[conanh]

Hi! I'm fairly new to the CNC routing world, but am learning and having a great time.

At the makerspace I belong to, we have a CNC router that's been giving me some trouble. I'm not sure where the problem lies, so I thought I'd start in this forum since it uses Linux CNC for machine control.

The most common issue is that sometimes the tool will slow way down and move rather jerkily. I've had this happen on exports from 3 different CAM programs. The simulation in Fusion 360, which I'm using now, shows it moving moderately and smoothly through those parts though.

The second issue is that, at least last time, the machine did not follow the toolpath that Fusion 360 simulated. It's like it skipped some parts or mixed a few sequences around. For example, in the simulation the tool ramped down, then stayed engaged with the stock while it cleared an entire area, but in real life it ramped down, cleared just a little, retracted, moved elsewhere in the area, ramped down, cleared just a little, then retracted, moved and ramped down again. Perhaps this is a bug in the G-Code export--I'm still going through the output--but I thought I'd mention it in case this sounds familiar.

Anyone have ideas about what the problem (especially the first one) might be or where to start troubleshooting?


Many thanks,

Conan.

[NitroCH3NO2]

Conan,

The first issues of slow jerky movement leads me to believe that your program is using exact stop mode, G61. In this mode LinuxCNC will go to the exact endpoints of each line of code and stop before proceeding to the next line of code. This could be pronounced with small line segments used to make an arc for example. It would move from the start point of one line to the end point and stop. It will then move from that point to the next endpoint then stop. If the line is not long enough to reach full feed rate due to acceleration and deceleration the movements will be slow.

This can be fixed by using G64 for continuous feed. See the following on the wiki

LinuxCNC Documentation Wiki: TrajectoryControl

Also see the following for more information on G64.

G Codes

The issue with the new program and it skipping around I am not sure about. Check your g-code carefully to see if it was generated correctly.

[NitroCH3NO2]

Also If you are doing 2D paths you should be able to have Fusion 360 generate arc commands (G02,G03) instead of short line segments (G01). Look at your post processor options. If you are doing 3D paths arcs might not work.

[svenakela]

Yeah G64 P0.01 (for millimeter) will do the trick.

What is the G-code like? Can you share it?

[samco]

If that still isn't good enough - the next major release of linuxcnc (v2.7) has a new trajectory planner which is an awesome improvement.

sam

[conanh]

Thanks so much for the replies! I thought I had responded right away, but never hit post.

I checked my g-code, and it has no G61s or G64s.

Also, it looks like I have a good amount of G2 & G3 commands, along with plenty of G1 commands.

I still haven't had a chance to go through the G-code line-by-line, but am hoping to get to that today. He's the g-code if anyone is interested in taking a look and letting me know if you find anything odd: https://gist.github.com/conanh/22b1cab5024c6d0dcc26


Many thanks again!

Conan.

[NitroCH3NO2]

As good practice you should put one of the path codes G61 or G64 in the preamble of your G code. And change between them in the code when required.

I simulated the G code in your gist file in cut viewer mill. It seems that everything runs continuous no jumping around to different areas of the part. It appears to be a snake.

[svenakela]

It's not a snake really, we even did that on Heidenhain controllers sometimes to avoid shaky paths.

[conanh]

Nitro & svenakela, thanks so much for your replies!

I spent about 6 hours yesterday trying to troubleshoot this problem (the stopping during cutting) and don't really feel like I'm any closer.

Here's 9 second video of what I'm seeing: CNC stopping - conanh's library

From what I can tell, it may be pausing when it switches between types of moving commands (e.g. G1 -> G2/G3 or vise versa), I'm not 100% sure, but watching the code go by and the machine moved, that's what it seemed like.

To clarify the problem, the machine will accelerate into a movement then decelerate almost completely before starting the next movement.

I'll be spending more time this evening trying different models, but if anyone has more ideas, I'd love to hear them!

And, yes, it is a snake

[svenakela]

Nitro & svenakela, thanks so much for your replies!

I spent about 6 hours yesterday trying to troubleshoot this problem (the stopping during cutting) and don't really feel like I'm any closer.

Here's 9 second video of what I'm seeing: CNC stopping - conanh's library

From what I can tell, it may be pausing when it switches between types of moving commands (e.g. G1 -> G2/G3 or vise versa), I'm not 100% sure, but watching the code go by and the machine moved, that's what it seemed like.

To clarify the problem, the machine will accelerate into a movement then decelerate almost completely before starting the next movement.

I'll be spending more time this evening trying different models, but if anyone has more ideas, I'd love to hear them!

And, yes, it is a snake

Nope, no snake. And it has nothing to do with your CAM really, if you wrote a program by hand you will see the same behaviour.

It is not a switch between G1 and G2, it happens between all code lines and it is clearly a G64 setting fix. I do that on my LinuxCNC machines too and I run full speed through the entire program without stop & go-motions.

But it also seems that you have a VERY long acceleration and deceleration settings, and that is something you have to adjust in LinuxCNC. As long as the acceleration is low you will never reach high speed on short movements. If you don't know how to do it, make a backup copy of your machine settings and start the Config Wizard. Test a higher acceleration rate and you will gain not only faster increments but a faster machine in total as you will reach higher speed on all lines executed in a G-code program.

I would say you should have such a high acceleration your machine is shaking (which also can be even higher if you add a wall mounted support to your router table). When you are running a long program the G64 setting will smooth the lines out and the shaking will not be present and you will cut much faster in general. And if it still is shaking, slow down the speed in Axis instead of the G-code.

MadCAM generated tool path, LinuxCNC, G64 P0.01 (mm).