[awpross]

Using one of the synchronized movements results in unexpected issue when a g0 or g1 command on the same axis is used directly afterwards.

It seems as if the motion engine has an issue with calculating the acceleration after one of the mentioned G codes.

For example :
G33.1 followed by G1 Z100 causes my servo drive to immediately go to error state after the G33.1 command with the error "Position follow error". Which indicates to high acceleration or wrong timing in step / dir signal.

This behaviour is not when using G33.1 followed by G9 and then G1 or G0..
It is the same for G84 G74 and G33.1 P0 but not G33.1 P1 (or was it P1 and not P0? not sure)

I have tried different acceleration and deceleration settings but in fact this does not change the issue... However a lower acceleration seems to increase the issue.

I use synchronized motion without encoder because my spindle is not equiped with an encoder.

[PlanetCNC]

Send me profile .zip and g-code.

[awpross]

Attached you will find the requested files.

I was able to solve the G84 G74 by not using M3 or M4 right after that G-Code because it is not necessary.

I marked the failure position after G33.1 in code.

I should mention that I set the servo drive to a very low tollerance of step differences because I am trying to find potential issues in acceleration or decelleration I experienced on my classic stepper drive. On the classic drive i can only see step looses after homing procedure, with the servo drive I was able to find the exact position where the potential problem may be.


The reason for me to use G33.1 for tapping with P1 is, that G33.1 P0 G84 and G74 are traveling back, after they stopped the spindle which is an unnecessary movement. You can see this in simulation too.

I currently use regular G1 for tapping because of performance. We are doing thousands of tappings a day and with G1 it is of cource not as exact at reversing but it is much faster because the movement is smoother due to blending support in plain G1 code.

[PlanetCNC]

Can you try with latest beta version:
https://planet-cnc.com/wp-content/up...2022-03-05.zip

[awpross]

beta does not make any difference. It still fails without additional G9 after G33.1

[PlanetCNC]

Regarding G84 and G74 - I don't understand what you solved with M3/M4? Using M3/M4 should not cause any issues.
My tests do not show anything wrong with G84 and G74.

I can confirm issues with G33.1 P1 and it will be fixed in next version.

[awpross]

Regarding G84 and G74 - I don't understand what you solved with M3/M4? Using M3/M4 should not cause any issues.
My tests do not show anything wrong with G84 and G74.

I can confirm issues with G33.1 P1 and it will be fixed in next version.

The G84 and G74 issue on my side was caused by a different behaviour that may or may not be expected but caused a too fast direction change due to a too high acceleration in my settings.


G84 and G74 are working, but there is a behavior i didn't expect. When returning, those cycles are overtraveling the desired z position because of the deceleration. However insted of retracting to the desired retract position which is in my case higher, the cycle first moves back to the Z position and then to retract position.

This makes that cycles inefficient due to unnecessary motion. I have taken some short video clips to show that behaviour. I calculated that this unnecessary movement may produce a delay of up to 1 hour when tapping thousands of threads a day...

[PlanetCNC]

G84 and G74 cycles internally use G33..1. This is synchronized move. while spindle is rotating axes must move. Only after spindle is stopped axis can stop. That is why you get overshoot. It is completely expected. Those cycles must then return to start height.
Much more efficient is G33.1 P1. P1 means "do not return to start height". This way your code can be faster if you don't care about end height.

[awpross]

Thats why i came finally across the issue with g33.1 P1... looking forward for the fix. Thank you very much.