Cross drilling in lathe

[mats_asson]

I'm still working on my Index G200 post. I have a problem with cross drilling. It seems that it always drills through the center of the part, regardless of my tool plane and rotary axis settings. The only way I can get MC to do a hole off center is to uncheck the rotary axis button. But when I do that MC splits up the drill move in small steps. And when I look at the drill op again the rotary axis button is checked again, autmatically. Anybody aware of the problem? The problem seems to be regardless of what post I use.

A bit hard to explain.. maybe I should upload a sample somewhere...

Mats

[Guest CNC Apps Guy 1]

Yes. please upload a file to CADCAM's ftp site.

ftp://www.ppcadcam.com

User: mastercam

Pass: forum

------------------

James M.

Mastercam Enthusiast

[Allan Brown]

Cross drilling under the C-Axis toolpaths is meant to drill on centre with out setting toolplanes. Use Mill drl under the same menu to use Mill drilling (requires Mill on the same seat of Mastercam).

[Guest CNC Apps Guy 1]

DOH!!!!!!

Once agin the obvious is overlooked. I hate when that happens.

------------------

James M.

Mastercam Enthusiast

[mats_asson]

OK... done some more checking. I made a new file, built a new post from mplfan.pst with y_axis_mch=1 and mill canned drill cycles disabled. Made a mill drill op and a similar c-axis cross drill op. Unchecked the rotarty axis button in both. Posted. Both ops give the same result. I get y-axis output but the drilling is split up in several small moves. If I don't disable canned drill cycles it works ok, but I don't have those in my machine. I'm uploading the sample real soon now.

Regards...

Mats

 

[mats_asson]

There... the file is uploaded to the Mastercam Forum directory. Hope that's ok. If you want me to I can upload the modified mplfan post also. I only made the two changes I mentioned earlier though.

Mats

[mats_asson]

Forgot to tell you the name of the file... yaxdrill.mc8

 

Mats

 

[mats_asson]

And Dave... you are right.. I should use the mill drill. The c-axis cross drill keep setting the rotary axis button automatically. I see no difference though when setting y or c rotation type.

Mats

 

[CycleTimeCharles]

This is from the Help file.

"The Cross drill option also lets you choose arcs to select the drill points and direction. In doing so, the arc center defines the drill point and the arc normal defines the drilling direction. Choosing arcs lets you drill off-center, i.e., in a direction that is not towards the center of rotation."

I tried on Mats part and it waorked fine.

Since it uses the plane # of the arc make sure you draw the arcs in the proper view.

YAXDRILLUSINGCROSSDRILL.zip on ftp://[email protected]/Mastercam%20forum/

I also added a facing operation with multi-line comments and it comes out all on one line. Multi-line comments does work Cross-drill operation being a mill toolpath. Can you check it LutherHeggs?

 

[mats_asson]

Yes!

Thanks a lot! It works now! This is a great forum! It posts correctly also. Doesn't seem to work with mill drill though. I get split up lines with it. Don't really need mill drill though if cross drilling works like that. Now only the rest remains... (sigh)

Thanks again... Mats