So ive had my cutter get stuck essentially while moving in the direction of the previous cut after getting to a certain depth and then moving through my work piece after it thinks it moved enough. This has o ly happened with deep (3/4-1in) contour cuts with my compression bit. I need a way to reliably make these cuts though. I was thinking id compromise the final quality and just do a bit more sanding by getting an upcut bit but im not sure it will be enough and it will delay my project about a week while I wait for the bit. I also thought about babysitting it during the final cut out with the air conpressor. Anyone have other ideas?
What are your feeds and speeds and depth per pass ?
The top section of a compression bit is downcut so indeed it will tend to push chips down the slot. You have basically two options:
- use a shallow depth per pass, preferably with an upcut endmill as you mentioned, and once the profile cut is completed you can change to the compression endmill run a single contour path at full depth with it to clean-up the edges in one go.
- add extra geometry outside the profile you want to cut (say, offset outwards by half the cutter diameter) and cut as a pocket. That way there will never be a deep slot, but a deep pocket, and that makes a world of difference since chips will have somewhere to escape to (the part of the pocket already cut), rather than being stuck at the bottom of a slot that is only as wide as the endmill.
1 Like
I thought about using the extra geometry method. I’ll do that for now, and probably a shallower depth of pass too, and get then upcut bit for future tasks. Thanks. Feeds and speeds where pulled from the amana tool site (110 FR 18000rpm)
1 Like
Beware that while RPM and feedrate are usually spot on if you follow their recommendation, depth per pass is another story. They tend to recommend a depth of cut better suited for heavier machines than Shapeokos, so it’s usually a good idea to run at half the depth per pass they recommend or so.
3 Likes
Your Depth of cut is beyond what your machine can handle.
Consider what keeps the machine in place as far as bearings and rails;
There should be a calculator somewhere on the internet but basically you only wanna max your depth of cut at 10% of what your bearing size is.
Unless you have a way to measure the torque that your motor is asking for when you get stuck;
If you dont have a way to measure torque during cut, then it is a good idea to use a piece of scrap to dial in.
On new material I will cut several y axis lines and x axis lines to dial in speeds and feeds and DOC;
I will cut circles, squares, triangles, and adjust from there.
Goodluck
The reduction in cut depth and extra geometry worked to get the prototype i needed done today but im having trouble with the wood splintering rather than cutting at times. I wouldnt think the cutter is too dull because i havent had it long and its amana’s solid carbide 1/4in compression bit. Ive had it maybe a month with roughly 30hours cutting time. Mostly mdf if that matters. I just moved to real wood this week.
Try climb cutting instead of conventional. If you must use CC, Offset your profile outward by 0.250", and then again by another 0.050" (0.300" from part). Contour the 0.300 curve. It will conventional cut your line, but the opposite side of the bit near the part will climb cut and leave 0.050" for a finish cut. Then do the same with the 0.250" offset line to climb cut the finish cut.
Okay thats makes sense from what little i know about climb cuts but im a bit lost on how to get it done. Whats a good alternative to cc? Because I’m not sure i understand exactly what to do to get the climb cut.
Black is your outline you want to cut.
Offset that 0.250" (Green)
Offset that one (should still be selected) another 0.050" (Red)
Now contour/profile the red line (inside) using a DOC on the tool
Then contour the green line using a deeper DOC or Full depth.
The area between the green & red line is now gone, so you are only cutting with one side of the tool, and only removing 0.050. Climb cutting pushes the material into the part rather than pulling it away & chipping it out.
1 Like
Okay. That makes sense, yeah. Still open to ideas beyond CC though. Im sure im going to out grow it eventually but you’ve been super helpful.
Also check the cutting length on the bit. You should have a bit that has a cutting length greater than the depth of your cut. When the cutting length is shorter than the depth of cut the chips can pack in the cut line and cause all kinds of problems. If you are not removing the chips completely when cutting this adds to the force needed to move the bit in the cut.
MDF will dull a bit quickly
What material are you cutting. I have had good results using up cut bits in Maple and mahogany.
Anthony
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.