3 Photos:
3/4” birch ply, 3/8” compression bit. 360ipm @ 18k RPM, conventional milling
Is this bit deflection?
at 360 IPM it could be machine deflection, too, if the bit path is left to right to bottom. Or if you’re using servos they might need tuning to not go as far over their target. Either could be worked around by lowering your max acceleration in that direction so that the machine slowed down more for corners.
How to tell? Try running at 50% speed override and see if it looks better. If so, try to move the spindle by hand and see how much play it has. If it moves, find out why 
path is bottom to top in first two photos. Top to bottom in the last. I tried 75% speed and still had the problem. For scale, you can see the groove from the bit in the spoil board in photo 2. Spindle is solid as a rock.
I’m thinking maybe as the machine decelerates to go into the turn, and the feed rate decreases, the bit is springing back.
Hmm… maybe it’s a G64 problem?
What control is this on (Mach or EX?) and can you post the G code?
I don’t know what a g64 problem is. It’s a Mach4 system. Here is some Gcode:
Next time you can post G code files right here on your post
I checked one out and it looks like you’re using rounded corners:
This is fine (and probably the right choice) but it’s worth understanding what’s happening here:
Your machine is taking a small arc at each corner, this means the load is getting transferred from the X motors to the Y, and vica versa.
I believe what you’re seeing is some kind of mechanical looseness. Perhaps a loose belt, worn pinion (these are wear items). Could be loose bolts, worn bearing blocks, etc.
Point being is that his looks mechanical so I would start there.
There are some good tips here: Troubleshooting
It wasn’t a conscious choice. I used an ordinary outside profile toolpath in Aspire. I double checked the client’s drawing file I used, and the corners look perfectly square.
I will investigate this. Thank you.
It’s not he corners in the drawing, there’s a toolpath choice that will “round” corners or keep them square. You have chosen to “round” them in your toolpath, that’s why you can an arc’d corner and not a perfect 90 degree corner. This is a fine choice for cabinetry, and frankly most things wood. You get a TINY roundover on the corner, but the machine decelerates less because it’s not actually changing directions all at once, it’s rolling around a corner. This makes the machine run smoother and saves a little time.
I pointed this out because that oddity you’re seeing is presenting in a similar way to when folks try and cut a circle and it comes out as an elipse instead, it’s because as the X motors hand over load to the Y (and one of them is loose in some way) you can get that elipse.
It looked to me like a “go around the corner” toolpath that results in a square corner but avoids high acceleration in the toolbit. I.e. tool compensation was off and you’re viewing the toolpath.
My toolpaths are all like that - the bit follows a curve but the result is square.
This is the feature I am talking about in Aspire/VCarve:
When you have this unchecked the toolpath “rolls” around the corner. When you check it you get a perfect 90 degree corner, no radii.
Most people should leave this unchecked by default unless you have a specific reason to turn it on.
A small radius speeds things up and makes the machine run smoother. A true hard corner and slow the machine down.
It should also be noted on EX control the “smoothing” settings can also have some effect on hard corners (depending on how you have smoothing setup)
This feature is not available on Mach
Right, but with a straight bit that doesn’t affect the corner shape - you get a sharp corner either way, assuming vcarve is talking about making the bottom of the carving as sharp as the top, with a v-bit. A straight bit can roll around a sharp corner and still be moving “smoothly”.
As for mach, I thought it did support G64 smoothing?
This isn’t for VCarving, this is for a profile toolpath.
It does, but it’s not “S Curve”. That mode does work, but sometimes it can ignore some corners, and overly round others.
This is how the Centroid smoothing works, it’s quite a bit more sophisticated: https://www.centroidcnc.com/centroid_diy/downloads/acorn_documentation/centroid_gcode_smoothing_users_manual.pdf
What I was getting at was on something like that cabinet panel you could likely send it with non CAM rounded corners, pick a smoothing mode in Centroid (like “precision router”) and it would effectively do the same thing.
Do you need to do it that way? Probably not for panel processing, but if you did do it that way, all of your corner speed tuning is “on control” and something you can do on the fly, rather than having to re-post your G code if you want to try sharp vs hard corners.
Depends on your stick-out and width and depth of cut. If your stick-out is minimal, then tool deflection is probably not the main contribution.
Out of curiosity, what are your width and depth of cut, what spindle do you have, and what’s the model of the bit? A cutting feed of 360 ipm is pretty aggressive for this machine and for most spindles and bits you would use with this machine.
If that were the case, wouldn’t you see deflection after it got back up to speed after the corner? I see significant deflection on one side of the cut and none on the other. If it happens in one axis but not the other, then it suggests a mechanical issue.
With the right drive system, bit and hold down you can cut like this.
Not necessarily…
When closest to the corner the bit is moving slow, and then it speeds up. If there’s mechanical slop the bit could be getting sucked closer to the work when it speeds up (depending on cutting direction)
so maybe I can test this hypothesis by cutting some circles and measuring them
That would work, or just checking the machine for slop/worn pinions would be good way to go. With an error like that I suspect if you put a tool in the spindle and grab it with your hand, or lock up the steppers and try and push the machine back and forth on each axis you’ll find the culprit very quickly
full width, 3/8”. 3/4” deep
8.7hp
Onsrud 60-123MW
Onsrud’s data sheet recommends running it at 567 ipm. It likes to run fast to dissipate the heat.
When I grab the spindle or the gantry and just apply back and forth pressure, I feel no slop. Is there a more scientific way to do this? How do you lock the steppers?
You can start here:
The test I like to do to check for worn pinions is to look at them first to see if you see wear, then I like to leave the machine idle and get my hand/thumb touching a moving part of the machine and a fixed part of the machine, this is pretty easy to do on X and Y. I can usually do this with my thumb.
Once I do that I push and pull the moving part of the axis back and forth with rough 20-40 lbs of force.
In my thumb I’ll be able to feel if there’s any detectable slop in the pinions.
It’s also worth checking to see if your hold down is good, your machine frame is tight, and in general to see if anything else is really loose.
You could also back off your feeds somewhat after you’ve ruled out mechanical stuff.