Sieg KX3 Y_Axis Skipped Stepper Steps😢

Advert

New Replies

Report Bug

Help/FAQs

Sieg KX3 Y_Axis Skipped Stepper Steps😢

This topic has 41 replies, 8 voices, and was last updated 10 May 2021 at 08:20 by JasonB.

Viewing 25 posts - 1 through 25 (of 42 total)

1 2 →

Author

Posts
5 May 2021 at 16:59 #543335
Nicola Casali
Participant
@nicolacasali98042
Continuing the saga with behavioural anomalies..

I replaced my LED lamp with a "quieter" EMI producing LED lamp. That helped. My UC300eth is powered by 5V from a USB cable. I moved that to a USB battery pack to reduce ground loops. Just learning about those! That helped massively with spindle erraticness. EMI is still present but its effects on the spindle are very minor.

So over the last few months I've been experiencing unexplained inaccuracies in machining I've put down to bad workholding and user error. Tolerances haven't needed to be critical, up until now. I started machining some small parts out of mild steel using two passes.

It's on the second passes that the penny suddenly dropped. The endmill is not touching the -Y side but cuts heavily into the opposite side, +Y. It can't now be workholding, maybe the steel is being stress relieved during milling?

Using a dial indicator before and after air cutting a job instead of the stock, it seems the Y axis is out by a massive 0.20 – 0.30mm. X is fine. I've loosened the Y gibb, just in case I overtightened it a few month back. That helps not.

I think my motor tuning settings are default, as set up by John Stevenson. Could this also be an EMI problem?

Is there anything else I could be looking at that could be the cause?
Advert

5 May 2021 at 16:59 #15352
Nicola Casali
Participant
@nicolacasali98042
5 May 2021 at 18:22 #543367
Martin Connelly
Participant
@martinconnelly55370
It seems like lost steps in one direction. This can be caused by tapered gib strips that can move about when the axis is moved, loosening in one direction and tightening in the other. If this is the case (the tapered gib moving that is) the solution is to prevent this unwanted movement with one of a number of options. One is to make sure that any adjusting screw is not moving when the machine is in use. The next is that if the screw is working in a slot make sure the slot is a snug fit around the screw and third if there is only one screw at one end add a second screw at the other end to pin the gib strip where it is set.

If you don't have a tapered gib then it may just be that the motor has too low a torque for the machine, adding large vices to a small machine can increase the loads on the motors. A number of solutions for this include fitting a larger motor, adding a planetary gearbox in line with the motor, using timing belts and pulleys to reduce the speed of the drive to the leadscrew but increasing the torque, You could also add motors with feedback encoders but they require suitable motor drivers so that may be the most expensive option.

Martin C
5 May 2021 at 21:32 #543423
Nicola Casali
Participant
@nicolacasali98042
I disconnected the lead screw nut for the Y axis and moved the table by hand. There doesn't seem to be any binding in any direction. I'm not sure how tight the tapered gib should be, but it's not loose.

It's not a machine I built. I purchased the KX3 new in 2011. I don't _think_ I've had this problem before. It could be a problem with the UC300Eth motion controller I installed in 2017.

I may have to limp along for now with accuracy in only 2 dimensions. The parts I need to machine only require that.

What I could try immediately is:

1. switch to an unused parallel interface on the UC300Eth.

then

2. swap the x and y pins on the breakout board.

3. swap the x and y stepper drivers to see if it's a driver issue.

4. swap around the stepper motors?

5. switch back to using an old Windows XP PC with parallel port to rule out UC300Eth. (I was about to dump that old PC)

6. ?
5 May 2021 at 22:41 #543438
Joseph Noci 1
Participant
@josephnoci1
Nicola,

Are you using MACH3 or UCCNC software with the UC300ETH?

Are the X and Y steppers the same type, ditto the stepper driver modules?

Are the two driver modules set up the same way, dip switches, if any, etc.

Some drivers can be set to go Half Current in the steppers during short pauses in moves, which when driven in microstepping mode can lose micro-step position within the native motor magnetic detent step – if that accumulates it can result in an accumulating step error. If your drivers have such capability, disable it.

I would also suggest checking the stepper pulse train definition setup in the software – MACH3 and UCCNS both have a section where you set up the dwell period between stepper direction control change and the beginning of the next step pulse train – if that is to short for your stepper driver, it can result in lost steps. Likewise, the minimum width of the stepper pulse train can be set up as well – I would make them not less than 5us, even go for 10us, for your kind of setup. At least make sure the Y axis setup is the same as the X Axis.

From your description is seems the Y axis is loosing steps in the -Y direction, biasing the cut to the +Y side. Does the part you are cutting have any rapid Y moves that are more in the -Y direction than +Y? If so , could be that the Y max acceleration ( or velocity) setting for the Y axis are to enthusiastic. X has to move only the X axis, vice and workpiece – Y axis moves include the whole X axis, vise and workpiece, and the Y axis mechanics.

Joe
5 May 2021 at 23:22 #543444
Nicola Casali
Participant
@nicolacasali98042
Swapping parallel ports on the UC300Eth did not help.

I never did set up UCCNC in the end, despite having a license. I'm still using Mach3.

I don't know which drivers are being used or dip switches. The machine is set up against a wall and access is from the back. I did manage to fit wheels to the base, so I am able to move it and check those things out. It's quite a hefty machine though.

I've now gone for your suggested 10us pulses and started a job without stock. I've reduced the acceleration for Y from 300 to 200 in Mach3. With 5us pulses that didn't make any difference. Let's see with the 10us pulses.

Actually, the table is gradually moving away from me, meaning it's having problems 'moving' the spindle in the + direction.

The only rapids are once at the start and then rapids only for z throughout.

Currently, I only have a small 70mm vise bolted to the work table.
5 May 2021 at 23:37 #543447
Nicola Casali
Participant
@nicolacasali98042
Job finished. Y is off by -0.25mm. This was with 10us pulses and 200 acceleration. Tomorrow I'll take a look at the stepper drivers and compare any settings. If they are identical I'm going to swap the X and Y and retest.
6 May 2021 at 00:07 #543449
Keith Petley
Participant
@keithpetley53472
Nicola, before swapping the X and Y over check for backlash in the Y.

Move in one direction (eg +Y), zero an indicator on it, move the same direction again and then come back. Try it a couple of times and then a couple in the reverse direction. Backlash problems normally give a repeatable set of readings.

If it's worked OK for a long time and then "degraded" I'd look for a mechanical problem first, electrical failures tend to be all or nothing.

I once chased a weird problem which looked a lot like lost steps but turned out to be a ball nut mounting block had come loose.

Keith
6 May 2021 at 00:26 #543451
Nicola Casali
Participant
@nicolacasali98042
I checked for backlash. There appears to be about 0.02mm.

I did check the ball nut. I checked it as I unbolted it to see if there was any binding in the tapered gib. I tightened it back up really well. It appears to be a consistent step loss in one direction only. Bizarre! I can reverse the direction of Y travel in Mach3. That's what I'll do next. That'll confuse it..
6 May 2021 at 01:42 #543454
Nicola Casali
Participant
@nicolacasali98042
Reversing the Y axis causes it to lose steps in the opposite direction by the same amount. Let me sleep on it..
6 May 2021 at 06:59 #543458
John Haine
Participant
@johnhaine32865
Is backlash compensation enabled, and if so is it set for the right value? If it is enabled, try switching it off.
6 May 2021 at 09:13 #543475
Joseph Noci 1
Participant
@josephnoci1
Actually, the table is gradually moving away from me, meaning it's having problems 'moving' the spindle in the + direction.

Very strange behaviour if none of those fixes sort it out! I suppose it could be a Stepper driver failure, but I doubt it.

Nicola, I am not sure I understand your axis direction – If the table is moving away from you, its the same as the table remaining still and the head moving toward you – that is Y -Ve direction, not +Ve…

Not really important here as it still has no bearing on the problem..

I doubt backlash comp has anything to do with this – backlash comp is a symmetrical function and would not create such asymmetry.

Nicola, if the G-Code file is not to big would you care to post it here?
6 May 2021 at 10:16 #543492
JasonB
Moderator
@jasonb
Nicola you should be able to access the electronics from the side, the back panel is really only to get at the mechanicals

Looks like the Y gib is only a single screw but as the problem is now showing up with direction altered unlikely to be that. Might be worth marking the ball screw to see if that is returning to the same position and possibly also either side of the coupling

Edited By JasonB on 06/05/2021 10:16:41
6 May 2021 at 11:10 #543508
Ronald Morrison
Participant
@ronaldmorrison29248
My Y axis would skip steps. Turned out I was setting the current to the stepper to high and the driver would momentarily overheat and shut down for a few steps. Turned the current down and it didn't have enough power to push the mill through the material. Ahh, power is voltage times amperes. Raised the voltage on the power supply and now it steps just fine. That may not be your problem but is another avenue to explore.
6 May 2021 at 11:12 #543509
Nicola Casali
Participant
@nicolacasali98042
JasonB, I have marked the ballscrew and it returns to the correct place when the table hits the dial indicator I've set up. And thanks for the view of the stepper drivers.

This is actually my first attempt at 3D machining with Fusion 360. I'm thinking about rotating the model and stock by 90 degrees to see if X starts getting affected.

Joseph, here's the file.
https://www.filemail.com/d/zgorgrgcozwfvti

Edited By Nicola Casali on 06/05/2021 11:16:04
6 May 2021 at 12:27 #543518
JasonB
Moderator
@jasonb
So if the screw is returning to the same position then it does not sound like it is missing steps otherwise it would be at a slightly different angle.

Any chance of also posting the F360 file. There is an option to share which will give you a link.
6 May 2021 at 13:02 #543521
Nicola Casali
Participant
@nicolacasali98042
JasonB, when the dial indicator I set up is indicating zero, the ball screw has returned to its mark. However, in Mach3 readout it's off by 0.25mm. To me that means the ball nut is fine, at least.
6 May 2021 at 13:32 #543524
John Haine
Participant
@johnhaine32865
Have you tried moving the table back and forth along the Y axis using G code via the MDI? If you typed in –

G91 (sets incremental mode)
F100
G1 Y10
G1 Y-10
G1 Y10
G1 Y-10

…while checking the motion with a DTI it should always return to the same point at either end of the travel.
6 May 2021 at 14:34 #543528
Nicola Casali
Participant
@nicolacasali98042
Nice simple test. Will try soon. I don't think I tried that one yet. Although I have written a loop in g code that does something similar, but in absolute mode. That loses steps. I have tried moving the table back and forth using a Vista pendant with the wheel with a variable velocity. That loses steps too.
6 May 2021 at 15:19 #543532
John Haine
Participant
@johnhaine32865
Remember to give it a G90 when you finish or you can get very confused!
7 May 2021 at 02:36 #543614
Nicola Casali
Participant
@nicolacasali98042
Posted by John Haine on 06/05/2021 13:32:01:

Have you tried moving the table back and forth along the Y axis using G code via the MDI? If you typed in –

G91 (sets incremental mode)
F100
G1 Y10
G1 Y-10
G1 Y10
G1 Y-10

…while checking the motion with a DTI it should always return to the same point at either end of the travel.

I put this in a loop in a text file and ran it 200 times at F250. It didn't skip a single step, or didn't accumulate lost steps. I jogged the Y axis back and forth with my pendant a dozen times. No steps lost. I didn't rerun the F360 file. This was 1:30am. I will try again tomorrow during the day, when whatever conditions may be playing a part…return? Mysterious.
7 May 2021 at 06:47 #543618
Joseph Noci 1
Participant
@josephnoci1
Posted by Nicola Casali on 05/05/2021 23:22:24:

I've now gone for your suggested 10us pulses and started a job without stock. I've reduced the acceleration for Y from 300 to 200 in Mach3. With 5us pulses that didn't make any difference. Let's see with the 10us pulses.

Actually, the table is gradually moving away from me, meaning it's having problems 'moving' the spindle in the + direction.

The only rapids are once at the start and then rapids only for z throughout.

Actually, there are many rapids in X,Y and Z in your file , with the Y rapids the longest paths, so maybe there is still something there..

Do you know what the rapid traverse rate is set up for?

It is just a bit confusing from your descriptions though-

It's on the second passes that the penny suddenly dropped. The endmill is not touching the -Y side but cuts heavily into the opposite side, +Y. It can't now be workholding, maybe the steel is being stress relieved during milling?

Using a dial indicator before and after air cutting a job instead of the stock, it seems the Y axis is out by a massive 0.20 – 0.30mm.

Job finished. Y is off by -0.25mm.

JasonB, when the dial indicator I set up is indicating zero, the ball screw has returned to its mark. However, in Mach3 readout it's off by 0.25mm. To me that means the ball nut is fine, at least

I put this in a loop in a text file and ran it 200 times at F250. It didn't skip a single step, or didn't accumulate lost steps.

This implies that you don't lose steps, but that the machined parts is incorrect in Y, and when you don't loose steps the MACH3 DRO shows you are 0.25mm out….

It is not possible to move a fixed distance while not loosing steps ( Confirmed by DTI) but Mach3 DRO show 0.25mm still to go…so nothing sensible here…

Your G code file has X/Y moves in the 30mm range with many XY rapids – Maybe try John's file thus:

Set a round rod in the chuck – say 10m OD and place in table center – zero all axes,

Set the DTI on the table , up against the rod at the diagonal of the square in the MDI text below and zero DTI, then run the MDI text below ( Run the file first to be sure which direction to place the DTI so you don't crash it!)

G91 (sets incremental mode)

G0 Y-40
G0 X-40
G0 Y40
G0 X40 < this should get you back to the DTI zero point

Run that say 10 times and see that the tool tip is back at zero, and that the DRO says 0

Joe
7 May 2021 at 07:27 #543621
JasonB
Moderator
@jasonb
Nicola, when you do those tests that show the Dti reading zero but Mach screen 0.3 are you moving by jogging until dti reads zero? I would have thought you need to get mach to move to a position and then back to zero and then compare dti to screen.

Joe, I'm not sure if Nicola pays for F360, I have a feeling she is using the free version in which case Rapids will not be enabled and it will be moving at the feed rate, seemed like that when I ran a bit of the code on my machine yesterday

Nichola sent my her F360 file and I can't see anything that would make the metal distort in Y so that early question can be ruled out. There are some quite heavy cutter engagements of the 12mm tool (unless Nicola is using shorter stock) Could it be play/backlash ? otherwise cuts are quite light at 3mm wide x 1mm deep. Maybe try putt the dti on the table and jogging one way then the other and see how many 0.01mm jogs it takes before the dti shows movement. maybe also play in the X gibs.

These show the her tool paths which I have suggested some alterations to as step downs are much too small on the adaptive and take a long time with that slow moving hss tool. Yellow are "rapids" but likely running at tool feed rate. Blue is cutting.

Then she had a contour with 10mm ball to finish, not in the g-code

Compared to my adaptive but still with here tool choice and speed/feed

And my scalope to finish again with her tool

Edited By JasonB on 07/05/2021 07:28:47
7 May 2021 at 08:12 #543632
Joseph Noci 1
Participant
@josephnoci1
Posted by JasonB on 07/05/2021 07:27:13:

Joe, I'm not sure if Nicola pays for F360, I have a feeling she is using the free version in which case Rapids will not be enabled and it will be moving at the feed rate, seemed like that when I ran a bit of the code on my machine yesterday

G0 Z5. < Quickly…..
X31.497 Y-24.859
Z1.4
G1 Z0.2 F215. <- at modal feed rate
….

G0 Z5.
X-5.963 Y-1.818
Z1.4
G1 Z0.2 F215.
…

G0 Z5.
X31.912 Y-24.243
Z1.4
G1 Z0.2 F215.

Many dozens of these in the Gcode file Nicola sent me…

Still think its a velocity/acceleration issue at high traverse rates, but I am normally wrong..

Joe
7 May 2021 at 08:32 #543637
JasonB
Moderator
@jasonb
Put it another way, there were no excessively rapid movements on my machine which is set up as stock, I think Nicola said hers was too so without going to look that's 1000 or 1500mm/min rapids. But it does rapid in Z and Y to get back to the beginning of the next cut

Edited By JasonB on 07/05/2021 08:39:49
Author

Posts