Milling with C axis on a 5 axis machine.

[civiceg]

I am trying to mill a round bore with the C axis rather than interpolate with the X and Y. This is not practical at all, but it there a way to get MasterCam to output no x/y moves and just rotate the c axis to bore a hole? I am trying to have my file all done it MasterCam without any hand programming. 

[jlw™]

Axis sub or 5 axis path with limit on Y.

 

I have my post configured so that I can do it with axis sub. Much faster, create a 2d path of what you want hit the axis combo page and hit radio button for 3 axis.

 

 

What post are you using?

[civiceg]

UMC 750 

[jlw™]

I'd try axis sub to see your output. If it's a no go, 5ax path.

 

Can you upload a file?

[civiceg]

Axis sub was a no go when I first tried it, still have not ruled it out, playing with 5axis options as I find time. This has been on my back burner of things to do. 

[crazy^millman]

Axis Sub should do it with no problems you would think, but they don't work. Not sure if you are using a 3rd party post, but I am not aware of and CNC Software post that will support it. I had to cheat not to long ago and make a 4 Axis post give me the output I needed to do exactly what you are after.

[David Colin]

Look if you don't have polar interpolation mode with M/G code on your machine. Thus, you program G1/G2/G3 X Y Z as usual (sometimes swapping Y address with C address) and machine is making Y substitution itself. On our Mazaks we are using G12.1/G13.1 but machines usually are using G112/G113

[civiceg]

Not supported on Haas mills

[David Colin]

Then I think you ll need to do it with a 5axis toolpath or make important PP modifications for 2D contour toolpath...

[Guest]

Not supported on Haas mills

That's not entirely accurate. AFAIK getting MC to post that code is one thing, writing a cycle manually is another. I have done precisely that on a UMC and of course Matsuura. The Matsuura I did just a spiral contour and told CAMplete to lock X, move Y and spin C. It's bad@$$!

 

FWIW, CAMplete Truepath is available for Hass UMC-750's. :

 

[David Colin]

To tweak your Mastercam post shouldn't be that hard...

You'll need to break arc(s) of your 2D contour toolpath. This can be easily done using linarc$=1 switch (with a chord_tol$ value). Then it will be easy to calculate polar angle from x/y locations.

[Matthew Hajicek - Singularity]

If you just want it in the Mastercam file such that it posts out with the rest of your program you can use a Manual Entry op to insert handwritten code.  You can then use a dummy op that moves in XY for verification and stock model updates; post-ghost it before posting.

[MrFish]

We get this to work by creating a dummy operation and saving the back plotted tool path and then using this as the drive geometry for the operation with axis sub turned on and set to 3 axis. Works great in our DMG with C axis table.

 

PM me your email address and I'll send you an example if you need.

[Mick]

We get this to work by creating a dummy operation and saving the back plotted tool path and then using this as the drive geometry for the operation with axis sub turned on and set to 3 axis. Works great in our DMG with C axis table.

 

PM me your email address and I'll send you an example if you need.

 

Maybe I'm missing something, but why don't you just draw the geometry? What does the saved backplot geometry give you? I think the op is just wanting a ramp on bore, with Z/C rather than XYZ?

[MrFish]

Maybe I'm missing something, but why don't you just draw the geometry? What does the saved backplot geometry give you? I think the op is just wanting a ramp on bore, with Z/C rather than XYZ?

Not sure why but if you just turn on axis sub with a normal op using standard geo we don't get any axis sub at posting. But if I do it this way we do. May be a post configuration thing .

[MrFish]

Not sure why but if you just turn on axis sub with a normal op using standard geo we don't get any axis sub at posting. But if I do it this way we do. May be a post configuration thing .

scrap that, just tested again with latest post and worked fine on original op with axis sub

[civiceg]

 

 

That's not entirely accurate. AFAIK getting MC to post that code is one thing, writing a cycle manually is another. I have done precisely that on a UMC and of course Matsuura. The Matsuura I did just a spiral contour and told CAMplete to lock X, move Y and spin C. It's bad@$$!

 

He was talking about the control converting X/Y moves to C axis moves, lathe sure, mill not so much. Writing the cycle manually is not the problem, getting it done inside Mastercam without a workaround is. 

[Guest]

He was talking about the control converting X/Y moves to C axis moves, lathe sure, mill not so much. Writing the cycle manually is not the problem, getting it done inside Mastercam without a workaround is. 

 

Ahhhhhh. I see said the blind man to his 3 deaf children who picked up the hammer and saw.

 

I thought he said the machine could not do an X/C, Y/C move. Missed it.

 

[civiceg]

All good, 4 axis post, change machine definition for the rotary to revolve around the z, and axis sub using 3 axis output. Just what I wanted. 

 

 

I can see how doing this is extremely post dependent as I get varying results using different 5 axis post. 

 

 

Thanks for all the input!!!!