Question About Carving Outside the Material

[desert-rat]

I am carving a simple sphere.  Two-sided job.  I want the biggest sphere I can get out of the material (expensive material), which is 2 15/16" diameter.

1/4" EM roughing.  1/4" BN finishing.  

I am using a boundary offset equal to the bit diameter so I can carve around the sides of the sphere.  However, this boundary offset does not seem to work when I am up against the edge of the material.  The issue I am looking to resolve is that the software doesn't seem to want to let the bit move beyond the edge of the material so I can get a complete carve around the edges.  Here is a view of the toolpaths, which shows how the toolpath is not moving outside of the material:

This is leaving me with this:

I thought about changing the material size in the job set-up, but it seems like this could be problematic to ensure proper registration on the CNC.  I doubt I could get the material in the perfect position on the machine bed to compensate for this trickery in the job set up settings.

I suspect there is an easy solution to this.  Can anyone please help get me pointed in the right direction?

Thank you very much for any help.

Theodore

[Rcnewcomb]

For situations like this I first do a profile pass around the 3D design. I typically use a 1/2" end mill. I may do another pass offset outward even further if i am trying to avoid collet collisions.

[desert-rat]

After some additional searching, I think I found a good solution from Steven (@adze_cnc) and wanted to add it to this thread for anyone who might stumble on this in the future.

Basically, to overcome this, you would indeed change the material size in the job set-up, but the trick is to then (1) offset the X,Y datum position and (2) re-center your components in the material. These two additional steps allow you to still position the material at 0,0 on the machine bed.

Steven provided a really good explanation, here:
https://forum.vectric.com/viewtopic.php ... al#p301166

If anyone has any additional thoughts or a better solution, please step in. Otherwise, thank you very much Steven.

Theodore

[desert-rat]

For situations like this I first do a profile pass around the 3D design. I typically use a 1/2" end mill. I may do another pass offset outward even further if i am trying to avoid collet collisions.

Do you mean just to ease the roughing and finishing paths around the model? I had been contemplating this very thing.

However, I don't think it solves the problem from my original post, because although it might create my circle, it won't give me the 3D sphere shape at the edge, unless I am just confused about your comment?

Thank you for your comment Randall, I think I'll do as you mentioned.

[adze_cnc]

I think I found a good solution from Steven (@adze_cnc) and wanted to add it to this thread....

Excellent. Saves me searching for the that post to link to here. I hope that it helps. A generalized version of that is summarized here. At that post I suggest making the XY dimensions arbitrarily 2 inches (50mm) larger as the amount of "fake" material doesn't actually mean anything as long as it can fully contain the toolpaths.

For deep cuts like this I also will run a profile pass and stop short of the full depth. Primarily that's in case the finishing path offsets causes it to crash into what the roughing pass doesn't cut.

[martin54]

If you want to work within the software then using the offset will work as has been said, also using the material centre rather than the bottom left corner would work.
I have worked at the machine in the past rather than use the offset within the software. Easy enough to zero your X Y position as normal but then change the DRO setting within the control software from zero to the offset value but that might depend what control software you are using for your CNC