[CNC-Dude]

I need to cut a disc which measures 18 inches in diameter. The Tormach PCNC table can tackle this in the X axis, but the Y axis is not big enough. If I place my rotary table flat on the XY table (instead that across the A axis), I can enhance the cutting space and cut this disk without having too much on either X or the Y axis.

How do I configure the rotary table to be flat on the table within Sprutcam? Can this be done, or am I tripping? I know I can do this manually, so this is an option, but if I can automate it, then even better!

Thanks for your input!

[saabaero]

It might be easier to code this manually.

Just set your Z position to the initial cut height and then rotate the A axis 360 degrees. Advance the Z axis to the next depth cut and rotate the A axis 360 degrees again. Continue until you have your final cut depth.

Sample:

(the normal setup lines)
G00 Z.020 (rapid to Z safe height)
G01 Z-.125 F 25
A360
Z-.250
A360
...

Or you can ramp through the part using a helical move:
G00 Z.020 (rapid to Z safe height)
G01 A360 Z-.125 F25
A360 Z-.250
...

or
G01 A1440 Z-.500 F25 (4 helical depth cuts)

[CNC-Dude]

Saabero, thanks for your answer!

To make the disc in the manual fashion seems easy enough. What worries me is all the other features in it. There is a bunch of holes and pockets which would require a fair amount of programs in between manual table moves. Seems to me the resulting parts will not align very well if not done in a single run.

There is not a lot of information on the web, which is always the case for these kinds of intricate matters. However, I did find a post in which a gentlemen offered a machine setup file which apparently does this. The attached ZIP file was corrupted so could not validate this, though. Still I am hopefull there is a way to do this.

[Scott_M]

I played with it a little bit. I could not get the "Tormach" to do it. So I changed machines to 5-axis milling machine ( table A-C ) and it seemed to simulate correctly but the Tormach Post Processor only output X and Z moves ( no C ) It would probably work with another post Processor. You will need to find one that knows what "C" is. I would start with Fanuc PP's

Scott

[CNC-Dude]

Hi Group,

I contacted Tormach and Daniel Rogue was more than quick to send me the machine details along with superbly accurate install instructions. In less than 10 minutes I could see the simulation cutting my piece just like I had envisioned it.

You have to enable Polar Mode at the Rotary Transformation for the Contour operation, or the table will try to take the cut through XY which is obviously not possible.

I truly want to thank Tormach and Daniel Rogge for lightning fast response!

[spacemanspiff]

Hi Group,

I contacted Tormach and Daniel Rogue was more than quick to send me the machine details ...

Avayan,

Did they send you a file reorients the 4th axis displayed in Sprutcam so it is flat on the table? If so, could you post the file? Thanks!