Mazak X/C Pocket Milling Sample Using Rough and Finish pass for Matrix Control on Head 2 Only

Mazak X/C Pocket Milling Sample Using Rough and Finish pass for Matrix Control on Head 1 and Head 2

Pocket Milling using X/C on a Mazak.

Did you ever try to mill a simple square or rectangle on the centerline in Mazatrol. Did you find out that it couldn't be done because you simply don't have enough Y axis travel. I hate having to write multiple units of line left, or line out routines to accomplish a simple task. Boy it sure would be nice if you could mill a pocket using X/C mode.

Guess what, you can. Mazatrol supports the function, but you can't select the option from your control. You need to generate the code with an offline Mazatrol editor that supports X/C milling. Or, you can copy the XC pocket milling file example here and download it to your control. You'll note that you can simply copy the unit into your own program. (If you don't know how, scroll to the first line below where you want to insert the unit, and hit the right orange arrow on the keyboard and select the Unit Copy softkey. Scroll down to find the Mazak-XC-POCKET program and select it, then enter the unit number for the X/C pocket routine. You'll now have an X/C unit in your Mazatrol program. You can edit the data, or copy it in your control as you wish. Someday Mazak just might enable this feature. It's very helpful.

By the way, on a Matrix controlled Machine, Parameter E92 controls whether the pocket is milled from the inside out, or the outside in. Pretty cool isn't it.

Apparently this works on machines other than my Integrex as long as you have a Matrix Control. It works on a Mazak lathe and you can pocket mill even if you don't have a Y axis on the machine.

I've been told the same option works on a Fusion Control, but we have no way to verify that since we don't have anything that doesn't have a Matrix control on it. If you have an offline programming solution that can generate an X/C pocket milling cycle and you can test that it works, please send me a copy of the program and I'll post it here. Us Integrex users need to stick together. Collectively we can accomplish some really cool things.

Here's a little trick that works well. It starts by knowing where you need the tool tip to be in relation to the machine home. To figure that out, with the part held only in Head1 call up the tool and jog it into position. Then from the manual mode, go to the position screen, scroll to the Z axis position and enter a zero in the input field. The Z position will read 0. Now highlight the home button and send the Z axis home, but note how many inches it had to move to get there. Now you're all set.

You can call up a manual program unit and enter the following commands... you can even do it in an MDI block:

G0G28U0 (send X home incrementally)
G0G28W0 (send Z home incrementally)
G0W-xx.xxB90. (Move Z incrementally the distance you figured earlier and swing the B axis to B 90)

The tool will neatly arc down into position above where you want to make your cut. You can reverse it to come back out for your next tool.

Your machine might not collision check the tool path, so use caution.

See the program sample as an example. Unit 7 arcs the tool into the cut, unit 11 arcs it out, unit 12 arcs the next tool back in. It works really sweet, and saves a lot of time.

If you are having issues cutting your fist 5 axis part, download this simple EIA program and try to run it. If it throws up an alarm, you likely have a parameter issue that needs to be resolved before you will be able to go any further.

You need to program true 5 axis moves in EIA, since there is no way to do it in Mazatrol. Good Luck!

Integrex MK-IV Alignment Procedure

Integrex MK-IV Alignment Notes

Mazak Applications Alignment Training Manual for Integrex MK-III Series

The manual for the MK-III series is useful if you have an older machine, but also helps users of the newer versions, since it gives you a good overview of what needs to be done.