[ihavenofish]

I'm not familiar with path pilot (machine controller) but a quick look at its info sheet says that it has a trajectory planner and this is where you want to look

Pathpilot is tormach's user interface for linuxcnc. It does not have jerk control. It is a hot topic of discussion on their forum and that discussion seems to suffer from an all or nothing mentality - jerk control on every conceivable motion case (difficult math), or none at all.

[peteeng]

Hi IHNF - It doesn't need to have jerk control to behave smoother. MDew just wants to figure out how to set up pathpilot to be smoother. Actual jerk control is not easy, especially at DIY, Maker or hobby level. But good path smoothness and good gcode is and that can help improve performance. Then there is the motion planner or trajectory planner to help as well. I'll read some of the tormach stuff.... unless someone reading this already knows how to set this up properly. Peter

[ihavenofish]

G64 enables continuous contour motion.
G61 disables it.

This applies to most controls I think.

In linuxcnc (what the tormach runs) You have 2 parameters, and Q.

P is the maximum deviation allowed in the path. 0.001" will yield precision, but of course it will slow way down in corners. 0.04" will yield very fast (and therefore smooth) results, but can cause more inaccuracy than is desired. This is why you can set it per program, each operation might work best with different settings.

Q is block compression. best to set it to 0 always. What it does is collapse lines of code within a specified angle of each other, so you get less lines, longer segments and faster motion. sounds fine in theory but in practice you can get very out of square cuts.

If his issue is simply that G64 is off, and the machine is stopping at every line, this will fix it. It is possible his post from sprutcam doesn't add G64.

[peteeng]

Hi IHNF - Thanks for the info. I have started to play with G64 in my UCCNC code. Roughing runs can have slacker settings to create faster MRR. Then for finishing revert to finer settings. We'll see what MDew has to say. There are similar general settings in the UCCNC config..Peter

UCCNC has G64 and G61 what does a parameter line look like? ie what is its syntax? I tried to find a pathpilot manual but they don't seem to have one. Does anyone know if their out there?

[peteeng]

Hi Dazp - Lay speak jerk is not engineering jerk. A "jerky" action is due to machine compliance and rough accelerations. Engineering jerk has no strongly apparent observable effect. It does contribute to machine vibrations. It does effect accelerations which produce inertial forces that produce the lay jerky motion. I think this is one of the issues say in forums discussing this. People are misinterpreting what physical/engineering jerk is. They need to adjust accels vs having "jerk" control plus create smoother paths. Peter

[deadlykitten]

hy pette i saw also some of your replies in another thread, then you started this one

seems you are hunting, somehow, the big picture; please, i need to understand better what is behind your words :
... what made you to start looking into this ?
... why are you so focused on jerk , tangential/smooth movement ? if i may, this is local/simple, while mcs is global

sorry for repeating, my advice, is to eliminate from equation cad & cam, and focus only on cnc/mcs, because is better to focus only on one at a time; if you clear your thougths with cnc/mcs, then cad/cam will be clear, not the other way arround; cad/cam is an extension, is not the key, it simply generates input to suit the cnc

also, from cnc/mcs, i proposed that 1 linear axis example, because is simpler to focus on a single axis, rather than all at once

okey, now i will try to answer to some texts :

Its a series of point to point moves

not point to point ... is vecinity towards other vecinity; think of a group that croses the street on a crosswalk: some go middle, some go near an edge, others may go diagonally

there is a tolerance, just like how you would turn a part with diameter 100, and accept as good the 99.8 and also the 100.3

at the Gcode level the machine does not know if its a spline or an arc

this is true only for segmented toolpaths, thus g-code only with G01s; otherwise, it will make a difference between g01 and g02 for example

as for splines, i think you allready know that most cnc's dont have a g code for it

trajectory planner

that's the nominal, while mcs is cheking that real motion is within tolerance, or else will/should stop the machine

I have started to play with G64

is this exact stop mode ?

[peteeng]

Hi DK - Yes the other thread was someone else's and the jerk thing was high jacking it so I started here. Yes I am interested in the big picture. No use looking at this in small pieces yet. I am not focused on jerk it is only one part of making smooth fast toolpaths. But engineering jerk has to be considered at some point. I occasionally do non-linear transient dynamic analysis on machines thats fun and the software calculates velocities, accels and jerk....

Firstly I'm trying to establish best in-principle workflow & concepts from cad to swarf. Yes I understand that "point to point" is like a roadway that a car goes down. The machine control specifies the width of the road and and the tool stays within that width ( most of the time). G64 is constant velocity mode G61 is exact stop mode.

I like to understand things at a deeper level then just being a user of the software. I have been around awhile and have been around when toolpathing was done by specialists so I had to pay someone to create code for various things and I would take that on a disc to a machinist. I remember when a cheap parametric solid modeler (pro-engineer) cost about $30,000AUD and a workstation to run it was about the same $$$. Now you can get both for $1000. I also have been around making FE mesh manually and figuring out node vectors manually so FE models worked. Things have changed in 35 years and now everything is automated and is cheap, even free. This area seems to need some integration so I'm digging into it.... I like digging. I've stayed out of linux but linuxcnc maybe a worth while dig. Peter

By the way a G02 interpolated arc is still a segmented move. A CNC cannot move in an arc, it has to move in small linear segments. The arc move is created to be brief. behind the arc is an algorithm that breaks it into segments....

[deadlykitten]

behind the arc is an algorithm that breaks it into segments....

if i may, how small ?

I occasionally do non-linear transient dynamic analysis on machines thats fun and the software calculates velocities, accels and jerk....

so you can control the acc/dec shape and time ?

[peteeng]

Hi DK - I don't know that's one of the secrets on CNC. See image attached I did a quick search.. Someone out there may know how an arc is discretised? Its a parameter in the line, number of segments must have a default value as well. See digging helps the learning.

RE: FE You can put in a velocity profile or a force profile then FE calculates the vels, accels then modify that until you get what you want. I use strand7 and simsolid for this sort of thing.

Re: machine control - I am rebuilding a small test router at the moment and it will become a 3D printer. Maybe linuxcnc is the go for that. A bigtreetech board has been recommended if anyone can comment on that? Peter

https://www.biqu.equipment/products/...-control-board

[deadlykitten]

if you wish to tune it, you need to get data from the feedback loop

[peteeng]

HI DK - Seems a G5 is a spline move... but again it will be segmented with a parameter.. What do you mean by "tune it" the 3D printer, bigtree board or the FE model or other? bedtime here... Peter

https://marlinfw.org/docs/gcode/G005.html

[deadlykitten]

for example:
... if you can implement whatever acc function (shape, time, etc), and you wish to know which one is best (for whatever reason), you have to analize feedback data while each one is runing
... if you wish to know bezier segmentation, you need to get data from the mcs

live/feedback data

[mountaindew]

Hi MD - lets work with your problem theres enough of the brains trust here to solve it. You have a Tormach 24r in good condition. You use Sprutcam for toolpathing and path pilot is the motion controller. So if you make a square land (150mm x 150mm? say blank is 300mm square and the square land is in a 200mm dia pocket? pocket is 10mm deep? ) and cut timber or aluminium? you say it jerks in the corners. The CAD can't get that wrong so move to sprutcam and lets look at that. Or show us a shape that you do with the issue.... just looked at sprutcam and they do robotics as well. Interesting for me... Peter

https://tormach.com/machines/routers...nc-router.html
https://sprutcam.com/

do you use sprutcam for CAD or another CAD system. Exporting from CAD to CAM can have issues as well.... mainly model tolerances if you are using a nurbs modeller...

I use Ironcad for models and sprutcam for all tool paths and g-code "NO hand edit of any g code"
Here is a quick simple example of my art to part work flow done in just a couple hours. I used my 24r cnc router and 8lcnc lathe to make this simple project.
The cad -cam system and workflow I use is very well developed and rehearsed. Its easy for me to get accurate drama free results with little overall effort. It often takes me more time to dig around and find the "scrap in this case" material to make it out of then it does to make it! The jerk or giggle I get is when the gantry changes directions at 100-180 ipm shown on the inside and outside corners of the model and the tool paths changes in direction.
As mactec explained above this would be kind of hard to control completely in cam. It can be done but would take much more effort and it would still be limited and would be better done with the control trajectory planner. Im guessing higher end faster machines have this built in. To be clear it does not effect the accuracy that I see and the results like finish are more a function of quality of cutter -feeds - speeds then anything. This machine is pretty well designed for its size, weight and speed imho! Not to fast, not to slow, not to lite!


I needed a rack to hold 5c collets on work bench that are most used!
So I designed the rack. Total time maybe 20 minutes including breaking up model into 3 different files to export into cam.

Attachment 478728

Rack Base tool paths and g-code generated! With templates that have predefined operations I use this takes maybe 5 minutes.
Attachment 478730

Acrylic rack to hold the collets upright. Again with templates that have predefined operations this takes at most 5 minutes.
Attachment 478732

Rack supports or stand offs. cam templates are also used for cnc lathe to quickly import simple model in this case and setup ops and generate g-code. another 5 minutes
Attachment 478734
Take to machines, setup material and run!
Finished project
Attachment 478736
Ready and in use!
Attachment 478738

I am not much of a machine designer at this point. I am a machine user! 95% of my time is spent using and making things with the machines 5% of my time is spent cleaning and maintaining them. I dont often spend much time trying to figure out why they dont work or work correctly Thats why I purchased them and not build them! I do on the other hand spend a great deal of time skill building in cad -cam and machine operation to get results and make the process enjoyable! If I like what I do I do it more often

[ihavenofish]

So your machine will be shaking in motion reversal due to lack of jerk control.
BUT you can take care of a lot of the harsh motion with better paths. I do not know what sprutcam's features are, but in Fusion 360 you would use adaptive clearing paths, and filleting of sharp corners. This will take care of 80% of the harsh motion. The rest you kinda have to live with, but it hopefully wont be very bad.

[peteeng]

Hi MDew - All the systems you use are good quality commercial systems and should work well. My first impression is to check the machine mechanics. Second is to send a sample code to strutcam and let them comment. Does the glitch show up in a toolpath simulation?

Ironcad - solid commercial CAD. I assume you use a step file to transfer to sprutcam. This should be a high quality transfer of geometry. I have had issues with the export displacing objects but this is immediately apparent.
Sprutcam - I've spoken to the local agent today about the robot OLP. The 3 axis mill program is high quality so should behave properly. I suspect its a machine looseness. But check with Sprut about the glitch
Pathpilot - again solid commercial MC so unless set up totally wrong should be fine
Tormach router - solid commercial machine - check mechanicals

thanks for contributing - Peter

[datac]

>>>adaptive clearing paths, and filleting of sharp corners. This will take care of 80% of the harsh motion.

While I have not yet found time or developed enough interest in using adaptive paths, it is very clear they make a difference. It's beyond onvious just watching videos of those running them. To me, there is still a feature missing.

While I have seen many discussions like this, what I have never seen is discussion regarding a potential need for both the CAM and Control side to allow for "Acceleration Changes on the fly" defined in the G-Code itself. I've often struggled with controlling breakage of very small tooling, where just inserting (manually) a lower feed rate where the tool will approach such a particular spot, leaves much to be desired.

Now, I know that my old Flashcut control (V4... cant afford the new stuff) does allow me to manually do a feed hold, change any axis' acceleration ramp and restart the tool path with those new changes. Not sure how many other controls allow that. What I always felt I needed access to, was to be able during the cad/cam stage, insert locations where we desire an axis acceleration change not much unlike the way we insert an automatically generated "lead-In" or "bridge". Obviously it would require an addition to the traditional world of G&M code, but hey, that never bothered anyone during the development years of hobby CNC controls.

Yes, there would be a lot of different ways to do this, but both Cam and Control have to be on the same page. The simplest would be to cut ALL acceleration/ramping by a user setting percentage. The next level might be similar to how we might indicate "G28 Z0" to only send the Z axis to zero, perhaps a acceleration option for a single axis would be addressed like Gxx Z(percentage).

If I was not so busy these days, I'd be calling Flashcut about this. They have always allowed a list of variables and operators in the G-Code to provide other functions during code execution, but I never recalled any such regarding changes to Accelerations or Ramping. Even if they did, it would be something you would have to manually insert because no ones Cam would have a clue it exists.

So, this is where it might require it begin even in Cad, but certainly in Cam, and finally a CNC control that understands it. I do know Flashcut did create their own complete from scratch Cad > Cam > Control environment when they took a heavy aim at the Plasma/Laser world. That type of environment might be the ONLY way to actually get this type of option, and for all I know currently, maybe they already have it ?

Fun discussion !

[mactec54]

Hi MDew - All the systems you use are good quality commercial systems and should work well. My first impression is to check the machine mechanics. Second is to send a sample code to strutcam and let them comment. Does the glitch show up in a toolpath simulation?

Ironcad - solid commercial CAD. I assume you use a step file to transfer to sprutcam. This should be a high quality transfer of geometry. I have had issues with the export displacing objects but this is immediately apparent.
Sprutcam - I've spoken to the local agent today about the robot OLP. The 3 axis mill program is high quality so should behave properly. I suspect its a machine looseness. But check with Sprut about the glitch
Pathpilot - again solid commercial MC so unless set up totally wrong should be fine
Tormach router - solid commercial machine - check mechanicals

thanks for contributing - Peter

This is the best software that is available, and can be used with some cam systems, some cam systems have this already imbedded with their software https://volumill.com/products/volumill

[ihavenofish]

Most basic systems (mach, linuxcnc) seems to just have one set acceleration. Jerk control aside, it is definitely desirable to have variable acceleration for different motion cases.

Jogging is an obvious one. I definitely don't need or really want 1G for jogging. My DDSC v3.1 allows different acceleration for jogging, but nothing more than that. Others will do different accelerations for rapids as well.

On the fly acceleration changes seems curious. I am not sure exactly how it would work. The hang up on these types of features is having them work in all cases, with overrides.

They are making progress on the linuxcnc forum for jerk control. I'm hoping there is something to test soon on a physical machine.

[deadlykitten]

on the fly acceleration : citizen, okuma ( not as direct as citizen aproach, but still )

also, okuma detects faulty acceleration caused by damaged motor

[datac]

>>>> on the fly acceleration : citizen, okuma

Interesting ! How is it implemented ? Do they have defined G/M codes for it and who's Cam program is involved to allow it to happen without direct code hand editing ?