What's new
What's new

Mazak Mazatrol CAM T-2 Question - MNP Process

Pete Deal

Stainless
Joined
Apr 10, 2007
Location
Morgantown, WV
I have generally been parting off using a manual process so I can also chamfer the back side of the part during part off. Using a 3mm groove tool. I changed this process for a part I am now working on to put a 0.03" radius on the back side instead of a chamfer- Using G03. It gives me a "Illegal G Code Input" error. If I change the G03 to a G01 it makes a 45 degree chamfer. What am I doing wrong? (Photos Below).


IMG_0359 (2).jpgIMG_0358 (2).jpgIMG_0360 (2).jpg
 
Pete, you can do this with grooving process... No need to punch in all that manual code.

Make two grooving processes.
First, you make a shallow type 1 groove just to get your chamfer or radius on the back edge.
Start X is the part OD. Remember that type 1 grooves are measured Z on the part side of the tool (don't add tool width).

The second is a type 0 groove with 0 finish allowance.
Remember that type 0 grooves are measured z on the chuck side of the tool (add tool width to your groove Z point).
Start X = <final X from the type 1 chamfering groove> and final X = <part ID or 0 if solid>.

Here's an example from one of my programs...
Notes:
Process 12 is my type 1 groove with a 0.030" corner radius (It's only 0.040" deep).
Process 13 is the type 0 groove, note the tool width (.120") added to Z. (I cut down to 0.2" diameter).
Process 14 is the actual cut-off (I slow it down so the threaded aluminum part comes off with less energy).

IMG_2462.jpg
 
Thanks Chris I may change to that. I originally started parting using the manual process instead of the groove process to keep the spindle speed under control so parts would not fly all over.

I am still bugged that I can't make the G03 work. Tonight I went back out and deleted the whole thing and reentered it, made a new program with just a few manual processes using the G03 and was not able to make it work any how any way. There is obviously something I am missing.
 
Thanks Chris I may change to that. I originally started parting using the manual process instead of the groove process to keep the spindle speed under control so parts would not fly all over.

I am still bugged that I can't make the G03 work. Tonight I went back out and deleted the whole thing and reentered it, made a new program with just a few manual processes using the G03 and was not able to make it work any how any way. There is obviously something I am missing.

Try the 3 grooving process method I showed, I think you'll be happy with it.

On the G3 issue, I'm no wizard in manual process on our mazatrol machines, but I'm fairly savvy with g-code on the milling machines and program way too much of my milling that way. Your code looked good and I couldn't think of why it didn't work. So I just tried something similar with a clean program and got the same error message you did when I ran program check. So I started playing around, tried incremental moves instead of absolute... Same error.

Then, I cleared it all and started again. I figured out the issue. You can't have an offset line on a G02 or G03 line for some reason. Here it is working (at least in program check):


IMG_2695.jpg
IMG_2694.jpg
 
That's good to know! Thanks for working through that. I did try incremental too but not removing the offset number.

One thing, I think a lot of what I have typed in is not needed. I need to experiment more. I think the feeds and speeds may be modal and only need to be entered at the top of the process.
 
That's good to know! Thanks for working through that. I did try incremental too but not removing the offset number.

One thing, I think a lot of what I have typed in is not needed. I need to experiment more. I think the feeds and speeds may be modal and only need to be entered at the top of the process.

I'm pretty sure you're right about everything being modal.
I put it all on every line like you did.
 








 
Back
Top