Another Constant Velocity Question

[nick7251]

I have notice at higher speeds my machine is stopping and starting at every little node in the file. I am sure it pauses at lower speeds too, but it isn't noticeable because of the slow speed. I am also pretty sure I have CV set up correctly in Mach3 as I have been reading about this topic to death, but I won't rule out that I missed something.

My question pertains to the Post Processor. I am using sheetcam. Do I need to have G64 written in my post to enable CV mode? If so, where should I write it in? I have dug in my post and it isn't in there currently.

Thanks for the help.

[AREA]

I am just beginning to try and understand g code myself and am curious on this also.

I believe the G64 just turns on the smoothing but there are other setting somewhere that allow you to tune its sensitivity.

Anyone else have some insight on this?

[nick7251]

I think from what I have read the G64 smoothing is what enables Constant Velocity. Then in Config->general config you can "tune" the CV control. I just don't know where to put the G64 in the post to enable this. Or if it is truly needed. I love this forum for stuff like this... A lot of very smart people here.

[robertspark]

general configuration tab.

Look at your lookahead, this needs to be about 200 lines so that the buffer remains full with a motion controller.

Also look at "CV Distance Tolerance"

here is a document for you to read https://www.machsupport.com/wp-content/ ... ngs_v2.pdf

[nick7251]

Thank you Robertspark. Lots of info on those two settings everywhere. I am more curious of the need of a G64 in the output code of the post processor to enable those settings?

[robertspark]

all motion control software I have seen have a default setting for G64 or g61 (which mach3 has radio buttons on the general config tab)

hence once it is set there is no need to change it from G64.... unless of course you or your gcode flip between the two then good gcode would set and clear all modal commands for the task at hand ...eg you will see a lot of gcode / even the default mach3 initialisation string have g80 programmed (to clear any canned cycle.... that may still be active..... although few today probably use canned cycles in the hobbyist side of CNC)

[nick7251]

Okay good information. That clears up a lot, but now it raises another concern. I have CV set, but I am noticing it pause on nodes within an arc. That is what was leaving me to believe even though CV is set that it may not be active for some reason. Any ideas on what to check?

[robertspark]

..... there are no nodes in an arc (G03/G02)..... except at the start and end that is

if your CV tolerance is small then the machine will decelerate between the junctions and accelerate at the other side of the junction.

there has been various long running discussions on this over time, I will try to find and link to the last one. there are differing points of view but constant velocity is simply not a velocity which is constant it is more just the opposite of exact stop.

if we can agree that exact stop requires motion to actually stop at the end of each gcode motion command in anticipation of the next.

then the opposite of this is simply a continuous motion through all of the nodes. not the maintaining of a constant velocity.

eg.... when you drive your car you generally drive it in constant velocity mode.... you don't stop at every junction or bend in the road. but constant velocity is not the maintaing of a specific velocity (such as setting the cruise control at 50mph and you just turning the steering wheel to navigate your way around a city).


here is something for you to read

viewtopic.php?f=4&t=30670&p=187054&hili ... al#p187054

viewtopic.php?f=4&t=30670&p=187054&hili ... al#p187017

we never did get to the bottom of rods math (or he did not disclose it).... but does it really matter....

[nick7251]

Thanks Robert. I've been reading some of your other posts over on the sheetcam forum as well. Good info. I guess I was calling the start and end points of the arcs nodes. I see now that is the wrong term. Even still the machine is pausing at those points even though CV is turned on. What would you say a good starting point would be for CV dist Tolerance? In the meantime I will dig through the links you provided and try to find the answer myself.

[robertspark]

My advice [note, I own 1 plasma cutter, 1 mill, 1 lathe & 2 routers all cnc in a hobby environment so never classify myself as a has-been under pressure (expert)] is

for a minimum tolerance:
to adjust the CV to the radius of the cutter or 1/2 the kerf width.
(no point in less than this as the cutter ain't going to cut any smaller [in 2.5D or as a rough cut in 3D])

for a maximum tolerance:
to adjust the CV to the diameter of the cutter or kerf width. (this is what I use with plasma)

I don't make anything "high precision" {if I did / when I have needed to, I hire someone to do machine / laser cut it from a CAD file}

With plasma I start at the kerf width, and then think what is an acceptable number (I would accept for rounded corners). For artwork you probably want them nice and tight (eg: tree of life sort of stuff viewtopic.php?f=6&t=30254&p=182675&hili ... fe#p182675 ...... but then the corners are sort of rounded for the most part anyway but there are a few tight changes in direction)

For engine mounts, gussets and general transmission bracketry I've used a larger radius (1/8") [CV setting] as it will be welded up anyway and a nice radius is helpful sometimes.

Outside corners I tend to loop my corners so the velocity is kept up and you still get a nice tight corner (1/4")

note, I use UCCNC and G64 can be programmed with settings to adjust the tolerance from the gcode file from the default setting (which is also possible in LinuxCNC) but is not possible (from what I can see in manuals in Mach3 or Mach4)

find a number you are happy with... [trial and error]

kerf widths are given in the hypertherm manuals and are around these sort of numbers (depends on the torch and consumables etc etc.... check your specific operator manual for the charts)


It would be nice to know what others do use (but everyone seems tight lipped on some settings / tolerances they use and why)

[Rodw]

we never did get to the bottom of rods math (or he did not disclose it).... but does it really matter....

Neither did I. Time poor I cry! I have had a go at it myself but made an error with unbalanced units which I picked up later. I've asked 3 engineers and they all came up with a different answer....

Come to think of it, Robert, I am still waiting for your exam paper to be returned.

I think these are the two simultaneous equations that we should solve for.

[robertspark]

I've been busy too.... in the last month I've been made redundant (I saw it coming since the very start of covid19 in the UK), started tryng to setup on my own from scratch (website, photos, examples etc) + find alternative work. officially unemployed Monday and had 2 job offers by Tuesday PM, and I've accepted one .... so one less worry.... I'll have another look back at that post again

life.... never fails to amaze / confuse / change!

[Rodw]

I've been busy too.... in the last month I've been made redundant (I saw it coming since the very start of covid19 in the UK), started tryng to setup on my own from scratch (website, photos, examples etc) + find alternative work. officially unemployed Monday and had 2 job offers by Tuesday PM, and I've accepted one .... so one less worry.... I'll have another look back at that post again

life.... never fails to amaze / confuse / change!

Glad you were able to get off the redundancy scrap heap. Covid has been kind to us so record sales has cut into my plasma play time. But this month the government support for businesses cuts out so we'll see how it goes from here. I think we will continue with strong sales.

[robertspark]

yeah, the governments support started to be cut back from 1st August here, and ends 31st October (for employees).... for businesses I'm not sure, but its all done with loans I think.... which have to be paid back at some point and not just general taxation later on.

I think the worst (jobwise) is yet to come.... but hope as I ususally am... 100% wrong!

prepare for the worst, hope for the best.

back to plasma cutting / enough of problems / politics / points of view or opinion!

If you can't cut it, screw it, glue it, weld it or get paid for it. Its not important!

[nick7251]

for a minimum tolerance:
to adjust the CV to the radius of the cutter or 1/2 the kerf width.
(no point in less than this as the cutter ain't going to cut any smaller [in 2.5D or as a rough cut in 3D])

I have my CV distance set to my kerf width right now. I'm still getting the little pauses at the start and end points. What other settings should I look at? Again this is Mach 3 unfortunately. Don't have it in my budget to get a new controller to shift to Linux based software.

[nick7251]

Robert, in your screen shot above you set CV distance to 25. Is this mm? So that would be 0.984 inches. That is quite a bit more than three radius of the kerf. I'm thinking I'm way of on something here.

[robertspark]

ignore those numbers that is just a demo install of mach3

[nick7251]

ignore those numbers that is just a demo install of mach3

Okay. So I have 0.06 inches in my CV distance. I know that it was suggested to do half the kerf so I might update to 0.03". Sorry to need so much hand holding. Does that seem right? If so, I am back to square one on thinking that the machine isn't actually in CV mode even though I have it set. With those numbers correct it still pauses.

[robertspark]

Try setting the number to a large number (like shown in the manual I listed above / earlier).

put the number at 25 and run it again and see if it slows for the nodes?

(I have probably asked this.... ) but I'll ask it again.... are you using a motion controller, if so, which one? Does it have a buffer adjustment? try increasing the buffer if it does. Increase the lookahead lines to 200.

I've just looked for the setting but I cannot see it.... but you can / could turn off the toolpath and see if that improves things.
Mach3 although being an older piece of software uses the toolpath quite a bit and if you have an older PC sometimes I've seen / heard of issues with graphics cards causing other issues (hence turning off the toolpath [which I cannot see where the checkbox is for turning it off] can improve things (or at least allow you a test run to try to see if its causing the issue.

As pointed out by Rod, acceleration is key with plasma cutting so if your acceleration is low, when there are changes in direction the node junctions can be more apparent (even in CV mode, with a small CV error setting)
Sorry this is a bit washing machine mechanicish..... try this / that and see if it works....

But you have an unusual problem (or others would be shouting from the rooftops) if it's not one of the issues listed above (low acceleration, small CV error / too small for the acceleration setting, small lookahead, graphcis card not up to scratch [old pc / wrong graphics driver] {unlikley these days as mach3 spec is soooo low.... but possible})

[nick7251]

Try setting the number to a large number (like shown in the manual I listed above / earlier).

put the number at 25 and run it again and see if it slows for the nodes?

(I have probably asked this.... ) but I'll ask it again.... are you using a motion controller, if so, which one? Does it have a buffer adjustment? try increasing the buffer if it does. Increase the lookahead lines to 200.

I've just looked for the setting but I cannot see it.... but you can / could turn off the toolpath and see if that improves things.
Mach3 although being an older piece of software uses the toolpath quite a bit and if you have an older PC sometimes I've seen / heard of issues with graphics cards causing other issues (hence turning off the toolpath [which I cannot see where the checkbox is for turning it off] can improve things (or at least allow you a test run to try to see if its causing the issue.

As pointed out by Rod, acceleration is key with plasma cutting so if your acceleration is low, when there are changes in direction the node junctions can be more apparent (even in CV mode, with a small CV error setting)
Sorry this is a bit washing machine mechanicish..... try this / that and see if it works....

But you have an unusual problem (or others would be shouting from the rooftops) if it's not one of the issues listed above (low acceleration, small CV error / too small for the acceleration setting, small lookahead, graphcis card not up to scratch [old pc / wrong graphics driver] {unlikley these days as mach3 spec is soooo low.... but possible})

My controller is the Pokeys57cnc controller. I am researching if I can adjust it's buffer. I already have Mach3 set to look ahead 200 lines.
My PC is new, but it may be short on graphics memory. It just uses the built in GPU. But it is a lot better than my old system.
As far as my motor settings I have: Steps Per = 1357.707, Velocity = 349.98, Acceleration = 27. I did not set these. I kept the settings from the factory when I changed out the controller to the Pokeys. But given the other things the factory just straight up got wrong (star grounding the table, THC implementation, Floating Head Post code, and other things I've had to fix) I would not be surprised if these numbers aren't the best for my needs. I did change the Steps Per to be more accurate. It was gaining about 1/8 inch across the length of my table before. Now it is dead on nuts.

Note: I bought this table used, but the original owner told me he didn't change anything.

[Dfabltd]

what is the file your trying cut or is it with every file

[nick7251]

Seems to happen with every file. I confirmed that G64 is active in Mach3. So it is running in constant velocity mode. I am guessing now that my CV Dist tolerance is set too small. Haven't had a chance to go test and find out. I have it set to .06.

[nick7251]

I got a chance to change my CV Dist tolerance. I changed it from .06 to 20, but that seemed to make no difference, or even make it a bit worse. Hard to tell, but it didn't fix it.

[nick7251]

Any other ideas on what I can check? I'd love to get my machine to run without pausing at every new start point.

[Rodw]

Any other ideas on what I can check? I'd love to get my machine to run without pausing at every new start point.

Well I could say use Linuxcnc
I can't really help because I've never used Mach3

But by the sound of it, you have lots of line segments in your files so its likely exacerbating the issue. I don't do arty stuff so don't have problems like you describe. I would look at your artwork to see if it could be streamlined.

Acute angles > 90 degrees can be problematic (eg star points). On a diagonal, a CNC machine can accelerate faster than if it was pure X or pure Y becasue both motors can contribute to the movement. On a star point aligned with the X or Y axis, the motion is going to be coming all from one axis so it has no choice but to stop and reverse direction. In fact, it would be interesting to see the difference in quality with starpoints between one aligned north or east with one aligned north east on a 45 degree angle to the axes directions. Can you add a small radius or fillet on each corner?

I will say that a recent motor upgrade allowing much higher acceleration has made a big increase in cut quality as the torch does not stay below the feed rate for long!

Linuxcnc is significantly different than Mach in this area is there is no such thing as constant velocity mode. In addition to the P parameter that specifies the maximum distance you can be from the path, the additional Q parameter of the G64 command enables the naive cam detection and will straighten out any consecutive line segments where the deviation is < Q. This link gives some interesting background to the issue you face from a motion planner perspective.
http://linuxcnc.org/docs/2.8/html/user/ ... ry-control
I've never played with them but there are a number of configuration settings available if you follow the link where it says
"For more information on the Trajectory Planner ini options see the Trajectory Section in the INI chapter."

Thanks Robert for the suggestion re using kerf width as a tolerance. I've always suspected we've blindly adopted default tolerance settings designed for a mill and need to be more plasma specific. I will try that.