Title pretty much says it all.
I’m just getting into 4 axis machining on my 770M with my new MicroArc. Now that I better understand multi axis CAM (a little).
I’m trying simple cylindrical parts, using rotary tool paths and I’ve been looking at the Gcode produced.
I see that there is a lot of dithering going on in Z and sometimes Y when the majority of the motion is X (axial) and A (rotary) as one would expect. I’m guessing/assuming that this is because the tool path generator needs to work on parts that are not strictly cylindrical. That makes sense.
What I’m concerned about is I’ve enabled backlash compensation on my mill and this dithering will cause excessive directional changes which could be or is bad in the long run for the mill.
Is this a valid concern? I’m seeing 20 or more lines in a row where Z alternates +/- .0001, is that enough to make it add/subtract the backlash comp on every G1 command?
Is it worth investigating using smoothing and/or tolerance to reduce the dithering? Smoothing doesn’t seem to affect the dithering but does reduce the code as expected.
-Dave
David,
You should add some smoothing to get rid of those movements. Bearing brinelling is a deep rabbit hole, but the short version of it is that with small repeated movements the lack of lubrication will eventually cause wear. 20 lines of code is not near the point where wear would be expected but defaulting to having smoothing on is a good practice.
Backlash comp is automatically applied to every move.
Thank you,
Norman
In my limited experience for A axis tool paths looser tolerances = smoother more efficient cutting. Also the A MicroArc is not a tight tolerance workholding. It holds tight but I have a hard time holding tolerances of .025mm unless it’s super light cuts right on center. The fewer axis you have involved in The cut the better your result will be. If your rotating and moving x and y it’s going be low tolerance. I have found that if you leave a little more on the roughing allows the finishing to keep more engagement resulting in a nicer finish. It’s a slippery slope.
Thanks for the quick response. I’m glad that my intuition was correct.
Clearly this problem is with the Fusion tool path generators and how they handle generic 4 axis programming.
To be clear:
Smoothing doesn’t really change the problem (at least as implemented by Fusion). I have a .nc for a short rotary path (1” diameter, about 1” length with 3/8 end mill). It has about 720 lines of G1 to spin and advance X. Almost all of them contain a Z where the Z difference is .0001
Not Good.
What I’ve found is cranking the tolerance down to .0001 (lowest accepted by Fusion) all of the Z moves disappear. My guess is that what happens is the tolerance forces the Z values to be the “same” as the difference is below 0.0000 truncation of positions I see in the NC file.
This extreme tolerance cause the file size to double even with smoothing.
I’ve done some more experiments with wrapping a 2D contour - this correctly produces a single Z but getting the full 360 to generate is kludgey.
I ran into a lot of this with fusion, using the g-code posted for the Santa stocking holder. Thousands of lines of code for a simple move where z comes straight down, stops and then A rotates only a few degrees. It added hours to a 8 hour program removing almost no material. I couldn’t try lowering tolerances because I don’t have the manufacturing addon.
These machines aren’t really 4 axis machines. I think the code is really having to stretch to accommodate the 4 axis moves. If you can, you are really better off doing complex 3 axis and just use the A for turning the part to the next position.