Jerk motion, what am I doing wrong?

Post anything you want to discuss with others about the software.

Re: Jerk motion, what am I doing wrong?

Postby rmat » Tue Dec 18, 2018 1:08 pm

Interesting thing I just observed playing, with current settings, small Helical (boring 10mm hole with 6mm OD) motion in XYZ is smooth?
How come is this possible?
Anyways, going changing setup and see if it improoves.
rmat
 
Posts: 15
Joined: Thu Dec 13, 2018 12:22 pm

Re: Jerk motion, what am I doing wrong?

Postby Robertspark » Tue Dec 18, 2018 3:28 pm

I would suggest setting up a bit of gcode such as the following to do a simple square and then observe your changes.
Code: Select all

G91
F3000
M98 P201 L20
M98 P202 L20
G90
G0 X0
M30

O201
G1 Y250
G1 X250
G1 Y-250
G1 X-250
M99

O202
G1 X250
G1 Y250
G1 X-250
G1 Y-250
M99


I've never done it but if you are into observing the effects of jerk here is one way it could be measured:
https://youtu.be/qYJpl7SNoww
aka the beer test! :D

I would also suggest starting with all of the UCCNC motion settings set to zero and then you can see the effect of them on the actual observed motion.
2018-12-18 15_09_25-.png
Robertspark
 
Posts: 1892
Joined: Sat Sep 03, 2016 4:27 pm

Re: Jerk motion, what am I doing wrong?

Postby rmat » Tue Dec 18, 2018 5:30 pm

Hey Robert, I like the beer test, and Im gonna go do exactly this after this excercise Ive had with trying out your tests.

Conclusions, I have first set all of the drives to 200/mm, no change whatsoever.
Ive then lowered acceleration down to 200 and guess, I can barely knowtice any jerk.
But, I knew what I was going to end up with, very very slow machine. And since this is a mill, we want as constant tool load as possible. Ideal would be if we could sinchronize spindle with feedrate.
But since this is not possible, I want as constant feed rate as possible, and as far as I understand, high speed toolpaths should make this possible. And with accelerations on 200, feed rate goes from 400 to 3000 mm/min. Its just waste of tools.

My CAM is generating toolpath with all the corners rounded, so machine should hardly brake, but this generates many points, so maybe this is where the problem is. If I understand correctly, lookahead should taken care of this.
Just so you can see, Im attaching Gcode Im testing with, I can provide F360 file or whatever it is neccesary to give me a little bit of lookahead of where my problem is.

This code you are pasting, I understand completly. Please look at my code, try to run it if you have the ability. I would be super glad to hear its running smooth on your machine.
Please also look at this video: https://www.youtube.com/watch?v=IQ4BcIhjlyM

Its the same machine, same motors, only different controller. I switched it becaose Im installing tool changer, and there was just no I/O left on that one, besides its standalone and has some other limitations for more serious work.
So Ive made decision and between Eding and UCCNC picked up UCCNC becaose eding still hasnt got simple controller with kernel over 125Khz out yet, and UCCNC is really really straightforward to connect and allows just about anything.

So Robert, Cheers

Matej
Attachments
Test-cut4-8.rar
(47.76 KiB) Downloaded 610 times
rmat
 
Posts: 15
Joined: Thu Dec 13, 2018 12:22 pm

Re: Jerk motion, what am I doing wrong?

Postby Robertspark » Wed Dec 19, 2018 11:58 am

Matej

I've had a look at your test file attached to your last post.

I think its probably creating problems for you with jerk and jolt.

The reason is because all motion within it is linear G01 motion, but you have arcs within your gcode file created by stitching G01 motion together in very short segments.

Really you should be using G02 motion for these moves, that way the uccnc motion planner and uccnc does the motion planning for you.

What you have at the moment is a load of finite coordinates which have very small distances between them.

Because you have defined finite components then the motion controller HAS TO go to those co-ordinates or at least very close to those co-ordinates and you will not get the benefit of the Corner Error Max setting because the distance between your three co-ordinates of where the machine is now, where it should be in the next move and where it should be at the destination of the move after that.

Stepping back a bit to understand the Corner Error max.

What you are telling the machine to do is if you have a feedrate of 3000mm/min and a corner error max of say 4.2mm, the machine is allowed to round the junction of two linear moves with a radius of 4.2mm without slowing down

So if you have a tool with say a diameter of 8.4mm then this setting will do nothing to reduce the accuracy of the component finish because the radius is equal to / smaller than the corner error max setting. So the motion should be offset 4.2mm from the intended finishing cut line anyway.

However..... if you have a load of linear motion that has movement with finishing co-ordinates less than 4.2mm between them how do you expect the uccnc motion planner blend this motion?

Hence I would suggest letting the motion planner do its job and give it G02/G03 arc motion too..... that way the co-ordinates are not so finite and defined as to where the motion controller has to send the machine but allow the machine to use the corner error max, linear error max, linear addition length max and linear unify length max settings.

The arc radius tolerance is not applicable unless you use G02/G03 with the "R" {radius} defined and not IJ(K) notation for your motion / specifying the arc origin.

Yes there is a well documented anomaly (no it is not a bug) with how uccnc handles G02>G02 or G03>G03 or G02>G03 or G03 >G02 motion however it is (a) better than Mach3 can do it (b) will be changed / handled differently when the motion planner is changed to S-curve in the future (long term objective) you can read about it here (and there are a few other similar posts discussing the same issue under other descriptions. I think you'll find other planners will have a similar issue running the tests I ran though viewtopic.php?f=4&t=1657

Sorry I've never used Eding CNC, and when I was looking to jump ship from Mach3/4 I did consider them {along with a few others too}
Robertspark
 
Posts: 1892
Joined: Sat Sep 03, 2016 4:27 pm

Re: Jerk motion, what am I doing wrong?

Postby Robertspark » Wed Dec 19, 2018 12:15 pm

Attached is a screenshot of a section of your demo file

The N number is the line number that corresponds to your gcode *.nc file
The first column is X coordinates of the move
The second column is Y coordinates of the move
The third column is one I created to identify the distance of the move between each line of motion
I've highlighted some small motion with yellow in bold.

This is just an extract there are other small moves elsewhere too.
Attachments
2018-12-19 12_11_11-Microsoft Excel - Book1.png
Robertspark
 
Posts: 1892
Joined: Sat Sep 03, 2016 4:27 pm

Re: Jerk motion, what am I doing wrong?

Postby Robertspark » Wed Dec 19, 2018 12:24 pm

You may also consider the difference between roughing cuts and finishing cuts on tollerance settings.

I kind of wish there was two lots of planer tolerance settings one for roughing and another for finishing cuts, that way you get the benefit of faster roughing cuts that have the same feedrate however lower tolerance on blended motion and then for the final cut you can reduce the tolerances :roll:
Robertspark
 
Posts: 1892
Joined: Sat Sep 03, 2016 4:27 pm

Re: Jerk motion, what am I doing wrong?

Postby ger21 » Wed Dec 19, 2018 12:36 pm

Robertspark wrote:I kind of wish there was two lots of planer tolerance settings one for roughing and another for finishing cuts, that way you get the benefit of faster roughing cuts that have the same feedrate however lower tolerance on blended motion and then for the final cut you can reduce the tolerances :roll:


You can change the settings in your g-code, so that you can use different settings for roughing and finishing.
Gerry
UCCNC 2022 Screenset - http://www.thecncwoodworker.com/2022.html
ger21
 
Posts: 2663
Joined: Sat Sep 03, 2016 2:17 am

Re: Jerk motion, what am I doing wrong?

Postby Robertspark » Wed Dec 19, 2018 12:39 pm

ger21 wrote:
You can change the settings in your g-code, so that you can use different settings for roughing and finishing.


Other than exact stop / constant velocity what can you change. (excluding finishing cut doc and federate spindle speed etc)

What have I missed?
Robertspark
 
Posts: 1892
Joined: Sat Sep 03, 2016 4:27 pm

Re: Jerk motion, what am I doing wrong?

Postby dezsoe » Wed Dec 19, 2018 12:51 pm

See G64 parameters (from the manual):

Set Path Control Mode to constant velocity : G64
Program G64 D... E... H... L... P... Q... to put the machine into constant velocity path control mode.
All parameters are optional. If any parameters are left out (not programmed) then the software will
get that parameter's value from the screen settings.
The parameter D is the Stop angle setting.
The parameter E is the Lookhead lines setting.
The parameter H is the Linear error setting.
The parameter L is the Linear addition length setting.
The parameter P is the Unify length setting.
The parameter Q is the Corner error setting.
dezsoe
 
Posts: 2049
Joined: Sun Mar 12, 2017 4:41 pm
Location: Csörög, Hungary

Re: Jerk motion, what am I doing wrong?

Postby Robertspark » Wed Dec 19, 2018 12:53 pm

ahhh! :idea: :oops:
Robertspark
 
Posts: 1892
Joined: Sat Sep 03, 2016 4:27 pm

PreviousNext

Return to General discussion about the UCCNC software

Who is online

Users browsing this forum: No registered users and 3 guests