Mach3 cutting different on different speeds, the same Gcode. Why???

[lopata]

Hello fellas cnc enthusiasts.

I have build up a High speed machine in last few weeks, and I am having trouble with understanding Mach3 logic.

My machine setup.

Leadshine easy servo motors with drivers, 4Nm.

Max feedrate 10000 mm/min

Acc: 2000mm/s/s goes up to 4000 mm/s/s without problems, but that is insane acceleration.

Ball screw 2505 C3 precision.

All axis are below 0.01 true, with work table max 420x420x100 mm.

Machine does not stutter and shakes. Cutting in pure motion, without any hiccups.

Few problems which occurred.

1. Mach3 does not cut the same paths on the feed rate on 100% (around 30 mm/s) and on 50 %. How can this be, and why is that?

2. Making a part on CV=180 is not the same as CV=1, or ever CV=0.1 -- Can anyone explain a bit on this.

Questions:

1. Is this common issue with Mach3, and should I consider moving to EMc2 or Mach4?

2. What is the lowest CV tolerance that can be set? Mine is set to 0.1 mm, but I will be going to 0.01 or even less.

I have been making JIGs for my parts, and to tolerances from that CV is affecting my parts significantly. I should be running tolerances around 0.005 mm on 100 mm range, but there are tolerances greater than 0.1 mm.

The parts that has been cut on CV=180 cant fit my JIGS at all, while parts made on CV=1 can fit but with some convincing.


I have read up all the common issues with CV and Mach3, but I just need an answer why does Mach3 cuts differently on different speeds.

Thank you

Marko

Similar Threads:

• Feeds and Speeds DOC Gcode
• How do you decide cutting speeds for cutting plexiglas?
• why does mach3 alter my gcode?
• Image to mach3 gcode
• Mach3 Feeds & Speeds

[awerby]

CV stands for "Constant Velocity", called out by the G64 command. That tries to keep the tool moving at the same speed no matter what's happening in the toolpath. So when it gets to a corner, just like a car that's going fast, it's going to swerve around it instead of one that slows down to make a sharper turn. The less "look-ahead" you have set, or the more speed it's told to run at, the less adjustment it will be able to make. If you want it to follow your toolpath exactly, without cutting any corners, you can set it to "Exact Stop" (G61) instead. But that usually results in jerky motion and wasted time. Thus you end up having to tweak the CV settings in Mach3 until it gives you acceptable results. So get into the General Logic Configuration menu under CV control and try changing the "stop on angles" value from 0 to something short of the sharpest angle in your toolpath. You can change the CV distance tolerance to something besides 180 In General Configuration, you can also increase the look-ahead, which can help. To read what Art Fenerty, the originator of Mach3, has to say about it, look here: https://www.machsupport.com/forum/in...?topic=1724.10

[lopata]

Hello Andrew, thanks for the link. I have read that one also, but will do it again.

My current setup on the acceleration is 2000mm/s2, which is pretty high. Actually, maybe acceleration is extremely high for the hard aluminium.

Regardless of acc, the sharp corners get rounded. When I reduce the CV, its better.

I dont have the problems with CV as much, as all of my parts are rounded, and there are no sharp corners.

My problem is that Mach3 is making shortcuts when applied with different speeds. For example: If I run it with 30 mm, and slow it down to 50 % of feedrate, the mach starts to be more precise. If I return it back to 100%, it will not be precise again, which is disturbing thought.

Also, I am milling a socket which is 6.2 in diameter, with 6 mm end mill, and that sockets are making troubles, not fitting in the JIG. Roughing and finishing passes, but also finish pass is also a bit high speed.

I could be missing something. What I will try, is to make smaller cutter, and make another jig with new setup of CV.

What about EMC2 or Mach4?

Image will show you.

First two are my products, and last two is machine while being built.

Will also upload the video of milling.

[ger21]

You might want to look at UCCNC. Several people have found it's trajectory planner to be far superior to Mach3.

[samco]

Or linuxcnc... You can tell linuxcnc how close you want it to follow the programmed path. G64P.01 says go as fast as you can but don't deviate more than .01mm to do it. (for metric program)

[lopata]

Thanks fellas,

I have mentioned that I am using closed loop steppers from Leadshine. As the best combination from servos and steppers, but with lots of power and precision.

Last time I was having this problems, I was sure that my hardware (machine) was the issue, but now machine is heavy duty designed, and mach3 has to be the issue.

I am leaning towards the linuxcnc, and I would like to know are there any support for closed loop.

@Ger21: You are everywhere, and thanks for that blue Mach screen, have been using it on my last MM machine.

[ger21]

The Blue screen is not mine. Unless you mean the Aqua screen?

[lopata]

I was sure that was your screen. My bad

Regarding the issue I am having. Maybe the pictures will explain better.

First picture was made on 100% feedrate, on around 25 mm/s with CV=180, but unchecked.



Second pic shows the same Gcode but on 50% feedrate, reduced in mach3. Also CV=180, and unchecked.



How can this be and why is it happening?

Tomorrow I will do some test on CV settings =0.000001 units (mm) and will run the same Gcode on same speeds.

In backup, I will give it a go on EMC2 to see how it goes.

I know I am doubling my post on cnczone and machforum, but I really need answers.

[samco]

If whatever you are using for hardware is compatible between the two (linuxcnc and mach3) - why not try linuxcnc. Its stepconf wizard will import a basic mach3 xml file.

Stepper Configuration Wizard

If the mechanics are not the issue - then you could be seeing mach rounding corners at higher speeds. Again - linuxcnc you can set how close you want it to follow programmed path - G64Px.xxx

Here is an example of mach3/4 motion plotted using linuxcnc. (mach 4 has the same trajectory engine as mach 3)



sam

[ger21]

How can this be and why is it happening?

Because Mach3's trajectory planner is flawed. The only workaround is to cut at slow feedrates with high acceleration. Or use a different control.

[lopata]

Thanks for answers Sam, Gerry,

I am moving to Linuxcnc for sure, but I just wanted to give you my update of today.

Current machine setup is:

Velocity 6000 mm/s
Accleration 1000/s/s (was set to 300 mm/s/s)

In the video, I was engraving with 35 mm/s feedrate.

CV is set to 0.0001 (0.1) units, and Lookahead is 120 (Old value was 20).

The finish move is clearly slowing down and there is slight jerky feeling, but it was due the configuration of the spline.

In pictures you will see much higher precision, and all the corners are pretty correct.

Reference: End bit in picture is 6mm in diameter. and the top letters are 2 mm in height.





Still more to test, but I cant wait for linuxcnc to mount it all up.