Cutting Polycarbonate Profiles, Help!

[Kberry]

Hi all,

I am attempting to cut 2D profiles from 0.25" Polycarbonate sheet. We are getting a chattery edge on all radius as well as entry/exit points. I am using a Shopbot Buddy and an Onsrud 66-087 single O-flute Edge Rounding cutter at 100ipm and 15,000rpm.

We are getting great results in the straightaways but the curves are bumpy and the entry and exit point is very chattery. I think by extending our entry/exit lengths and radius I can fix that problem, but what settings do I need to alter to get a more consistent finish in the curves?
I read thru the forums and tried altering the ramp settings but there was no change in our edge quality.

Thanks in advance

Keith
IDS
Venice, CA

[Gary Campbell]

Keith...
Did you save the file using the "arcs" postP?
Which program did you create the vectors with?

[Kberry]

Gary,

We use Rhino with RhinoCAM and export to the Shopbot. Postprocessor is Shopbot, not the ShopbotGcode.

[Gary Campbell]

Keith...

It is pretty likely that your design uses short line segments instead of arcs for radius vectors.
You may want to export vectors to one of the CAD/CAM apps and post using the "arcs" post. It uses gCode arcs and results in much nicer radius cuts.

[joe]

Keith,

I think Gary is correct. This has been a problem with SB. Circles and curves which are made from short links seldom cut smoothly. Also Polycarbonate shows every defect. I'm cutting letters from this material which is .75" thick using a V bit. It's a test of nerves since it doesn't sand very well.

Joe

[Kberry]

Hey thanks guys,
I tried to create a Gcode file but it was turning off our spindle when I started the file, any suggestions I dont really understand the coding aspect that well.

Also our machine is really new, is there any sort of "breaking in" time, where we need to go back and readjust our motors, track etc?

[Kberry]

Here are some photos of our recent profiles you can clearly see that pattern bump/ridge

http://i776.photobucket.com/albums/yy50/keithb2077/005.jpg
http://i776.photobucket.com/albums/yy50/keithb2077/004.jpg
http://i776.photobucket.com/albums/yy50/keithb2077/003.jpg
http://i776.photobucket.com/albums/yy50/keithb2077/002.jpg

[jerry_stanek]

I would try a rough cut with a straight cutter with an offset then the finish cut so you would only be taking off a small amount and putting the bull nose in.

[Kberry]

Ok I ran a Gcode file, *.gcc and got the Same Problem. This leads me to believe it is the ramping in the Shopbot controls, any suggestions?

I also tried a straight cutter roughing and the bullnose only taking .020" and still no luck.

[Kberry]

Is this correct for Gcode? I had to delete M03 as a command because it was turning off our spindle.

G90
G00Z1.0000
X14.9403Y23.3034
G01Z-0.09F 40
X14.6903F 40
X14.625Y23.3077F 80
X14.5608Y23.3205
X14.4989Y23.3415
X14.4403Y23.3704
X14.3859Y23.4067
X14.3367Y23.4499
X14.2936Y23.499
X14.2572Y23.5534
X14.2283Y23.6121
X14.2073Y23.674
X14.1945Y23.7382
X14.1903Y23.8034
Y24.9284
X14.1862Y25.0427
X14.174Y25.1563
X14.1537Y25.2688
X14.1254Y25.3796
X14.0893Y25.4881
X14.0455Y25.5937
X13.9944Y25.6959
X13.936Y25.7943
X13.8708Y25.8882
X13.7991Y25.9772
X13.7212Y26.0609
X13.6375Y26.1388
X13.5485Y26.2105
X13.4546Y26.2757
X13.3563Y26.334
X13.254Y26.3852
X13.1484Y26.429
X13.04Y26.4651
X12.9292Y26.4933
X12.8167Y26.5136
X12.703Y26.5258
X12.5888Y26.5299
X10.5888
X10.5163Y26.5255
X10.4448Y26.5124
X10.3755Y26.4908
X10.3092Y26.461
X10.2471Y26.4235
X10.1899Y26.3787
X10.1385Y26.3273
X10.0937Y26.2701
X10.0562Y26.208
X10.0263Y26.1417
X10.0047Y26.0724
X9.9916Y26.0009
X9.9873Y25.9284
Y23.4284
X9.9914Y23.3324
X10.004Y23.2372
X10.0248Y23.1433
X10.0537Y23.0517
X10.0905Y22.9629
X10.1348Y22.8777
X10.1865Y22.7966
X10.245Y22.7204
X10.3099Y22.6495
X10.3807Y22.5846
X10.457Y22.5261
X10.538Y22.4745
X10.6232Y22.4301
X10.712Y22.3934
X10.8037Y22.3645
X10.8975Y22.3437
X10.9928Y22.3311
X11.0888Y22.3269
X13.8388
X13.8937Y22.3313
X13.9474Y22.3441
X13.9983Y22.3652
X14.0454Y22.3941
X14.0873Y22.4299
X14.1231Y22.4718
X14.1519Y22.5188
X14.1731Y22.5698
X14.1859Y22.6234
X14.1903Y22.6784
Y23.8034
X14.1945Y23.8687
X14.2073Y23.9328
X14.2283Y23.9948
X14.2572Y24.0534
X14.2936Y24.1078
X14.3367Y24.157
X14.3859Y24.2001
X14.4403Y24.2364
X14.4989Y24.2654
X14.5608Y24.2864
X14.625Y24.2991
X14.6903Y24.3034
X14.9403F 40
G00Z0.91
X14.9203Y23.3034
G01Z-0.09F 40
X14.6703F 40
X14.605Y23.3077F 80
X14.5408Y23.3205
X14.4789Y23.3415
X14.4203Y23.3704
X14.3659Y23.4067
X14.3167Y23.4499
X14.2736Y23.499
X14.2372Y23.5534
X14.2083Y23.6121
X14.1873Y23.674
X14.1745Y23.7382
X14.1703Y23.8034
Y24.9284
X14.1662Y25.0412
X14.1542Y25.1535
X14.1341Y25.2646
X14.1062Y25.374
X14.0705Y25.4811
X14.0273Y25.5854
X13.9768Y25.6864
X13.9192Y25.7834
X13.8548Y25.8762
X13.784Y25.9641
X13.707Y26.0467
X13.6244Y26.1236
X13.5365Y26.1945
X13.4438Y26.2589
X13.3467Y26.3165
X13.2457Y26.367
X13.1414Y26.4102
X13.0343Y26.4459
X12.9249Y26.4738
X12.8138Y26.4938
X12.7016Y26.5059
X12.5888Y26.5099
X10.5888
X10.5187Y26.5057
X10.4496Y26.493
X10.3826Y26.4721
X10.3185Y26.4433
X10.2584Y26.407
X10.2032Y26.3637
X10.1535Y26.314
X10.1102Y26.2588
X10.0739Y26.1987
X10.045Y26.1346
X10.0242Y26.0676
X10.0115Y25.9985
X10.0073Y25.9284
Y23.4284
X10.0114Y23.3342
X10.0237Y23.2406
X10.0441Y23.1485
X10.0725Y23.0585
X10.1086Y22.9714
X10.1522Y22.8877
X10.2028Y22.8081
X10.2603Y22.7333
X10.324Y22.6637
X10.3936Y22.5999
X10.4684Y22.5425
X10.548Y22.4918
X10.6317Y22.4483
X10.7189Y22.4121
X10.8088Y22.3838
X10.901Y22.3634
X10.9945Y22.351
X11.0888Y22.3469
X13.8388
X13.8906Y22.351
X13.9412Y22.3632
X13.9893Y22.3831
X14.0336Y22.4102
X14.0732Y22.444
X14.1069Y22.4836
X14.1341Y22.5279
X14.154Y22.576
X14.1662Y22.6266
X14.1703Y22.6784
Y23.8034
X14.1745Y23.8687
X14.1873Y23.9328
X14.2083Y23.9948
X14.2372Y24.0534
X14.2736Y24.1078
X14.3167Y24.157
X14.3659Y24.2001
X14.4203Y24.2364
X14.4789Y24.2654
X14.5408Y24.2864
X14.605Y24.2991
X14.6703Y24.3034
X14.9203F 40
G00Z1.0000
G29
G28
M05
M30

[jerry_stanek]

what program are you using to create your cut files. Try enlarging a corner section and see if it is segmented. I have that problem sometimes when I have a DXF file

[Gary Campbell]

Keith...
You seem to be missing the point. It appears to a number of us that your design program is either set to draw arcs as short segments, or does it by default. Selecting another postP from that program will NOT improve your cut quality, assuming the above is true.

To make sure of vector quality, especially in materials that show cut quality like clear plastics, export your 2d vectors into a CAD/CAM program such as PWks, VCPro or ArtCam and zoom in on the vectors.

If the corner arcs are made up from many short points, you have found your problem, as the vectors were created with segments instead of arcs.

If the corners show up with 3 points that define an arc, then toolpath using one of the "arc-inch" postP's in one of the above listed. They all have one that works good.

In the rare case that all methods above results in similar poor corner quality, your problem is mechanical. Your ramp settings will do little to change what you show in the pics.

[erik_f]

Why not call Mecsoft and ask them if what Gary is saying could be the problem. I generally draw all my 2d in Rhino with no problems. Granted I don't every cut plexi. I stopped using Visual Mill a while ago because Part Works was so much easier to use for 2d...and now I use Aspire for all my Cam work. I found I had to go in and change parts of Mecsofts post processor to get it to work right. I did find Mecsoft easy to work with and helpful when I called them. To me the software interface is good but Vectric is better at least than Visual Mill basic.

[garyb]

Just my observation from what I'm seeing
Your code is very vanilla and lacking, I would suggest you get a better pp or have this one adjusted to suit.

Your feed rate is too slow and your rpm too high for that single flute cutter.
your lead in speed is 40ipm and your feed rate is 80ipm not 100, when your machine ramps down into a corner you're now under 80ipm but your rpm is still up there causing the chatter looking cut. It may also be causing the piece to vibrate.

I've come across the M03 problem before, try the M07 in its place although its to turn the mist coolant on some have cross coded it.
Does the M05 turn your spindle off?

[Gary Campbell]

As I am not all that familiar with gcode.. I did a check. There are NO gcode arc calls in your file. Therefore either your design programs doesnt support arcs, or the feature is disabled. The other option is that you selected the wrong postP.

and I will never be wise enough to question Gary B ;)

[garyb]

and I will never be wise enough to question Gary B ;)yeah right, I would like to get you in the shop for a couple of days to pick your brain;)

Gary is correct there is no G2/G3 moves in the file, I just don't believe that's the problem, I ran the file here and it runs real smooth on my machine.

[jd9737]

Keith.

I was just curious. Does that bit you used require a single pass cut. I'm cutting polycarbonate for the first time and I need that type of edge.

Bill