Vibration Problems

[jpmassey]

I've been working on an issue for a while now, and I wonder if somebody has any suggestions.

When cutting arcs, the torch vibrates ever so slightly, as to cause a poor cutting edge. This doesnt happen on straight lines and circles, only arcs. I am mitigating the problem by running about 30 ipm, which makes the cut tolerable, but requires alot of cleanup. 12 ga steel @ 40 amps is supposed to be 70 ipm, which results in a jagged cut.

Stats:
-I am using servos in a rack and pinion system, with gecko drivers.
-Mach 3
-Sheetcam
-Solidworks to make dxfs

-Running in CV mode, plasma mode, angular discrimation set at 90*, no backlash compensation
-Arc are defined by only a few points in solidworks

-Hypertherm 1250, new finecut tips, .08 gap, no THC (it doesnt effect it), cutting 12 ga steel.
-4'x4' Dynacnc table

I am led to believe this is a CV problem, as it doesn't really happen with circles. I have tried every CV setting I can see, with no effect.

Any help would be appreciated.
-James

[keebler303]

If you have low count encoders, the position will be in steps no matter the CV mode or not. It may be this or that your geckos are not properly tuned and you have a constant overshoot-correct, overshoot-correct action in your closed loop which gives you a jagged oscillation.

Also could be your file generation. If circles are coded as circles but arcs are coded as linear interpolated segments, it could seem jumpy. Try increasing the accuracy of the linear interpolation to smooth out the transitions.

Matt

[DSL PWR]

Well on my table (homebuilt but I have the same controls as you) I had the same issue.

1. Move the motors away from the rack and run a program. Unless you have some neat gear you need to tune your motors using your hearing and touch. Some dithering at a standstill is normal, but when running the program the motors should run smoothly. At first my y axis was herky jerky in the slower parts of the arc.

2. The spring on my x axis wasn't strong enough and the pinion would walk out of the rack on accel and decel, causing more roughness. Also make sure the pinion is parrellel to the rack.

[jpmassey]

Originally Posted by keebler303 It may be this or that your geckos are not properly tuned and you have a constant overshoot-correct, overshoot-correct action in your closed loop which gives you a jagged oscillation. Matt

Hmm...this is an idea. I don't have an oscilloscope to measure the overshoot. Any other ways to tune the geckos?

[jpmassey]

Originally Posted by DSL PWR Well on my table (homebuilt but I have the same controls as you) I had the same issue. 1. Move the motors away from the rack and run a program. Unless you have some neat gear you need to tune your motors using your hearing and touch. Some dithering at a standstill is normal, but when running the program the motors should run smoothly. At first my y axis was herky jerky in the slower parts of the arc. 2. The spring on my x axis wasn't strong enough and the pinion would walk out of the rack on accel and decel, causing more roughness. Also make sure the pinion is parrellel to the rack.

1. Move the motors away? You mean move the pinion away from the rack?

2. This table doesn't have a spring to hold the pinion against the rack. You have to just pry the rack against the pinion and tighten it down.

[DynaCNC]

James, I ran your g-code on my machine here at the shop. The jagged arcs are about the same on our machine as they are shown on your photos. I looked at your g-code generated from vectors from your CAD program and it is generating hundreds if not thousands of little straight lines to form your arcs. This is why the standard straight lines and circles are fine and the arcs you are generating are jagged. If you can get Solidworks to generate vectors that are arcs instead of a thousand little lines to form an arc your arcs will smooth out.

David Cress

[jcc3inc]

Sir,

If your rack and pinion setup uses 14 1/2 degree rack, it is a poor choice; if you do not have a spring load of the pinion into the rack,it is also a poor setup.

Regarding the straight line approximations discussed above, I once analyzed a spiral shaped path made of these straight line segments, and found that the program was of very poor quality; on a continuous curve, there were jerky changes of direction, one segment pointed too far, the next segment pointed not far enough to approximate the curve, and viewing the path on an enlarged backplot revealed his also.

As a test, why don't you make an arc or a circle using G02 X0Y0I2.5J0 or something similar woth G02 or G03; this would eliminate the poor code if the circle/arc proved to be good!

Regards,
Jack C.

[EPIK Ltd.]

Thanks for the constructive criticism Jack, it is always gladly appreciated.

I am sitting here with Dave right now. We are watching a client/other CNCzone member cut G02 and G03s right now through 3/8 aluminum perfectly on a 2 year old DynaCNC machine with the same parts always used--- he seems quite happy.

Not to mention, if you are using SheetCAM to generate your Gcode, it will not read polylines correctly in .dxf format. I recommend going into the SheetCAM folder on your C: drive and reading the HELP manual; it has helped me greatly. You are not the only person who has come to us with this problem---SheetCAM addresses this software error.


If you need any more assistance, feel free to email me,

tyler@epikltd.com


Tyler Shinaberry
EPIK DynaTech

[jpmassey]

Dave,
Since I haven't heard anything new from yall in a while, I've been doing my own research, mostly in other forums and in the help manuals. I spent the entire last three days cutting lots of air.

What I have found:

The dxfs from solidworks are indeed 'vectors'. Sheetcam doesn't turn splines (non circular arcs) into a series of circular arcs. It turns them into a series of straight lines, with lengths determined by the detail reduction setting. The circles in the dxf are circles in the Gcode.
How I know:
If I turn the detail reduction to something like .2, it turns the spines into 'octagons'. If I put it to .0002, the spline is almost perfectly approximated by tiny little lines.
I have also been using .emf files from inkscape. The result is the same.
The files you sent me to test with was also the same way.

What I did to reduce 'vibration':
In Sheetcam:
Set the detail reduction to something reasonable. I put it at .002, as I have alot of detail in most drawings.
I upgraded to the most recent version.

In Mach:
The 'angular discrimination' option in the Constant Velocity section of Mach doesn't work very well. I tried a lot of numbers, but nothing changed. Turning it off completely helps quite a bit.

Turning off 'plasma mode' helps a bit too.

I messed with motor tuning alot. Setting reasonable accelerations help. I had it ok at 30.

I also upgraded to the most recent version.

The table:
Bolting 12ga to the side completely stopped table vibration. Overall vibration was reduced alot, now it’s only from the gantry. Works good as a down draft setup too.

To troubleshoot with the backlash problem I had the pinion smashed against the rack pretty hard. I noticed that when jogging with both axis, the torch vibrated. I pried the rack with a screwdriver with one finger and then tightened it to make sure I wasn't over doing it. Once I reduced the pinion pressure, that vibration was reduced.


In the end, now I can cut most larger (>.5") shapes up to 70 ipm. It’s still not where it needs to be. I would like to cut 14ga about 100 ipm.

I suspect the gecko drives may have a bit of overshoot. I'll have to borrow an oscilloscope and check it out.

Overall, the table works pretty good when I keep it slow. With the new electronics, the THC works great. I have cut 4 - 4x4 sheets one after another. I just need to run faster to get the time and dross down.

[EPIK Ltd.]

Great Job James,

I honor your responsibility in the matter and understanding that NO machine will ever come out of shipping perfect to run straight from the crate--- as well as the fact that plasma cutting is not going to be perfect, it requires work to clean them up, heat distortion occurs, and the flame is not perfect---compared to the alternatives, it is very cost effective for many. If a salesman of any company ever tells you that a machine will enter your door ready to run that day, they are lying. Shipping alone is capable of wacking up a machine; hence why DynaCNC gives 90 days of tech support FREE with each machine. The table was designed by Dave to be simple for the operator to adjust because adjustments are inevitable in the ownership of any machine whether it cost you $10,000 or $1,000,000. I have seen/participated in the setup of a quarter million dollar Mazak which went through 3 days of nonstop multi professional in-house setup; compared to that, the minor adjustments needed upon arrival of a DynaCNC machine are trivial, although necessary.

I am not addressing this to you as I do not know the whole situation; but for the good of anyone readings this,I cannot stress this enough…
To tell if your machine is ready to run, DO NOT START CUTTING some fancy design you plan on cutting for production the minute you get it. Start out with something simple, and without arcs, like a square or cross. From there, you can begin to see what kind of adjustments need to be made and whether it is related to software or hardware. Precise interpolation is a science; it is unbelievably hard to know every variable occurring during machine operation, especially when we are not there to personally view the operation.

As for the software issue, I do not have SolidWorks and neither does DynaCNC. When we receive a file, the only program I can use to open them for adjustment is AutoCAD; which I have learned from past experiences loads SolidWork files as polylines (which is why it is suspected that SheetCAM also reads them in this way)... But as the Gcode shows, G02 and G03 are generated--- Hence our understanding/concern of the situation. While troubleshooting, we can only go by what information we are given. Without knowing how the machine handles simple tasks (ie a square), there is no way to properly troubleshoot--- plasma cutting alone can generate enough variables (humidity, metal consistency, voltage, cleanliness of tip, etc) to make it hard to know if the cut is truly acceptable or not.

Reading the SheetCAM Manual, which is great (located within one of the language files I believe), explains how to set your line resolutions (they show .020 as reasonable for line segments when cutting plasma). Reading the SheetCam manual will tell you that SheetCAM is not capable of calculating splines or polylines; which are in essence vectorized. However, splines are generated by mathematical equations. As you discovered, resolution settings will help out if at all deemed necessary.

Good luck as you continue to tweek your machine/software. It is always good to know that there are happy customers out there and I know that Dave and I both will bend over backwards to help our customers become successful and profitable. For potential buyers of any machine, please take the above into consideration; as machine builders, we understand the frustrations… but they are worth it in the long run.

Glad you like the new electronics, Dave put a lot into that box.

Tyler Shinaberry
EPIK DynaTech tyler@epikltd.com