Cancel
Showing results for 
Search instead for 
Did you mean: 

Drilling rotating C axis

Solution Partner Pioneer Solution Partner Pioneer
Solution Partner Pioneer

Hello everyone

 

I'm trying to run a Mori Seiki mill turn machine with y axis, and I have a problem when I try to drill on a radio.


What happens is that instead of positioning in X and go moving the C axis at each point, it makes XY is positioned at each point.

 

How can I do to fix the XY and just go by rotating the C at each point?

 

Thank you

 

Forget clarify that tried and using the UDE "Lock axis" and it was not successful

9 REPLIES

Re: Drilling rotating C axis

Phenom
Phenom

What post are you using? Is it a linked post - and has a mechanism to change kinematic modes (like a head ude?) Some posts may have an XZC linked post you can switch in and out of. It is all dependent on the particular post. Locked axis can be made to work - but that again depends on the particular post.

NX10.03
Windows 7 Pro

Re: Drilling rotating C axis

Solution Partner Pioneer Solution Partner Pioneer
Solution Partner Pioneer

Hi, thanks for your answer.

 

I'm using an custom post, its is a linked post, one for lathe, and another one for milling.

 

I'm trying to modify the post to work properly in all cases.

 

To switch between post i define the UDE Head, asi mill or turn.

 

So, what you mean is that i need to build another post whitout the Y axis for this type of case?

It is not a issue of the NX?

 

Excuse me for my bad English, I try to make myself understood.

Re: Drilling rotating C axis

Esteemed Contributor
Esteemed Contributor

The easiest way is to have 2 mill posts - one with the Y axis, one (an "XZC" post) without.

 

You can use the "Set Polar" UDE to modify things as well, but then you may have to get a bit fancier with the post.

 

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Drilling rotating C axis

Valued Contributor
Valued Contributor

Just to make sure, did you align your drill vector normal to the surface? I don't have the experience as the two who posted earlier, but I don't recall having an issue with XZC with drilling on my post. It only outputed a Y move if the tool vector didn't intersect the z axis.

Using NX 8.0.3.4

Re: Drilling rotating C axis

Solution Partner Pioneer Solution Partner Pioneer
Solution Partner Pioneer

I've just discovered that is a problem of the postprocessor.

 

I got the same Operation, and postproceced it with the demo "MILL TURN" (in NX9) postprocessor and I got a right code, rotating C axis.

 

So, the demo post "MILL TURN" is a single postprocessor for milling, could i copy a command or some else of this post and put it into mine to worked well without making several posts?

Re: Drilling rotating C axis

Phenom
Phenom

In the postprocessor directory - there is a post called "millturn_baxis_5axis" - is this the one you are referring to? If so - the mill kinematic setting is "5_axis_head_table" which I haven't used but it would use tool vector to spin the table (C) for your drilling. Check to see that your mill post has this kinematic. Look for the following line in the tcl:

 

set mom_kin_machine_type                      "5_axis_head_table"

 

XZC mode would be for drilling in the face in XY plane - I didn't catch that you were drilling on outside of cylinder.

NX10.03
Windows 7 Pro

Re: Drilling rotating C axis

Solution Partner Pioneer Solution Partner Pioneer
Solution Partner Pioneer

No, the post that I used is millturn_3axis_mill.

 

I'll find in the TCL for some similar code, on both posts

Re: Drilling rotating C axis

Phenom
Phenom

Ok - I opened it - I don't have experience with that kinematic. Still I would expect the tool vector to drive C - so if your hole axis is on center of the cylinder - it should leave Y at zero.

NX10.03
Windows 7 Pro

Re: Drilling rotating C axis

Genius
Genius

Hi,

 

Create one more linked post using Mill turn option in post builder (XZC). Use appropriate HEAD so that NX selects this post when you post process your operations. This should solve your problem.

BR
Mak
TC10/NX 9

Learn online





Solution Information