 G91 Y0

From the drop-down menu, select TOOLPATHS   and Transform. 

• Set up the Type and Methods window as shown in Figure 6.

In section 1, you are telling the software that the selected operations in section 3 will be rotated. In section 2, you are telling the software to rotate the tool plane, which accounts for the rotation of the pallet on the machine (90° in this instance). In section 4, you are telling the software to copy the initial operations and not to send the code for the original toolpaths to the machine (or else these original toolpaths will be run twice). In section 5, you are telling the software to create a new work offset for each new tool plane. In this case, create four new work offsets. The very first one will be work offset zero (Mastercam starts counting at zero)— increment each of the following work offsets by one. This means that on a Fanuc-controlled machine, the first side will work from work offset G54, the second side will work from work offset G55, the third side will work from work offset G56 and the fourth side will work from work offset G57. On an Okuma controller, the work offsets will be G15 H01, G15 H02, G15 H03 and G15 H04, respectively.

• Set up the Rotate tab as shown in Figure 7 and accept these selections.

You should also notice that the original three toolpaths have a picture of a ghost