Something to try, would be to use exact stop for the posted code.
Air run the code.

Reduce velocity values for each axis in steps of 20% each time you run it and see if the problem stops.
If not, then start reducing the accel values by 20% at the lower velocity setting. See if the problem stops.
If not, then your motors ( actualy it could be a combination drive / motor / settings ) may be the problem and it has to do with acceleration. To make small combination moves you need almost instantaneous accel ...decell.  
Fortunately if your problem is repeatable you can play around and try to find what is causing it.

FWIW:
I had problems with my mill and it drove me bonkers. Wasn't skipping in the traditional sense, ( couldn't hear a skip at those silly 0.0001" moves), could not tell exactly when,  it was random in the 1000's of lines of code and never had a problem with 2D machining.  Put dwell in the code and could never duplicate it at different locations and like you the code was for very small moves ( had external DRO's to compare Mach to actual location).

Adjusted the machine to reduce / MINIMIZE the torque required to move all axes and still MINIMIZE the backlash.Adjustment done such that I could measure the required torque to just move the axes and also see what the backlash was. In the end the required torque to just move the axis was reduced from around
80 / 90 in oz to about 15 in oz and for 350 in oz motors that's a great improvement.
Things improved.....so i changed the steppers to 500 in oz and have not had a problem since.

In general a lot more torque was available which provides for improved acceleration ( you higher up on the curve for given motor rpm.....actual in or closer to max power on the curve.

Just some thoughts and have fun playing around,

BTW.....One can do all the advanced calculations etc. they want using computer programs but
when the day ends good old fashion test, measure, try is sometimes required.

RICH

I am using an Ethernet Smooth Stepper.

I might be wrong here but I seem to remember something about (some/all ?) external controllers suffering from buffer underflow when dealing with lots of extremely short lines.

Certainly in the snippet you posted, the code starts with lines in the order of 1/100ths of an inch long but towards the end it drops to lines a few thou long. (see pic).

Re: the great micro-stepping/torque myth/truth debate - crikey this one runs doesn't it? - 

How about a PRAGMATIC approach?

Micro-stepping a) increases resolution (up to a point) and b) reduces resonance.

Re: a) - more than 10 is pointless. The argument goes something like this: A stepper has a full step accuracy of +/-5% or a 10% swing. That means it's accurate to within 0.18 degrees. That just happens to be the resolution of factor 10 microstepping. So, how can you increase resolution beyond the accuracy its capable of? - answer: you can't it doesn't make sense.

Re: b) - We're running full step or perhaps low micro-stepping and we get resonance. That resonance builds up and results in a stall. Stall happens when torque is zero. We increase micro-stepping. It no longer stalls. Which therefore has the most torque?

Hey everyone.

So, this is all a lot for me to take in because I would not consider myself professional at CNC but here is what I have gathered.

1. Try halving my micro stepping and see if it produces a smoother result
2. Play with reducing velocity and acceleration to produce a smoother result



I also wanted to try to give more back story. The shuddering during this toolpath is definitely repeatable, it is not random.
When really trying to hear and see the shudder, I have been running the CNC dry (just running the toolpath in the air, not cutting anything).
I used to have 125 oz in. steppers on the machine and I do remember the shuddering while running this toolpath then.
The closed loop steppers (linked to in a previous post by me) are new and this is my first time running them through movement tests.


I will try 1 and 2 up there ^ but please let me know if you have any other possible solutions or you need any more information from me.

Stirling, thanks for that, I learn't something with (a) [never considered].

(b)... can you not tune out with digital programmable drives?   (Leadshine AM882)

Say I'm using 1/2 stepping on a plasma z (because I've not got the right leadscrew... yes!) ... 2mm / 200 steps / 2 micro steps... 0.005mm / step

Or if I'm using a better l leadscrew (10mm pitch).... 10 / 200 / 2 = 0.025mm per step .... or would I be better with 4 u Step resolution or some other custom number?

Something I've never known... can you set a stepper drive with a microstep resolution of 5 (odd number multiples).

Thanks for the time & guidance.

__________________________________________________________________________________

Back to the OP & helping

With regards to the external motion controllers and buffer under flow..... would increasing the lookahead not help and also changing the SS velocity update frequency too?

Lookahead is presently set at 100 lines, and the velocity update frequency 1kHz..... although you'd need to reduce the update frequency to increase the ESS buffer  (or reduce your step frequency update too.....  which is 128kHz..... hence halving the ustep resolution will allow for the ESS step frequency update to also be reduced to 64kHz)

He said he's using closed loop stepper drives, so doesn't that throw all the microstepping issues out the window? You're dealing with an encoder, and probably can't adjust the microstepping to the motor, as it's probably related to the encoder count.

Jerky motion can be caused by a combination of lookahead and the various CV settings. First thing you should do is turn off all of the CV options, both on the Settings page and in General Config. But make sure CV mode itself is turned ON.

I think you have the old problem of a marginal table with a bit of loose motion and NOT a heavy weight frame Which gives you little damping effects AND running microsegmented code that Mach3 does not handle well. Have you bumped up your look ahead to at least 200 ??  Do you have any setting set in the CV mode.  

The problem starts for mach3 not being able to handle CV in microsegmented code very well so it ends up running as exact stop. Then the banging starts as the frame not being a rigid structure cannot dampin the resonance properly. Mach3 has a bang bang planner and that does not help matters with fast tables.

SO you end up with shake rattle and roll. AN Scurve planner would smooth thing s out a lot.

(;-) TP

Hey everyone.

Here is what I have come up with:

Just right now, I noticed every time the toolpath would start up, the CV MODE would turn off and I was originally not noticing this.
The start of my code looked like this:

N100 G17 G20 G90 G40 G80 G64 G49 G0 M05
N102 G8 P1
N104 G90 M5 Z0
N106 G52 X0. Y0. Z0.
N108 G43 H5 Z.25
N110 T5 M6
N112 G0 G90 G54 X7.3898 Y9.0113
N114 S13000 M3
N116 Z.1
N118 G1 Z-1. F50.

ETC...

I then wrote in a G64 (as previously recommended) and noticed this turned on CV MODE.
The NEW code:

N100 G17 G20 G90 G40 G80 G64 G49 G0 M05
N102 G8 P1
N104 G90 M5 Z0
N106 G52 X0. Y0. Z0.
N108 G43 H5 Z.25
N110 T5 M6
N112 G64 G0 G90 G54 X7.3898 Y9.0113
N114 S13000 M3
N116 Z.1
N118 G1 Z-1. F50.

Here is what happened:

Almost all of the shuddering went away, and I started having a smooth, curve like motion come out of the CNC toolpath. The toolpath was running A LOT better. There is only a small amount of shuddering of very rapid small moves from front to back (backlash?), but it is barely noticeable.

I timed the toolpath for efficiency:
200 lines lookahead

At 3mins 48 secs, CV MODE on, 9890/9890 lines finished
At 3mins 48 secs, EXACT STOP on, 2366/9890 lines finished (very shuddering and jerky motion)




Now this seems to have solved my issue but I am left with a couple questions:

1. What should I have turned on in relation to CV MODE (other than CV MODE)?
2. Do I need 4000 pulse/rev for microstepping or is there a better amount to use to optimize my system?
3. Is there any other things (settings, etc) you folks can think of to help make my system run smoother?
4. Why does my GCODE turn off CV MODE?
5. Should I always have CV MODE on?
6. How can I program Mastercam to always input a G64 into my GCODE?

IF you noticed on the first line it did include teh G64 (CVmode) BUT it then turned it off with G8 (exact Stop)

(;-) TP

is G8 a valid code with Mach3?

http://machmotion.com/cnc-info/g-code.html
http://machmotion.com/documentation/Software/Mach3/Mach3%20GCode%20Language%20Reference.pdf