THat might NOT be the best thing to do. all small line segments can cause a degrading of performance in some situations. Using the mini lines you may need to bump your look ahead setting to 200 or more.



You need to test each combination on YOUR machine.

Yes, just found that out by running the code so I went back and changed the smoothing to 'Line Arc' and now I keep getting an error message in Mach saying 'Radius to end of arc differs from radius to startLine 18' and Mach won't continue to load so I don't know if other arc lines have the same problem or what the cause is - I need help again.

I have copied some code below:

%(TAILPLANE FINISH)
G90 G40 G49 G64
 (DEFINE OPERATION : FLATLAND OPERATION)
T02 M06(8mm End Mill)
G0Z15
G0X-2.807Y164.564
Z5.0
G1Z0.0F1000.0
G17G3X-2.23Z0.0Y164.625I-2.655J165.879F2500.0
X-1.594Z0.0Y164.957I-3.47J167.772
G2X1.47Y166.899Z0.0I47.596J90.722
X2.667Y167.2Z0.0I2.667J164.671
G1X5.907Y167.196
G2X5.965Y166.833Z0.0I5.864J167.003
G3X-1.685Z0.0Y162.027I96.14J14.82
X-2.197Z0.0Y160.975I-0.87J160.98
G1X-2.193Y159.457
G3X-1.603Z0.0Y159.202I-1.817J159.516
G2X10.895Y166.917Z0.0I102.294J4.876
X12.102Y167.2Z0.0I12.102J164.485
G1X15.687Y167.196
G2X15.732Y166.86Z0.0I15.647J167.019
G3X-1.604Z0.0Y156.292I104.368J1.96
X-2.197Z0.0Y155.164I-0.83J155.164
G1X-2.193Y153.623
G3X-1.609Z0.0Y153.375I-1.824J153.68
G2X21.069Y166.941Z0.0I105.99J-0.758
X22.289Y167.2Z0.0I22.289J164.2
G1X26.299Y167.195

Line 18 is the red one.

Thanks,

Mike

You need to swap the ij mode in mach3 config

Graham

Thanks, Graham but I figured that might be the problem and did the swap but now get the same message on a different line - this is not going well

Mike

CLose down mach and restart again. Then double check your IJ settings. 

It seems that the code wants abs IJ. I would double check your CAM settings.

(;-) TP

I have tried closing Mach, re-opening it, checked the IJ setting and tried it in both modes but I am still getting the 'Radius to end of arc differs from radius to startLine 2081' error but now, in incremental IJ mode, I get the error on line 2081 so it is getting to that line OK, through all the other arcs without a problem. I have copied some more code below, this time from line 2033 - 2085 and again, the red line is the problem.

X91.082Y33.471
G3X135.247Y30.092Z-3.0I184.426J2120.356
X165.909Y28.268Z-3.0I165.381J2521.227
X222.965Y25.87Z-3.0I148.246J2846.988
G1X243.522Y25.261
X262.168Y24.798
G3X343.52Y23.48Z-3.0I154.263J7008.442
X390.709Y23.065Z-3.0I196.538J9999.9999
G1X390.695Y21.065
G2X326.234Y21.684Z-3.0I93.057J9999.9999
X271.483Y22.594Z-3.0I99.173J7608.821
X200.837Y24.657Z-3.0I82.44J4033.896
X160.036Y26.589Z-3.0I95.551J2450.467
G0Z9.231
 (DEFINE OPERATION : PROFILING OPERATION)
X394.722Y25.138
Z4.75
G1Z-0.25F1000.0
X393.391Y55.608F2500.0
X395.401Y55.434
X396.72Y25.225
G2X392.695Y21.05Z-0.25I-3.996J-0.175
G0Z9.231
X393.262Y58.566
Z4.75
G1Z-0.25F1000.0
X392.837Y68.311F2500.0
X394.845Y68.171
X395.272Y58.392
G0Z9.231
X392.707Y71.272
Z4.75
G1Z-0.25F1000.0
X391.353Y102.297F2500.0
X393.361Y102.157
X394.715Y71.131
G0Z9.231
X391.136Y107.271
Z4.75
G1Z-0.25F1000.0
X389.912Y135.301F2500.0
X391.92Y135.16
X393.144Y107.131
G0Z9.231
 (DEFINE OPERATION : PARALLEL LACE OPERATION)
Z15.0
X388.331Y126.091
Z8.873
G1Z3.873F1000.0
G19G3X388.331Y110.905Z4.25J-15.698F2500.0
G1X388.323Y110.669
X388.302Y110.426
X388.268Y110.182

From the earlier lines you can see that the arcs are all there and Mach is accepting them with no problem. The problem line is the first arc in the YZ plane hence the G19.

This is becoming very frustrating,

Mike

Mach3 will not do 3D arcs, turn off helical/spirals in the post processor and try again.

Graham

Graham,

Now I am really confused - for the past two years I have been drilling holes with Mach using helical arcs, produced with EdgeCam. I tried turning helical arcs off in EdgeCam and I still get the same error reported but on a different line. The code below is a drilling cycle using what I thought were helical arcs. If they aren't, please tell me what they are and I can re-set my brain

Thanks,

Mike

%(TAILPLANE HOLD DOWN)
G90 G40 G49 G64
 (DEFINE OPERATION : PROFILING OPERATION)
T01 M06(5mm End Mill)
G1X65.0  Y10.75
Z0.0  F100.0
G17G3X65.0  Z-1.0  Y10.75 I0.0  J-3.25 F500.0
X65.0  Z-2.0  Y10.75 I0.0  J-3.25
X65.0  Z-3.0  Y10.75 I0.0  J-3.25
X65.0  Z-4.0  Y10.75 I0.0  J-3.25
X65.0  Z-5.0  Y10.75 I0.0  J-3.25
X65.0  Z-6.0  Y10.75 I0.0  J-3.25
X65.0  Z-7.0  Y10.75 I0.0  J-3.25
X65.0  Z-8.0  Y10.75 I0.0  J-3.25
X65.0  Z-9.0  Y10.75 I0.0  J-3.25
X65.0  Z-10.0  Y10.75 I0.0  J-3.25
X65.0  Z-11.0  Y10.75 I0.0  J-3.25
X65.0  Z-12.0  Y10.75 I0.0  J-3.25
X65.0  Z-12.0  Y10.75 I0.0  J-3.25
G1Z5.0 

G19G3X388.331Y110.905Z4.25J-15.698F2500.0

You seem to be missing the K from the line.

Graham

After Graham's post about the missing K value, I took a cautious look at the code wizard in EdgeCam by loading the post processor I was sent from New Zealand. Although I did not really know what I was doing, I did manage to find where the error was and it was indeed a missing K token in the pp. Once I had rectified that and proved the code was good, I got adventurous and made a few more changes to suit my machine.

I have to report that all seems to work very well and it is thanks to the help from this forum that I had the confidence to delve into the unknown - thanks.

One slight problem still occurs and that is, when I use the -1 scale on the X axis to do a mirror image, I get the arcs going the wrong way and the toolpath window looks a mess. However, if I mirror in Y, everything is just fine. I figure this is because the arcs are in the YZ plane so if the scaling is in X, the start and finish of the arc is reversed, hence the mess in the toolpath window. By scaling in Y, there is no effect on the X coordinates.

I have learned a great deal over the last couple of days.

Cheers,

Mike