Mazak Post

[pip]

Has any one used the Mazak post from the V8 disk, and with any joy. We have a VQC 15/40, and would like to try some 3D machining on it, using Mastercam V8. Any advice appreciated.

[Mark H]

I am using the Mazak post off the V8 disk. I did make some minor changes to it. The main thing that I had to changed was how the G28G30 was handled. I changed it to work how the Mpfan.pst works - mi3 sets G28 or G30.

I succesfully use the post on the following machines;

• Mazatech FH-6800 with Mazatrol 640M PC-Fusion-CNC controller
• MTV 515/40N with M-plus
• VTC 16A with M-plus
• AJV-35/60 with M-32

Other changes that I made, but may not be necessary for your application;

1. stagetool = 0 (The VTC16A did not like it)
2. Q. 164 = n (disable 4 axis, again VTC16A)
3. Force default WCS to be G55 not G54 (one of our very old M32 controllers would not properly reset the G54 after my EIA program was completed. So when a Mazatrol program (conversation program) started, it did not have the correct WCS. But this was a problem only with one of the old M32 controllers, all the new controllers handle G54 correctly.)

[Mark H]

One thing that I forgot to mention...

The Mazatech FH-6800 with the Mazatrol 640M PC-Fusion-CNC controller does not like the "%" at the beginning or end of the program. The program would not run at all and the controller did not give any warning, it just sat there no matter how many times I hit the cycle start button. All of the other controllers want the "%". I'm sure it is just a setting in the controller's parameters, but I haven't had a chance to look into it. So what I do is post the program and if it goes to the FH-6800, I just edit it and delete the "%".

[This message has been edited by Mark H (edited 03-12-2001).]

[pip]

Thank you for your help, we are going to try the post this week.