Z-axis Skip during 3D cut

[Chazz]

I am having a problem that is new to me -- my Z-axis stepper is sometimes skipping during a cut. It has happen three times now -- twice in the last cut. The first two skips (or what appeared to be a skip) were very small. The last one... changed my Z by about 3/8"!!!

It has only happened so far, while doing a 3D finishing cut with a 1/4" ballnose bit. The 3D pattern has some shear Z-Drop surfaces; but the tool seemed to run those fine.

Also, I admit that I was not there watching. So some of this is supposition.

Lastly, I have recently finished the 5.5" Z upgrade. However, it seems to travel just fine. The spring is in place.

Thoughts?
Thanks,
Chazz

[scottp55]

Chazz,
Sound like you might be losing steps?
What Diameter was Roughing bit,material,and 3D finish Move Speeds?

[MogulTx]

Also check to make sure the bit is not slipping in the collet.

[Chazz]

Chazz,
Sound like you might be losing steps?
What Diameter was Roughing bit,material,and 3D finish Move Speeds?

Using Router
1/4 ballnose (Amana Tool #46294)
harder wood (like white oak) sorry, not up on my wood IDs
Roughpath's machining allowance: 0.1"
Finish path's feed speed: 2.0"/s
Finish path's plunge speed: 2.0"/s

First skip on this last cut was about 0.03" and the second one was about 0.13".

I can't really tell if the bit slipped but as a sort of test, I tried to use the motor to drive the ballnose into the spoiler board (router off) and it didn't seem to move in the collet.

[MogulTx]

Chazz.

The combination of the pulling forces of the router being driven into the material and pulled against it in a rotational manner, may move the bit. You should be able to measure the bit extension out of the collet and tell if it moves after XXX minutes of run time. ( The collet might heat up and expand and allow the bit to slip.) The fixes for that are (1) replace a loose or damaged collet (2) tighten the collet nut more. (3) replace the bit if it is loose in the collet from being milled too small. (4) replace the collet with the next size smaller collet so that it grips more aggressively ( assumes a metric collet and a loose fit and that a 1 mm reduction in collet size would force it to grip more aggressively). A dirty collet can also be a problem. If it is clogged with sawdust, in the "fingers" of the collet, it may not grip an appropriately sized bit with enough strength to entrap it. Solution if to blow it out and or scrub it with a brass or plastic bristle brush to remove debris.

Dull bits can contribute to bit pulling out. Bad feed /speed rates can contribute. ( I have never run my systems at 2.0 in the Z while doing a 3D roughing cut. Is it wrong? I dunno. But I would back it down to 50% of that and see what the performance is. Maybe even to .7 and see what the performance looks like. I am guessing that you may have pulled a mostly well secured bit out of your collet... but it is merely a guess at this time....)

Work on it. Let us know what progress you make.

[scottp55]

Well, So much for my theory...with using the same bit, those speeds, and that allowance, it shouldn't be a toolpath thing.
Does it do it running regular 2D operations as well, or just 3D with the 2IPS plunge?
When you did your Z-upgrade, did everything look good with no wear marks and moved freely on rails?
Can you inspect back there to make sure no new wear marks, all bolts still tight,and nothing protruding where it shouldn't.
On a Keypad Move/Jog (multiple times to limits) does it return to the zero you set (maybe use a softwood test block and feeler gauges)?
Did you install your upper Z prox, and is it working?
Did you redo set-up and check the box (I think third page?) "I have Z prox" and does it now run the Z routine with a double tap/pause at VC set safe-Z briefly, then continue to upper Z prox and retract an 1/8"?
Does it do it on an aircut of that model?
I might make a VCP file with material set-up safe Z set to approx what your 3D Z is and, run an aircut using your common 2D settings just to try to isolate it.
Good Coms and packet size test?
Out of ideas then...So I'd call Tech and see if they had run across a similar problem.
Imagine you've checked most of these already.

[Chazz]

Chazz.

The combination of the pulling forces of the router being driven into the material and pulled against it in a rotational manner, may move the bit. You should be able to measure the bit extension out of the collet and tell if it moves after XXX minutes of run time. ( The collet might heat up and expand and allow the bit to slip.) The fixes for that are (1) replace a loose or damaged collet (2) tighten the collet nut more. (3) replace the bit if it is loose in the collet from being milled too small. (4) replace the collet with the next size smaller collet so that it grips more aggressively ( assumes a metric collet and a loose fit and that a 1 mm reduction in collet size would force it to grip more aggressively). A dirty collet can also be a problem. If it is clogged with sawdust, in the "fingers" of the collet, it may not grip an appropriately sized bit with enough strength to entrap it. Solution if to blow it out and or scrub it with a brass or plastic bristle brush to remove debris.

Dull bits can contribute to bit pulling out. Bad feed /speed rates can contribute. ( I have never run my systems at 2.0 in the Z while doing a 3D roughing cut. Is it wrong? I dunno. But I would back it down to 50% of that and see what the performance is. Maybe even to .7 and see what the performance looks like. I am guessing that you may have pulled a mostly well secured bit out of your collet... but it is merely a guess at this time....)

Work on it. Let us know what progress you make.

I don't recall ever having this problem in 2D... ever.

I doubt the collet has any issue. I have never hit metal in operation and while there is alway dust on it when I pull it to do my bit change, it always comes off by just blowing on it. It seems brand new.

The bit has a line between the silver and gold portions which would make an easy reference mark for checking for slippage in the future. However, I didn't note where it was when I put it in this time.

The bit is pretty new as in this week was the first time I used it. That said, I suppose there could be a defect that I am not able to see.

I don't know what my roughing plunge speed was off hand. The 2.0 (and the problem so far) is only in 3D finishing cuts.

I have a theory which I will post shortly...

[Chazz]

Well, So much for my theory...with using the same bit, those speeds, and that allowance, it shouldn't be a toolpath thing.
Does it do it running regular 2D operations as well, or just 3D with the 2IPS plunge?
When you did your Z-upgrade, did everything look good with no wear marks and moved freely on rails?
Can you inspect back there to make sure no new wear marks, all bolts still tight,and nothing protruding where it shouldn't.
On a Keypad Move/Jog (multiple times to limits) does it return to the zero you set (maybe use a softwood test block and feeler gauges)?
Did you install your upper Z prox, and is it working?
Did you redo set-up and check the box (I think third page?) "I have Z prox" and does it now run the Z routine with a double tap/pause at VC set safe-Z briefly, then continue to upper Z prox and retract an 1/8"?
Does it do it on an aircut of that model?
I might make a VCP file with material set-up safe Z set to approx what your 3D Z is and, run an aircut using your common 2D settings just to try to isolate it.
Good Coms and packet size test?
Out of ideas then...So I'd call Tech and see if they had run across a similar problem.
Imagine you've checked most of these already.

It just happens in 3D finishing cuts.... I don't KNOW that it is a stepper slip in a plunge, it could be bit slippage upon the upward move.
In the upgrade, I did not find any worn parts. Nothing required a hammer to get back together. I would say that the long spiral gear coming out of the Z stepper didn't seem as well lubricated as the others. I gave it a shot of lub; but it just doesn't have the same free feeling. However, this cut shouldn't have taken the Z travel to the top end of the screw gear...

As for Z testing, I have always wanted to modify the Z-zeroing script to report what the difference was from the old Z setting to the new.... hummm
I have not attached the Z-prox switch nor changed any settings to let it know.

I have done some pretty severe fluting passes in 2D mode which would be kind of like this 3D stuff... no problems noted. However, it was a medium dense wood rather than hard.

[Chazz]

25576I think that there are some contributing factors and I have a way forward for some testing....

1) The pattern had a steep drop-off -- as in vertical.

2) In the more severe case, the bit could have been pinched between the 7/8" pattern drop-off and the 7/8" 3D cut boundary.

3) By leaving 0.1" machining allowance on the roughing pass, there was a lot to pull out on those vertical surfaces.... all at once... like, for a moment, doing a 7/8" deep pass through the hardwood material. (opinions on this please.... how much of a machining allowance when using 1/4 upcut for rough and 1/4 ballnose for finish?)

I still don't know if it was a stepper skip or bit slip; but I can note when I put the bit in and report if it happens again)

I will take a picture and post shortly... (should have done this at first)

[Chazz]

So, I had left the desktop and all on, with the bit in and decided to redo the cut as a test.

1) I zero'd the Z to the spoiler board.
2) I moved it to Z 0.
3) I measured from the spoiler board to the bottom of the plexiglass under the router.
4) I ran the 3D finish cut again. It did jump again -- in a different spot -- BEFORE it got to the new material that had not been cut yet....
5) I moved it over to the spoiler board and eye-balled it down to just touching. It was at +0.04" Z.
6) I remeasured from the spoiler board and it was the same measurement. From this, I would claim that the bit did not slide in the collet.

7) I removed the bit and ran the router down to the lowest I wanted to get it to.
8) I zero'd Z to that point.
9) I cautiously ran the router to the highest I could comfortably get it. This turned out to be about 5.4
10) I made a long script of "jz 0" followed by "jz 5.4" over and over again.
11) I ran the script.

While the script was running, I noticed odd movement in the servo screw gear down from the Z servo. From the router moving from top to bottom, the bottom of that screw gear was moving side-to-side by 0.15" I think I can adjust something to get rid of that movement; but I don't see this as being enough to cause my original problem. Especially since the 0 - 5.4 test ran for 20 minutes or so without skipping a beat.

Thoughts?

[Brady Watson]

3D rough with a smaller tool and/or with a smaller pass depth to more closely follow the model contour. The most important function of roughing is to make a nice clean, easy path for the finishing tool to clean up. This means no ambient/waste material around the perimeter for the tool to slam into (shock load) when finish machining. I would strongly recommend using carpet tape for hold down and do your 3D rough and a 2D profile of the perimeter of the model. Then do the 3D finishing.

Reduce your Z speed to 1 IPS. 2 is too fast in hard lumber with a steep drop off in the geometry of the model. I would suggest machining at 2,1 inches per second and see if your issue is resolved.

Without a properly setup dial indicator it is not possible to reliably check the Z stepper/screw arrangement for backlash. Try machining as suggested above first.

-B

[Chazz]

I agree that, in the future, I should use a closer machine allowance in the rough cut.

I probably didn't make it clear in my earlier post. In this test re-cut, the skip happened in the area that had already been 3D finish cut!!!!! The shear faces could have contact; but no more than that. It wasn't cutting anything!!! I was doing it to see how it did on the part that had not been finish-cut yet -- it just didn't get that far before skipping.

I am willing to try the plunge rate of 1 rather than 2.

I also thought of doing the majority of the cutout (at least the shear surfaces) prior to doing the finish pass.

Unless I have the wrong ideal of backlash, I wasn't saying that it was a backlash adjustment. What I am calling the "screw gear" is the long black cylinder that looks like the body of a large machine screw and it is either attached or a part of the shaft of the stepper on top of the whole desktop. When the router is at its lowest extreme, I took a measurement of how far this was from the side plate of the gantry. Then I ran the router to the upper extreme. I re-measured the distance from the bottom of the screw gear to the side plate and it was 0.15" farther away. It seems to me that a trivial shift of the mounting of either the backlash spring/assembly or the stepper itself could remove this difference. I have not moved forward with trying it as of yet.

[Brady Watson]

In the name of clarity, it is important not to jumble certain terms....

You don't want to change the machining allowance. You just want to use a shorter pass depth while 3D roughing so that it more closely follows the model. This is something that few understand or get, unless they've paid their dues toolpathing a ton of 3D parts.

Leadscrew is the proper term for the screw moving the Z axis. The end is free to flop around because putting a bearing on the end of it to hold it would make the machine more prone to binding. If you look to the left (X0) of your gantry at the bearing in the X leadscrew block, you can feel it has a sloppy fit - on purpose. It's just there to counter the effects of gravity.

It is possible that there is some backlash in the Z due to the way in which the leadscrew is attached to the motor. It's rare for this to happen, but not impossible. If you take a dial indicator and do some testing, you should be able to determine if there is backlash in the Z. You would have to send your Z motor and screw off to SB to have it adjusted.

The other thing besides speed that can cause a positional loss is your VR settings. If they have been modified they can make the tool move abruptly/aggressively and cause it to lose steps. There is also an outside chance that your Z axis motor driver is a little flaky, but the other things need to be ruled out first.

Keep in mind that when people have problems with these machines, 95% of the time it is because of operator error, with 5% being a machine defect or something in need of adjustment. When things go wrong or unexpected, it's usually something stupid. That's not to say you are 'at fault' from a critical view, but that in my experience, one little overlooked thing can really kick your butt some times.

-B

[Chazz]

In the name of clarity, it is important not to jumble certain terms....

You don't want to change the machining allowance. You just want to use a shorter pass depth while 3D roughing so that it more closely follows the model. This is something that few understand or get, unless they've paid their dues toolpathing a ton of 3D parts.


I agree about terms and I apologize if I butchered them.



Machining Allowance:
The machining allowance is a virtual thickness which is added to the 3D model when the Roughing Toolpath is calculated. This ensures that the toolpath leaves some extra material on the roughed part.

This is beneficial for two main reasons, the first is that when roughing it tends to be done with relatively large tool and aggressive cuts and so is more prone (depending on the material) to chip, this “skin” helps to prevent the chipping affect the finished surface. The second reason is that most tools cut well when they are constantly removing material. Therefore leaving an allowance of material on ensures that there is always at least some material for the finishing toolpath to remove.

Pass Depth:
The maximum depth of cut the tool can cut. The Pass Depth controls the number of z level passes that are calculated for a toolpath. For example, creating a pocket 1" (25.4 mm) deep using a tool that has a Pass Depth of 0.25" (6.35 mm) will result in the toolpath making 4 passes.


These definitions are why I thought machine allowance was the adjustment as to how closely to follow the model's shape and that pass depth was how much of the material to take out on each pass when cutting.


Leadscrew is the proper term for the screw moving the Z axis. The end is free to flop around because putting a bearing on the end of it to hold it would make the machine more prone to binding. If you look to the left (X0) of your gantry at the bearing in the X leadscrew block, you can feel it has a sloppy fit - on purpose. It's just there to counter the effects of gravity.


I can see that one would not wish to restrain the bitter end of the leadscrew. I just noticed it and was adding it to the list of symptoms. I don't think that 0.15" movement is enough to cause a problem; but I don't know. My swag would be that if I could get a combined shift of between 0.02" and 0.03" and it would be minimized. However, I do not think it is a primary contributor to this problem.


It is possible that there is some backlash in the Z due to the way in which the leadscrew is attached to the motor. It's rare for this to happen, but not impossible. If you take a dial indicator and do some testing, you should be able to determine if there is backlash in the Z. You would have to send your Z motor and screw off to SB to have it adjusted.

The other thing besides speed that can cause a positional loss is your VR settings. If they have been modified they can make the tool move abruptly/aggressively and cause it to lose steps. There is also an outside chance that your Z axis motor driver is a little flaky, but the other things need to be ruled out first.


I have done a fair amount of 3D cutting prior to this and in all of that, I never had this problem while I was at a Z limit of 4". It is only after switching to the Z limit of 5.5" that these symptoms appeared. I have not changed the software at all. I did regenerate the toolpath and I changed the finish tool from 1/32" to 1/4" ballnose. This would be the first time I used the 1/4" ballnose on hardwood. However, I have not attempted to do a 3D finish cut with the 1/32" ballnose since my Z upgrade.


Keep in mind that when people have problems with these machines, 95% of the time it is because of operator error, with 5% being a machine defect or something in need of adjustment. When things go wrong or unexpected, it's usually something stupid. That's not to say you are 'at fault' from a critical view, but that in my experience, one little overlooked thing can really kick your butt some times.


I whole-heartedly agree. I fully expected/hoped that someone would say, "Oh, yeah, that happened to me because I didn't pay enough attention to step X of the installation procedure." Alas, I also seem to find the combination of things to do that nobody else does... lol