On a rotary 3D carving project, the machine failed six times. The first two times I pushed a long 1/2" endmill too fast, too deep. The endmill stalled in the wood, slipped down from the collet, and lost z-height - my fault. On the second stall, the collet significantly tightened down on the slipped bit - nearly too tight for me to loosen it again. However, after getting it off, I blew out the dust and did not notice any damage to the collet.
I swapped that 1/2" endmill with a 1/2" ballnose and tried 3D roughing passes in a raster (not z-level) toolpath. This caused the next four failures. I do not think that they were due to the feedrate, as it was slow - about 100 ipm. I have run the same endmill at 200 ipm for raster passes before without issue. The stepover is also small - about 10-20%. Each time, the z-axis lost height/ did not retract up properly/ during the program and carved into the stock too deeply. After each z-axis slippage, I re-zeroed the ballnose. It does not appear that the ballnose slipped in the collet like the first two failures, which means that the z-axis lost height somehow.
After reviewing the four ballnose failures, it appears that the issues occurred during the U-turns of the back-and-forth passes of the 3D raster toolpath. Further, it appears that the z-height loss happened when the U-turn occured when the bit has just dipped into a valley and then tried to lift back up out of that valley right at that U-turn. This is the point where the bit is engaged with the wood 100% in a frontal cut, not the 10-20% stepover side cut. When the endmill does a U-turn where there is no material at the turn (zero frontal engagement), the slippage does not seem to occur. But then, it also seems like the z-axis height loss might also happen when dropping down into a valley and back up in the middle of a raster pass.
I don’t know if the pull-up shear against the wood is too great for the z-axis motor to overcome (doesn’t seem like it should be), if the z-axis movement is too fast for the Mach 4 vs the x-axis movement (doesn’t seem like it should be at my slow feedrates), if there is bind/pinching caused by the rotary rotation reversing against the bit during the U-turn (as my raster passes are on a 45-degree angle against the baltic birch veneers), or somethine else.
VCarve Pro was used to generate the toolpaths.
Various posts have discussed frayed cables, bumped cables (not the issue), z-motor brakes (no idea how to check this) or tolerance and smoothing in Fusion 360 (not using that software), or Mach 4 lowered acceleration settings (I am using the defaults).
Any knowledge what is causing this and how to fix it?
Thanks,
Matt
The core of this particular issue is command throughput. In Fusion, tolerance and smoothing is a good way to solve it. It could potentially happen with any CAM program, though. The problem happens in regions where the G-code contains many very small steps, and the command buffer in the controller can’t keep up with the physical motion of the machine. If you see a lot of small steps in the relevant sections of your G-code, then look for a way to fix that within VCarve.
It might help to post the G-code at and around the U-turn.
Last time I had this type of problem, it was because it was a new bit and I hadn’t cleaned the shipping oil off it. A bit of acetone on the collet and bit and the problem went away.
Have you measured the bit stick-out before and after to rule out slippage?
I do a lot of 4th axis work so I know it can be done. In the beginning I kept forgetting to use the right post processor. I wish I had more to offer. I use Aspire .
Thanks for the tips; I’ll try some acetone on the first bit (the 1/2" endmill), as it was a new bit. I’ll also try to measure the stick-out for next time.
However, the 1/2" ballnose that lost z-height four times was an old bit. Considering its first three slips were 1/4" each, and the last one was 1/2" of height lost, that ballnose did not slip, as it looked like it was in the same position as it was initially, not 1-1/4" down.
If the new bit left oil on the collet, that will affect every bit after it. Clean everything.
Thanks for suggesting a likely cause. VCarve is a bit weird in that it’s not a pure-geometry program in calculating its toolpaths. 3D models are converted into grayscale heightfield image maps which are then used to calculate the toolpaths. So resolution of the image map determines how accurate the toolpath is. There are Standard, High, Very High, Extreme, and Maximum model/image resolution settings. The Maximum resolution setting was used for my files; but of course, while being most accurate, it also generates the smallest line segments. That could cause the issues you are talking about.
After your post, I found the 2D/ 3D/ Vcarve toolpath tolerance settings in the Options menu. Like the Avid video here: Z Movement loosing steps, reproducable any height, with this code - #11 by Stephen , the VCarve default settings were 0.0004".
While they can be tolerance-reduced, Vectric told me that 3D toolpaths cannot normally be “smoothed” into efficient arcs (rather than polylines) as in Fusion’s setting because 3D toolpaths generally are not XY arcs but move in all three directions.
I made a tiny toolpath area and gcodes for the Standard, Very High, and Maximum resolution settings, with the default 0.0004" tolerance. The gcode file sizes were 15kB, 22kB, 27kB.
After I changed the tolerances to 0.001" I resaved the test toolpaths. The Very High decreased to 16kB (barely over the Standard default), the Maximum decreased to 20kB (smaller than the Very High default).
Unfortunately, I do not know how to re-import gcodes back into Rhino so I can look closely at the tolerance-reduced versions vs the default versions to see which is smoother or has fewer tiny segments. The files are attached. My hunch is that the issue might not be the U-turn at all, nor the drop (perhaps) but maybe the round-over from the plateau into the drop.
Toolpath tolerance test gcode comparisons.zip (38.5 KB)
Hi Brian,
Within Aspire (which will be the same as VCarve Pro), what are your 2D/3D Toolpath Tolerance settings?
Also, when you set up a job, what Modeling Resolution do you typically use?
Hello Matt, I use the default on the tolerance (0.0004) I use very high on modeling res. And for sure if you don’t want your bust to split wide ass open, no matter what your moisture meter says DO NOT USE LOGS FOR CARVING.
Do a proper glue up of any hard wood. Use the gadget to do a rounding toolpath. Then import your model and rough it out I always leave 0.06 to 0.07 machining allowance , now it will give a warning that leaving that much for the finish bit to remove might be a problem, but for me it has not been, What is a problem is using the suggested 0.02-0.04, I would find places that the roughing bit cut too deep into the model.
I posted some more pics showing splitting when using logs, this won’t happen if you do a glue up.
