Backlash?

[branchy]

I have just bought a 2 year old Pro cam CNC Router.
I think I have a problem with backlash but need some confirmation.
The machine has Redcom DC Servo's,HSD 9KW (12 HP) Electro Spindle,Swiss Rack and Pinion Drive and Linear bearing guide system. It is operated with a Centroid control panel.
The spec sheet say's it has a 30m/min cutting speed capability.
I have just upgraded from a SCM record 2 with ballscrews so maybe I'm expecting too much (I'm not tech savvy I should add!)
As the photos illustrate, I seem to be overshooting corners running at a feed rate of 4000mm/min cutting a 400mm x 400mm square. The "W" on the left in the second image was being cut at a speed of 1000mm/min (result not so bad) whereas the "W" on the right was cut at a speed of 2000mm/min and RPM 18,000. The base of the "W" is my issue.
I have been advised by the manufacturer that if I insert G61 I will have sharp corners. This I have subsequently established will only work on straight lines not arcs obviously and is extremely slow if I am cutting out a full sheet of squares 400mm x 400mm.
My work involves cutting all sorts of shapes out of different materials and was advised by the manufacturer subsequent to purchasing, that their machines are primarily made for the cabinetry industry.
My question is do you guys think that my problem is backlash or am I running too fast?
And secondly, is there anything I can do to either the machine or the parameters in order to get a happy medium for what I want to do with programs that contain both straight lines and arcs.
Any advice would be greatly appreciated.
Cheers

[awerby]

If it works perfectly at lower speeds but overshoots when you speed up, that's not backlash. Backlash, which is due to a small gap between a screw thread and a nut thread. becomes evident whenever you change directions, but it's not speed-dependent. You'll see evidence of it if you're running at 1 ipm or 300 ipm. What you're noticing might be inertia, as the heavy gantry is flying towards a point, then suddenly changes direction - it's like the "whiplash" effect you'd get if you were going forward in your car and suddenly slammed it into reverse.

Andrew Werby
ComputerSculpture.com — Home Page for Discount Hardware & Software

[branchy]

Hi Andrew,
Thanks for your reply. That makes sense, what I don't understand is if the machine has a capability of cutting speeds of 1181 ipm, does that just mean it can cut at that speed so long as there are no corners involved?
To be honest, I wouldn't have bought the machine if I knew I would have to run the machine at a feed rate of 40 ipm to achieve square corners on a piece that is 16inch x 16inch.
Given that that just might be the case, is there anything I can do to improve the rigidity of my machine so that I can increase my speeds and at the same time have reasonable results or is it just a matter of changing parameters to suit my needs, depending on the job I have at hand?

[Stowe Figler]

Hey Branchy,

I have experienced this exact thing both on Multi-Cam and Onsrud wood routers. I think they're called Master-Cam machines in Australia.

Yeah your going too fast for the corner your trying to turn, and the inertia of the gantry is causing a sloppy corner. So mellow your speed a bit. The controllers and cam programs I used factored these things into the code. Some don't, and you have to program it in yourself.

Your rack and pinion system may be slightly disengaged. I used to check for this by putting a dial indicator against the vertical column by your X axis motor. Power up the motors, and push with my arms, to try to get the dial to move. When I could push the gantry over .005", I knew I had to tighten up the gap between the rack and pinion. Around .002" to .003" was perfect. You don't want it any tighter and your gonna damage things.

If I remember correctly, cutting 3/4" birch plywood with a 3/8" tool I could have a gap in my rack system and still travel the low 200 IPM with a nice inside corner. Its when I pushed her hard over 375 + IPM thats when the slop would start to show up.

I hope this helped, even though I'm a Seppo

[ger21]

Sounds like maybe the servos aren't tuned correctly? Or maybe the control isn't setup correctly?

[branchy]

Stowe Figler, despite being a seppo, your advice is greatly appreciated
I used to operate a Multicam SR2412 about 4 years ago and I don't remember having to run that slow when going around corners. I guess as you say the cam and controllers may have factored these things in with "look ahead"?
I will organise for someone to come out and check the rack and pinion and hope that it is slightly disengaged.

Gerry, thanks again. I will also follow up on those 2 things as well.

Cheers

[branchy]

Hi Guys,
Had a cnc service guy come in today to test my machines for backlash as an overall precaution. Turns out I had 0.2mm give on the dial test in the Y axis of the Procam. Not a necessity to fix considering what I do right now, but I will get it done at some point.
I still have to fine tune the servos and controller as Gerry suggested but I'm working my way through that ever so cautiously!
A big problem has been cutting out circles. They look terrible! I have two software packages, one being Ezcam the other Aspire 3.5. When I generate code for the same circle in the two different Cam's, Ezcam generates 12 lines of code with G2 and I and J commands. Aspire generates 4 pages of code with just linear interpolation.... No G2!
Is it just a matter of me getting my post processor corrected so that it generates G2 (Circular interpolation)?
Thanks again guys.
Cheers
By the way, I was able to overcome my overshooting problem by checking sharp corners box in Aspire and the results aren't too bad all things considered.

[ger21]

Is it just a matter of me getting my post processor corrected so that it generates G2 (Circular interpolation)?

Probably yes, provided you're working with true circles to start with.

[branchy]

That they are Gerry.
Encouraging!
Thank you.

[branchy]

Hi Guys,
As suspected, the PP didn't include any provision for G2 or G3 commands.
It has since been revised and all works well.
Thanks for all the help.
Cheers.

[inventor83]

Im having a similar problem with aspire. Except im using the engraving/quick engraving toolpath. There is no "straight corner" tab for engraving. When I try to engrave a square the corners are badly rounded. Any advice?