Strange Issues with a 3D Adaptive toolpath.

[Benjammann]

Hello,

  I'm having two issues with a 3D adaptive toolpath that I'm trying to cut.

1. See video for strange jerky behavior that is occurring.

2. As the part is cut, the adaptive path seems to scale by .030" over 5 inches in the X-axis. Close to the origin my adaptive profile cut lines up nicely with some pre-drilled holes, but then on the other side of the part the cut is .030" off. Seemingly becoming more and more off as it goes to the right side of the part. I measured the holes and they are all within .001"  Any thoughts as to what could be causing this? Please see settings in the attached photo.

Thanks,

Ben 

[randyT9V9C]

What kind of machine are you using? I suspect your missing steps. Decrease your Optimal Load on the Passes tab. Typically, most tracodial paths use a chip load load between 10 and 20 percent. At present your load is 48% (0.09"). Decrease your load to between 0.02" and 0.03" and see how it goes.

[Benjammann]

I'm using a Taig Protomill 2000. So yeah, a bit underpowered. What's strange is that I've cut with those settings before and everything was perfectly smooth. I have since tightened up the table to reduce slop. Maybe that put more load on the motors.

So you suggest that I am possibly losing steps. Is the increased scaling over distance indicative of that? It wouldn't be the opposite? Where the commands were sent but due to too much load on the motor the table doesn't move as much as it should? I would think I'd see a scaling down not up. Is this not the case?

I've attached the file in case anyone wants to take a peek. It just seems like the adaptive operation is taking way too long. When I decrease the optimal load to .03 it then calculates to many hours rather than one.

EDIT: One thing I did just notice is that I had my no engagement feed rate set at 39. Could this be the cause of the jerky motion? It's trying to go really fast when not engaged and it can't handle it?

Thanks,

Ben

[randyT9V9C]

It's possible, Feed Optimization is slowing the feed is causing the apparent stutter. The other issue may be due to your controller attempting to interpolate so many small arcs. Tightening the gibs could also contribute.

The 3D Adaptive paths do not look correct. Adaptive clearing should use the side of the cutter to take a radial cut in a sweeping tracodial path. Your arcs look way too small/tight. For this part I'd use 2D adaptive. I'd take a full depth cut which is still less than 2x diameter. Remember endmills cut on the side as well as the bottom.  Are you cutting aluminum with a 4 flute cutter? You'll likely have better chip clearing with a 2 or 3 flute. Variable helix may be good also.

My calculator suggests the adaptive could be pulled off with a 2 flute endmill, full depth 0.355" with the 0.09" cut width (chip load 0.0008") but the speed would drop to 8 ipm. With the 0.03" the chip load is 0.0015" at 20 ipm. I'd opt for the thinner chip at the higher feed, this also cuts the deflection.

I like adaptive paths but they can be more processor intensive and slower depending on the conditions, a stepped down contour may be the fastest, provided you can keep the chips clear.

See the paths in the attached model.

[Benjammann]

Wow! Thanks so much. This gives me a lot to think about. I ended up figuring out that the jerky path was solved by restarting Mach 3 after I tested some old paths that did the same thing.

What calculator do you use? So you think that even on my underpowered machine I could do a full depth cut with the right end mill and settings? With the 3/16" mill at a depth of .130" I could go 15 ipm and not stall out. So you are saying go the whole depth and reduce to around 5 huh?  I have some extra material so Ill probably give that a try tomorrow

Here's the cut at my current settings:

Thanks again for the help.

[randyT9V9C · Accepted solution]

Ah, the power of the reboot. Who would've thought. 😉

I use GWizard. Understand a calculator may not take into account your specific machine limitations but it can be very helpful when estimating a starting point. Let's play with some numbers.

Using your original 0.13 dc, 0.09 cw, 15 ipm, and 0.0008 chip load, the HP requirement is 0.0337, torque 6.8,  and deflection is 39% (0.000396). The full depth cut using 0.03 (16%) cut width comes in very close, albeit a little lower, but less than half the time. Using a 0.355 dc, 0.03 cw, 15 ipm, and 0.0008 chip load, the HP requirement is 0.0307, torque 6.19, and deflection is 36% (0.00036). Definitely worth playing with.

If you really want to push it, use full depth 0.355, 0.03 cw, 40 ipm, and 0.0015 chip load. This will push your HP to 0.0837, nearly triple the torque to 17 and take deflection to 98% (0.000982). A more conservative 0.02 cw, 48 ipm, 0.0015 chip load, would bring the HP back down to 0.0662, deflection to 77% (0.000778), and torque down to 13.36.

Remember, healthier chips take way more heat all while removing more material. Thin chips tend to soften causing clearance issues. I normally use 0.002" per tooth in aluminum.

[Benjammann]

What do CW and DC stand for? Is CW the same thing as optimal load?

I think I get what you are saying though. A full depth cut with a thinner pass going at the same ipm will do the job in half the time? I checkout out the file you sent and I couldn't get the time to halve for some reason.

I have 1/4 hp motor, although I am thinking of modifying it with a 1 1/4 router as the motor. I think my max ipm is around 40 just jogging around.

Thanks again for the explanations. I think ill probably be getting G wizard and start learning it.