GGW! (Geometry Gone Wild)

[Diesel]

Ladies and Gents:

Has anyone ever seen SheetCam and/or Mach3 misinterpret geometry?

Take a look...

You can see the 90° angles in SheetCam with the resultant part as cut in front...with perfect fillets where there should be none.

Any ideas?

All of the other geometry on this part appears to be A-OK when compared to the .DXF (which originated in SolidWorks - customer sent me the file)
SheetCam didn't complain about the file or the post processing...no open contours, etc.

This is 18GA CRS and cut per book settings.
This is my first attempt at 18GA and also the first time I've tried looping sharp corners...the results speak volumes...it makes for very nice corners.

I've also had issues with SheetCam and/or Mach3 misplacing lead-in's and "torching" a few areas on some artsy stuff with lesser quality files.
I'll save that for another topic, but I have to wonder if the two issues are related...

Thanks!

Beers,

Matt

[_Ogre]

i had a similar issue cutting 10 gauge steel when we first had our table
acceleration issues compound on thin material and the higher speeds associated with it
use the rules in sheetcam to slow down before a 90* turn
it's not showing up on the outside corners from the looping corners, but if you slowdown before outside corners you don't need to loop

[tcaudle]

SheetCAM does not do toolpath compensation because of speeds or acceleration. Honestly it does not even know what those numbers would be for the motor tuning on your table. It simply displays what the drawing is and when you plot a toolpath (blue line) it will show you where its going to go using the tool you select. . On the other hand if you see a divergence form the toolpath in the Window in MACH then it looked at it's settings and decided it could not make the turns the g-code is calling for and it lets the toolpath "cheat " (cut corners)

SO if it looks one way on the SheetCAM screen and another on the MACH screen or cuts differently then its MACH applying the rules

Looks to me like either a bad DXF export (from the drawing program) or something on the IMPORT (into SheetCAM) is distorting the contours

[muzza]

This has come up several times here, do a search ot have a look through but the quickest and simplest remedy is to export your your drawing as an svg file to bring into Sheetcam.
Murray

[SeanP]

Solidworks outputs great dxf files, I never have a problem with those at all, post the dxf if you can, just to rule out your setup.

[Diesel]

acceleration issues compound on thin material and the higher speeds associated with it

Yeah, that makes sense. Lucky me. This part is the first time I've tried to cut 18GA and it failed miserably. The speed increase from 250 to 325ipm had all sorts of consequences.

SheetCAM does not do toolpath compensation because of speeds or acceleration. Honestly it does not even know what those numbers would be for the motor tuning on your table.

That's great info - thank you!

This has come up several times here, do a search ot have a look through but the quickest and simplest remedy is to export your your drawing as an svg file to bring into Sheetcam.

I recently created a Christmas ornament using a file I found on here and then modifying it with CorelDraw. When doing the traditional .DXF workflow, it imported into SheetCam just fine. When I tried the .SVG import workflow, the preview and the geometry in SheetCam looked like a cubist/Pablo Picasso piece...it was really messed up. I often use SheetCam as a filter - if it doesn't bitch about open paths and the post runs, then I hand carry the .DXF on a thumb drive out to the shop. I'll have to do some research on how to make the .SVG export/import workflow a success.
Here is the ornament:

MetalBuffet_2015_ChristmasOrnament.dxf

(496.3 KiB) Downloaded 79 times

MetalBuffet_2015_ChristmasOrnament.dxf

(496.3 KiB) Downloaded 79 times

Solidworks outputs great dxf files, I never have a problem with those at all, post the dxf if you can, just to rule out your setup.

Here is the .DXF as output from Solidworks. I've cut other parts for the same customer using the same seat of SolidWorks without issues. But I did have massive issues with an intricate piece - the gantry motion just stopped when it was about 90% done with the 270ish pierces. Man, was I ever heated...then to have it happen again...grrr...

GGW.dxf

(45.43 KiB) Downloaded 75 times

GGW.dxf

(45.43 KiB) Downloaded 75 times

Thanks Gents!

Regards,

Matt

[muzza]

Both of those files import into my Sheetcam fine. Can you upload the svg that you had trouble with.
Murray

[Diesel]

Both of those files import into my Sheetcam fine. Can you upload the svg that you had trouble with.

Yes, they both import into my SheetCam just fine as well.
The issue is when they are cut the geometry is not correct.

Here is a picture of the ornament.
.SVG on the left (scaled down a bit) that I cut last night (Exported the Corel .CDR file into Inkscape and then saved it as Inkscape's native .SVG)
.DXF on the right - cut on Christmas (Exported from Corel as a .DXF).

Both share a resemblance to the .SVG/.DXF but they have issues...and the issues with geometry being off are in the same spots.
Both cut with same settings in SheetCam. The .SVG was even cut with new consumables.

Here is the .SVG from last night...imports into SheetCam and Mach3 with no issues.

MetalBuffet_2015_ChristmasOrnament.svg

(45.21 KiB) Downloaded 85 times

MetalBuffet_2015_ChristmasOrnament.svg

(45.21 KiB) Downloaded 85 times

Regards,

Matt

[WyoGreen]

Matt, I took a look at your dxf. While it looks fine, there are a couple of things that I have found in the past to cause problems. One is Sheetcam seems to do best with polylines, your dxf imported into my Cad/Cam program as splines. The second thing I have found that sometimes causes problems is all the lines in each cut-out not being joined together as one. I changed your dxf to reflect what I normally do to my files before running them thru Sheetcam, see if that makes any difference. Both files look the same in Sheetcam, so it will be interesting to see if they process differently.

Steve

MetalBuffet_2015_ChristmasOrnament2.dxf

(113.06 KiB) Downloaded 78 times

MetalBuffet_2015_ChristmasOrnament2.dxf

(113.06 KiB) Downloaded 78 times

[Diesel]

One is Sheetcam seems to do best with polylines, your dxf imported into my Cad/Cam program as splines. The second thing I have found that sometimes causes problems is all the lines in each cut-out not being joined together as one. I changed your dxf to reflect what I normally do to my files before running them thru Sheetcam, see if that makes any difference. Both files look the same in Sheetcam, so it will be interesting to see if they process differently.

Thanks, Steve!
I downloaded the file - I'll give it a whirl!

What process/program did you use to make these changes?
On edit: I opened your modified .DXF in AutoCAD 2004...my inexperience is showing...I think I'm seeing way more nodes than before...

Regards,

Matt

[Diesel]

I changed your dxf to reflect what I normally do to my files before running them thru Sheetcam, see if that makes any difference. Both files look the same in Sheetcam, so it will be interesting to see if they process differently.

I cut your new file twice.
Once with the scribe and once without the scribe and without any path rules.
The geometry still isn't correct.

Here are the parts.
From L to R (newest to oldest): No scribe/no path rules, your file as-is with normal path rules, my old .DXF from Christmas Day.

On the original part (far right in the above photo), the geometry on the tree trunk is actually pretty close to the CAD file and the toolpaths. The other two are a little off, not to mention portions of them being torched off for some reason.

Regards,

Matt

[WyoGreen]

My compressors down right now, waiting on a part. Soon as it comes in, I'll try cutting your file on my machine. That might point us to where the problem lies. Maybe someone whose machine is up can cut it sooner (hint, hint)

Steve

[Diesel]

Very cool - I'd be interested to see if other folks can cut this without issue.
Thanks for your help!

Regards,

Matt

[Diesel]

So this issue seems to boil down to the Geckodrive inside the CandCNC controls morphing from microsteps to full steps beyond 4 revolutions per second (at the stepper).

On my table with 3:1 belt reduction (and given the gear diameters and so forth), this occurs at 251 ipm.
That means I can cut with a resolution of 0.00052" at speeds up to 251 ipm...after that, the resolution drops quite a bit.

As luck would have it, 16GA @ 45A (fine cut) is 250 ipm...and I've had good luck cutting that.
18GA @ 45A (fine cut) is 325 ipm...and my table is rounding corners as a result of being in full step mode.

I've experimented with slowing down on corners and have had decent results, but I may need to resort to the 'slow speed' chart and deal with the dross.
After looking around on some other forums, there are plenty of folks who can't cut above 150 ipm or thereabouts, so I consider myself lucky.

Many thanks to those that responded!

Cheers,

Matt