Multiple Fixture Support

Nowadays almost every NC control has the option to set up multiple workpiece coordinates systems by storing the coordinates of their origins in the controls memory. In the NC code, commands like G54 through G59 (Fanuc) move the part programs origin to the desired workpiece coordinate system during machining. This allows the operator to move the workpiece coordinate system that is called in the NC code to any location on the table by simply changing it's respective coordinates in memory. Although there are many different ways to support this functionality in EZ-MILL, mostly based on special customer demands, the below mentioned example is intended to show you the easiest way how to handle this.

Before we start let's assume that we already finished programming of a simple 2D part consisting of 4 work steps. We plan to place 3 of these parts on the machines table. For each part we set the corresponding workpiece coordinate system on the control. They are later called with their respective codes (G54, G55, G56) in the NC program.


G54	G55	G56

To achieve this we'll make use of EZCAM's integrated multiple fixture support. This is mainly handled by the Fixture and Add Translation settings located on the Work Step Data dialogs. When adding a single translation with zero distance for X and Y but with a certain number of copies, the system simulates all copies at the same place and increments the currently set fixture number by 1 for every copy during posting. In the below example we will ensure that the same fixture number (54) and Translation (X=0, Y=0, copies=3) is set for every work step.

Procedure:

Select the Work Step Data command from the Machining menu.
Go to the Tool Info tab and select the first work step from the Work Step ID list.
Input the number 54 into the Fixture field.
Repeat steps 2 and 3 for the remaining 3 work steps.
Now continue to the Verification tab and select the first work step again .
Click the Add Translation button. This will result in a new translation entry being added to the list.
Set the X and Y fields to 0, set the number of Copies to 3 and press <ENTER>.
Repeat steps 6 and 7 for the remaining 3 work steps.

Tip

Use the Repeat Group by Tool option to control machining sequence of work steps with same tool and identical translations.

Important Post-Processor Information

The post-processor used to create the NC code needs to be able to support the fixture number output. Otherwise contact the EZCAM support to get your post checked and updated.