Did a small (8") dome using the “offset strategy” where the bit starts in the center and works its way out. 1mm radius tapered ballnose, removing -at most- 0.04" doc. 18,000rpm, 60ipm in x,y,z axes. Did my roughing pass first so I’m not stressing the bit or machine at all.
Anyone else have this problem;? Suggested solutions?
(Using the Avid Benchtop Pro, NEMA 23 motors, Avid DIY electronics, ethernet smooth stepper, with 2.2kh water cooled spindle, Vectric Aspire 11.5, Mach-3. Windows 7 on an old Dell desktop.)
In F360? Try turning smoothing on and ratcheting it up to .005” and turning the tolerance down a bit.
If you are climb milling, I have sometimes found that conventional works better for light step over finishes.
Also, if you have more rpm in the spindle, use it. Bullnose cutters have essentially no radius at the center, so you’ll want to use all the speed you can for finishing passes.
When it is running, can you see, feel, or hear the chatter? Can you see or hear it when you are cutting air? That chatter looks like resonance, not tool chatter, IMO.
Last, post your motor settings, specifically, let us k ow if your z acceleration is less than your x and y. As a rough rule, and in my opinion, all your accelerations should be as high as your finish feed rate for a surfacing cut, and they should all be the same. That, plus Constant velocity mode is the biggest help IMO.
Well, I use Vectric’s Aspire so I don’t know about smoothing settings. My Modeling resolution is set at “Very High” I do use climb cutting rather than conventional. I suppose I could ramp up rpm and ipm and see if that helps. I do feel/see the vibration in the machine. Haven’t tried “cutting air”.
I’ve never had a problem with a pocket cut using the “offset” cutting strategy so wonder if it’s an issue with 3D modeling.
I see roughness that seems to be part of the model around the geometry of the parts in the simulation. Are you talking about the tool marks in the "flat regions?
What diamater bit are you using. it looks like you used a ‘radial’ machining tool path from the tooling marks. first of all 10% is most likely too large a stepover, reduce it. second move to a spiral machineing tool path as itll give you an constant stepover. the radial pattern is great in the center of the part but gets gradually worse as you move to the edge of the part. I do a lot of dome shape machining building archtop guitars and find that a stepover of 3-5 % work better depending on bit size.
When you are surfacing a 3D part, all three axes are constantly accelerating (there is basically always some direction change happing)
The surface is made up of a series of moves in segments generated by the CAM software.
In Mach, it does it’s best to keep the transitions between each segment smooth by using an algorithm to allow slight deviations from the path the CAM generates in order to keep cut speed high and not bring the machine to a full stop at the end of every segment.
The problem is that if your z axis acceleration is 20 and your x and y are 40, you might find situations where x and y have to slow down to wait for z. These moments of “waiting” are what I believe your are seeing in your part.
Constant velocity helps, but ultimately it is dependent on the motor capability. Try setting all your acceleration the same - bring your z axis accel value up to match x and y.
Also, if your peak z speed is much lower than x and y, bring that up a bit (and be careful when jogging!)
Which parts were imported vectors and which parts were originally drawn with Aspire’s built-in tools? Are you using ‘Fit Curves to Vectors’? I’ve seen un-smooth vector drawings downloaded from the Internet produce un-smooth cuts (for example) - it gives what it gets.
I personally don’t think we have enough information to be making configuration changes just yet.
