[Need TECH Help!]

Been doing some more testing cutting air I have a Gcode that has small arcs and lines (high speed toolpath) making 2 slots that are .280" wide with a .25" end mill. Ran this same program at work on a "industrial" machine with no problems, actually looks like table is vibrating its so fast
When running gcode on my mill, speed of axis look good at start, then after a few seconds axes start slowing down. Then if i pause program and resume, speed of axes again looks good at start and then slows down. I tried increasing the look ahead time. This helps a little but what ever look ahead i have, axes will wait that long after i start gcode before executing gcode. And still slows down after a few seconds.
Attached is gcode. Any ideas?

Troy

[Need TECH Help!]

So started reading the section of manual about the Trajectory Planner settings (Understood it a little bit. . And set the Break Angle(45), Look Ahead(1), Collinear Tolerance(.0002), Corner Tolerance(.0004) and Facet Angle (1.6).
Tom or anyone, do these settings make sense?
So far the motion of machine is fairly smooth with no slow down that i can notice by eye and ear but there is some hard start and stops that is noticed at beginning and end of tool path where the moves are larger.

Thanks,
Troy

[mmurray70]

Machine looks good in video, very fast. Good job. I also had to set break angle very high to avoid slow downs. I think i set mine to over 100 degrees to try and make 90 degree turns faster. Not sure how much it helped, but didnt see any other issues.

Whats your axis acceleration in the trajectory planner? The Jerk setting in kflop is only applied to rapid moves, for interpolated moves it is not used and full acceleration is applied right away and it can cause some harsh motion unless you set acceleration very slow. Kind of disappointing not to have jerk on coordinated moves. This is probably the only major feature kflop is lacking from an original controller. Seems like we have to live with fairly slow accleration or rough motion. Be sure to add a low pass filter to help smooth motion. This will round corners more, especially at high speed. Most industrial controllers work this way as well to an extent, not a real big deal, just slow down your finish pass. I think i set mine somewhere between 0.010 and 0,020 seconds, made a huge difference and allowed me to bump up acceleration slightly. Lower is more accurate obviously and larger will run smoother.

I guess our hardware is already capable of doing 3rd order interpolated moves if only Kmotioncnc could process it that way. Maybe someday you could add this Tom? I think i saw a post before where you mentioned it was very complex, but other controllers do it, I bet you could get it working too.

[Need TECH Help!]

My Accel is 30 and Vel is 12. Tried higher Accel and Vel but didnt help much.
I have a filter within main init program but not after like the manual on Trajectory Planner suggest as an option.

[mmurray70]

I couldnt reach 30 IPS^2 on my machine without my machine sounding rough in some situations. I think i had to live with around 15.

The coder for the low pass filter is below, makes a big difference. I would try much larger number then in sample program below though.

#include "KMotionDef.h"
main()
{
double Tau = 0.001; // seconds for Low Pass Filter Time Constant
KLP = exp(-TIMEBASE/Tau);
printf("Tau=%f KLP=%f\n",Tau,KLP);
}

[Need TECH Help!]

I couldnt reach 30 IPS^2 on my machine without my machine sounding rough in some situations. I think i had to live with around 15.

The coder for the low pass filter is below, makes a big difference. I would try much larger number then in sample program below though.

#include "KMotionDef.h"
main()
{
double Tau = 0.001; // seconds for Low Pass Filter Time Constant
KLP = exp(-TIMEBASE/Tau);
printf("Tau=%f KLP=%f\n",Tau,KLP);
}

Where did you place this code? In the Main Init C code or?

[mmurray70]

Where did you place this code? In the Main Init C code or?

Yes in the main init file, I placed it just after all the settings are set for each axis and it worked fine.

[Need TECH Help!]

This helped out nicely. Was also able to increase feedrate to 80IPM and shaved off over 4 seconds of cycle time. (Still cutting air thow. And Accel at 40.
Will try to get a video of it soon.
Thanks again,

[Need TECH Help!]

Here is a little video of the test gcode of a high speed toolpath.
https://youtu.be/pVHg96-1HY4

[mmurray70]

Those poor ballscews. I try and avoid really tight adaptive paths personally. But looks like its doing it fairly well

Seems like your hurco is built more solid then my machine. My mill would sound terrible with that toolpath at that speed.

[Need TECH Help!]

You should have heard ball screws before the fine tuning was done.
I was fairly surprised by the whole design of this machine giving its year. This toolpath would be a "worst case" scenario, more of a acid test. Got another test cutting some plywood that i will post a video of later.

[Need TECH Help!]

Here is a test cut in plywood that i think Tom will like.
https://youtu.be/qLxeTYGQMDA

[TomKerekes]

[Need TECH Help!]

Hi Troy,

Do you have any action configured for Halt in KMotionCNC | Tool Setup?

Regards

Hi Tom,
Was there something that you working toward when you asked this? Concerning the spindle runaway when feedhold is pressed during a G84 tap cycle?
Just to re answer, yes i have a C program that sets both CW and CCW bits for spindle to shut off and MDI a G80 and G40.

Troy

[TomKerekes]

Hi Troy, Yes. In that case you might try temporarily removing the Halt Action to see if it is related. G84 will invoke M119 to run a C Program using some Thread. Is your Halt Action configured to use the same Thread? Regards

[Need TECH Help!]

Hi Tom,
I removed the C program from Halt action and the M30 action, but after i feed hold (not halt) during tap cycle the spindle still runs away to full RPM. Axis do not move.

[TomKerekes]

Hi Troy,

Do you have an Action assigned to Feedhold?

Please post the current Version of the Rigid tapping C program you are using.

Regards

[Need TECH Help!]

Nope. No Action for feed hold.
Attached is Rigid Tap C program.

[mmurray70]

I still think you might be better off blocking feedhold to stay out of trouble. Its not an easy fix without major changes to the rigidtap program and init file. But if your set on getting it to work. Keep it mind that you dont actually want to do a normal stopcordinatedmotion like a normal feedhold would do. To properly stop while spinde is slaving in the rigidtapping program you need to just simply stop spindle and the Z will be still slaving and also stop with it and everything will stay in sync.

You could probably set a userpersist variable to indicate tapping is active and in your init file, when you press your feed hold button it could check if tapping is active or not and then either stop the spindle if tapping or do a normal stop co-ordinated motion if tapping is not active. And your cycle start button could check for the same to resume. Another userpersist variable could be set in the tapping program to set which direction the spindle needs to be restarted in.

Another issue you will have is if you setup feedhold to stop spindle and your almost finished and it coasts to the bottom it will restart again in reverse. If you turn tap by hand it could restart. A lot of complications and possible safety issues. Sorry i dont have any suggestions about the spindle ramp problem, but i just wanted to point these things out. Good luck with it.

[Need TECH Help!]

Hi Murray,
Having the feedhold turn off spindle i think would be the best way to handle it during a tap cycle.
As for restarting and reversing at bottom of hole, can there be way to ignore this when in feed hold? Or maybe Estop whole machine? Would be safer to break a tap than harm someone.