Page 2 of 2

Re: Pocketing with different tools

Posted: Mon Feb 09, 2015 10:55 pm
by kiark82
Hans wrote:This isn't exactly just rough with one and finish with another, because you'd run into massive tool engagement in the corners. What I think you want is "rest milling" or "remaining stock machining". I've only really used MasterCam and HSMworks, both have this capability. Info page: http://www.hsmworks.com/docs/cncbook/en ... ESTMilling
yes, rest milling it is, thanks for the right explanation. ill have a look into those two programs
Hans wrote:You could do it manually on the cheaper programs if they don't have it. That is, manually sketch up the remaining material to take out of the corners. At least you could use HSM-style toolpaths with lots of flute engagement and small WOC since the rest of the pocket is already to-depth.

EDIT: How small of corners do you need? I don't think the MRR really improves on a Shapeoko beyond 1/8" endmills. Maybe you'd be better off cutting slightly-relieved corners instead and saving yourself a manual tool change and setup.
it really depends. mostly the corners are ok for a 1/8 mill, but pocketing everything with it already needed 2 hours lately, so that changing inbetween would really improve my working speed.
DanMc wrote:So I just did a quick test in CamBam and in theory it's possible to cheat it, it's a bit of work so it might not be a real time saver.

My steps:
1)produce an inside profile cut of just one layer with the larger tool size
2) toolpath to geometry (make sure the polyline is closed)
3)delete rapids
4)select original geometry and the converted toolpath geometry and create a pocket op

you could play with the tool size in step 1 or do an offset to reduce redundant milling, just don't make the remaining space too small or CamBam will think it's too small for the second mill to fit in
thanks for the idea, ill try that out next time!
PsyKo wrote:You can also do the inside geometry (the one you're doing with the toolpath to geometry) with an offset operation with negative value. It should be faster than doing it with the generated toolpath.
i need to have a look at that too, thanks... have to read alot about offsets first though :)

Re: Pocketing with different tools

Posted: Mon Feb 09, 2015 11:24 pm
by DanMc
@PsyKo - I tried that but on square corners the offset is still square. In the interest of minimizing air-milling or overshooting a corner, I opted to use the tool path instead. When there is a larger difference in size of the two mills, tool path would save milling time, your method is obviously easier where the mills are closer in size.

Re: Pocketing with different tools

Posted: Tue Feb 10, 2015 7:45 am
by PsyKo
DanMc wrote:@PsyKo - I tried that but on square corners the offset is still square. In the interest of minimizing air-milling or overshooting a corner, I opted to use the tool path instead. When there is a larger difference in size of the two mills, tool path would save milling time, your method is obviously easier where the mills are closer in size.
Agreed. Didn't think about that corner issue.

Re: Pocketing with different tools

Posted: Wed Feb 11, 2015 9:12 am
by Brian Stone
I haven't experimented with it much, but Autodesk Fusion 360 can do rest milling for pocket operations.