Machine stops at end of tool path

[Cellar Dweller]

Hi All,

I have a 1995 Bridgeport with DX-32 controller. I had a post created for it to use in MC. (I will contact that gentlemen soon, nice guy from the forum here)

Anyway, my machine stops (shuts the drives, coolant, and spindle off) at the end of a tool path. If I skip the line it stalls on then it will run, but I have input an addtional S code for the spindle to turn on then it stalls again in the same place. The operation is a ramp contour with 4 passes. It stalls at the end of each contour. Here is the code.

Thanks,
CD

N10 G0G70G75G90
' PROGRAM FOR BRIDGPORT '
' SOURCE FILE = SR002 '
' CREATED ON 28-09-09 AT 19:09'
' 3/4 FLAT ENDMILL - TOOL1 - DIA .750 '
N20 M06 T1
N30 S2037 M03
N40 G0 X-1.025 Y.0549 (The start of a facing op, works fine.)
N50 G0 Z.25
N60 G0 Z.1
N70 G99 G1 X-1.025 Y.0549 Z.07 F6.4
N80 G99 X3.25 Y.0549 F18.3
N90 G99 G2 X3.5499 Y-.245 I3.25 J-.245
N100 G99 G2 X3.25 Y-.5449 I3.25 J-.245
N110 G99 G1 X-1.025 Y-.5449
N120 G0 Z.25
N130 G0 Y.0549
N140 G0 Z.07
N150 G99 G1 X-1.025 Y.0549 Z.04 F6.4
N160 G99 X3.25 Y.0549 F18.3
N170 G99 G2 X3.5499 Y-.245 I3.25 J-.245
N180 G99 G2 X3.25 Y-.5449 I3.25 J-.245
N190 G99 G1 X-1.025 Y-.5449
N200 G0 Z.25
N210 G0 Y.0549
N220 G0 Z.04
N230 G99 G1 X-1.025 Y.0549 Z.01 F6.4
N240 G99 X3.25 Y.0549 F18.3
N250 G99 G2 X3.5499 Y-.245 I3.25 J-.245
N260 G99 G2 X3.25 Y-.5449 I3.25 J-.245
N270 G99 G1 X-1.025 Y-.5449
N280 G0 Z.25
N290 G0 Y.0549
N300 G0 Z.01
N310 G99 G1 X-1.025 Y.0549 Z0. F6.4
N320 G99 X3.25 Y.0549 F18.3
N330 G99 G2 X3.5499 Y-.245 I3.25 J-.245
N340 G99 G2 X3.25 Y-.5449 I3.25 J-.245
N350 G99 G1 X-1.025 Y-.5449
N360 G0 Z.25 (the start of the ramp contour)
N370 G0 X4.244 Y.3105
N380 G0 Z.127
N390 G99 G1 X4.244 Y.3105 Z.027 F6.4
N400 G41 G48 X4.244 Y.3105 F18.3
N410 X4.244 Y.3105
N420 G99 X3.494 Y.3105
N430 G99 G3 X2.744 Y-.4395 I3.494 J-.4395
N440 G99 G1 X2.744 Y-.727 Z.0233
N450 G99 X1.4055 Y-.727 Z.0059
N460 G99 X1.218 Y-.727 Z.0035
N470 G99 X.2316 Y-.727 Z-.0093
N480 G99 X-.21 Y-.6491 Z-.0151
N490 G99 X-.21 Y.21 Z-.0263
N500 G99 X1.16 Y.21 Z-.044
N510 G99 X2.744 Y.21 Z-.0646
N520 G99 X2.744 Y-.362 Z-.072
N530 G99 X2.744 Y-.4395 Z-.073
N540 G99 X2.744 Y-.727 Z-.0767
N550 G99 X1.4055 Y-.727 Z-.0941
N560 G99 X1.218 Y-.727 Z-.0965
N570 G99 X.2316 Y-.727 Z-.1093
N580 G99 X-.21 Y-.6491 Z-.1151
N590 G99 X-.21 Y.21 Z-.1263
N600 G99 X1.16 Y.21 Z-.144
N610 G99 X2.744 Y.21 Z-.1646
N620 G99 X2.744 Y-.362 Z-.172
N630 G99 X2.744 Y-.4395 Z-.173
N640 G99 X2.744 Y-.727 Z-.1767
N650 G99 X1.4055 Y-.727 Z-.1941
N660 G99 X1.218 Y-.727 Z-.1965
N670 G99 X.2316 Y-.727 Z-.2093
N680 G99 X-.21 Y-.6491 Z-.2151
N690 G99 X-.21 Y.21 Z-.2263
N700 G99 X1.16 Y.21 Z-.244
N710 G99 X2.744 Y.21 Z-.2646
N720 G99 X2.744 Y-.362 Z-.272
N730 G99 X2.744 Y-.4395 Z-.273
N740 G99 X2.744 Y-.727 Z-.2767
N750 G99 X1.4055 Y-.727 Z-.2941
N760 G99 X1.218 Y-.727 Z-.2965
N770 G99 X.2316 Y-.727 Z-.3093
N780 G99 X-.21 Y-.6491 Z-.3151
N790 G99 X-.21 Y.21 Z-.3263
N800 G99 X1.16 Y.21 Z-.344
N810 G99 X2.744 Y.21 Z-.3646
N820 G99 X2.744 Y-.362 Z-.372
N830 G99 X2.744 Y-.4395 Z-.373
N840 G99 X2.744 Y-.727 Z-.3767
N850 G99 X1.4055 Y-.727 Z-.3941
N860 G99 X1.218 Y-.727 Z-.3965
N870 G99 X.2316 Y-.727 Z-.4093
N880 G99 X-.21 Y-.6491 Z-.4151
N890 G99 X-.21 Y.21 Z-.4263
N900 G99 X1.16 Y.21 Z-.444
N910 G99 X2.744 Y.21 Z-.4646
N920 G99 X2.744 Y-.362 Z-.472
N930 G99 X2.744 Y-.4395 Z-.473
N940 G99 X2.744 Y-.727 Z-.4767
N950 G99 X1.4055 Y-.727 Z-.4941
N960 G99 X1.218 Y-.727 Z-.4965
N970 G99 X.2316 Y-.727 Z-.5093
N980 G99 X-.21 Y-.6491 Z-.5151
N990 G99 X-.21 Y.21 Z-.5263
N1000 G99 X1.16 Y.21 Z-.544
N1010 G99 X2.744 Y.21 Z-.5646
N1020 G99 X2.744 Y-.362 Z-.572
N1030 G99 X2.744 Y-.4395 Z-.573
N1040 G99 X2.744 Y-.727 Z-.5767
N1050 G99 X1.4055 Y-.727 Z-.5941
N1060 G99 X1.218 Y-.727 Z-.5965
N1070 G99 X.2316 Y-.727 Z-.6093
N1080 G99 X-.21 Y-.6491 Z-.6151
N1090 G99 X-.21 Y.21 Z-.6263
N1100 G99 X1.16 Y.21 Z-.644
N1110 G99 X2.744 Y.21 Z-.6646
N1120 G99 X2.744 Y-.362 Z-.672
N1130 G99 X2.744 Y-.4395 Z-.673
N1140 G99 X2.744 Y-.727 Z-.6767
N1150 G99 X1.4055 Y-.727 Z-.6941
N1160 G99 X1.218 Y-.727 Z-.6965
N1170 G99 X.2316 Y-.727 Z-.7093
N1180 G99 X-.21 Y-.6491 Z-.7151
N1190 G99 X-.21 Y.21 Z-.7263
N1200 G99 X1.16 Y.21 Z-.744
N1210 G99 X2.744 Y.21 Z-.7646
N1220 G99 X2.744 Y-.362 Z-.772
N1230 G99 X2.744 Y-.4395 Z-.773
N1240 G99 X2.744 Y-.727 Z-.7767
N1250 G99 X1.4055 Y-.727 Z-.7941
N1260 G99 X1.218 Y-.727 Z-.7965
N1270 G99 X.2316 Y-.727 Z-.8093
N1280 G99 X-.21 Y-.6491 Z-.8151
N1290 G99 X-.21 Y.21 Z-.8263
N1300 G99 X1.16 Y.21 Z-.844
N1310 G99 X2.744 Y.21 Z-.8646
N1320 G99 X2.744 Y-.362 Z-.872
N1330 G99 X2.744 Y-.4395 Z-.873
N1340 G99 X2.744 Y-.727 Z-.8767
N1350 G99 X1.4055 Y-.727 Z-.8941
N1360 G99 X1.218 Y-.727 Z-.8965
N1370 G99 X1.1038 Y-.727 Z-.898
N1380 G99 X.2316 Y-.727
N1390 G99 X-.21 Y-.6491
N1400 G99 X-.21 Y.21
N1410 G99 X1.16 Y.21
N1420 G99 X2.744 Y.21
N1430 G99 X2.744 Y-.362
N1440 G99 X2.744 Y-.4395
N1450 G99 G3 X3.494 Y-1.1895 I3.494 J-.4395
N1460 G99 G1 X4.244 Y-1.1895
N1470 G99 X4.244 Y-1.1895 Z-.798 F6.4 (operation stops here, at least this is were the spindle is sitting)
N1480 G0 Z.25
N1490 G0 X4.194 Y.3105
N1500 G0 Z.127 (If I jump to this line and input a spindle command, it runs the next toolpath, then stalls again)
N1510 G99 G1 X4.194 Y.3105 Z.027
N1520 G41 G48 X4.194 Y.3105 F18.3

Thanks again,
CD

[psychomill]

Don't know much about this control but maybe it's confusing that last move since it really on needs to move in Z because the XY isn't different....

(your code)
N1460 G99 G1 X4.244 Y-1.1895
N1470 G99 X4.244 Y-1.1895 Z-.798 F6.4 (operation stops here, at least this is were the spindle is sitting)

Maybe try this?
N1460 G99 G1 X4.244 Y-1.1895
N1470 G99 Z-.798 F6.4 (remove XY positioning from the "stop" line)


.... or just simply dump this line and have it go to "G0Z.25" ??? (the next line)

[Superman]

Just a few queries

Your facing works fine
but
your 2D contours may be the problem
not sure on G99 or G48 functions, but you start cutter comp with G41, where is the G40 ( comp OFF ) before retracting, it is trying to go to the new XY descend point at rapid with comps ON, and then you restart G41 which is already ON

also
not sure if is a big issue, but the descend XY is the same as the take-up comp position

Are you using "Lead in / out" ?
If using "Wear" , then any values can be used ( say tangent, line=0.02, sweep 45°, arc=0.02" and copy to right side)
If using "Control" then the line and arc moves must be bigger than the tool radius ( just )( say tangent, line=60%, sweep 45°, arc=51% and copy to right side)

PS. to actually find the offending line, use single step, this stops the control from reading too far ahead
when using comps, the control does read ahead ( approx 4 lines- some controls read more ) so that internal adjustments to the toolpaths can be calculated before the tool arrives at the programmed endpoints

[psychomill]

Good catch Superman.... Didn't notice the comp at first....
Could be the machine not wanting to switch to rapid motion with comp on. Plus the comments on lead in/out...

Whatcha say CD?

[Cellar Dweller]

I say, I think I am going to wear my Superman under-roos to bed tonight. Well that all makes sense to me. I will give it a try in the am.

Not sure if this was a query Superman, but, yes the face operation works fine. And so does the ramp down. It cuts the part all the way down. But, when it is time to repeat the contour ramp to remove more material, it stalls.

I am pretty sure “wear” is being used. I almost always use it.

I am new to MC, my machine, and my PP. So the G41 looks like an issue? I will have to look at the controllers programming guide (1995 and a little short on details. LOL) and see what the controller expects to see after a G41. Of course I can edit to test, and then I assume try some different contour types, although I like ramp, and more importantly touch base with the guy that made the PP for me. All the code you are looking at is unedited MC output.

I know as time goes on, I will have to learn how to make changes to the PP as well.

Thanks A LOT guys,
CD

[Superman]

Comps are a major pain in the butt to diagnose problems
there are hidden and unexpected movements if comps are used and not configured correctly

To find the problems, set all tool radius comps to zero
--if you progam to the shape ( control ), then the toolpath ( in graphics dislpay on the machine ) should trace out the proper shape, and go thru the control without any comp errors,,,,,then if you put the proper comp in, it also should go thru without errors but graphics should show the toolpaths aroung your shape

--if you program to tool centre-line ( wear, reverse wear ), a lot of errors cease to exist. Machine graphics draws an offset toolpath around your shape, but then use a minus tool radius ( ie 1" tool put in -0.5000 ) should trace your desired shape ( except for corners and radii less than the tool radius )

A general wrap up,
to diagnose if it is a comp problem get rid of all G41 / G42, and run the program thru the machine graphics,
do the errors still exist ? No, then the problem was your comps

The problems can be numerous but the main ones are
- one big one is wrong size tool loaded onto the machine ( operator error )
- wrong tool radius set in machine ( operator error )
- arc endpoint errors ( machine parameter setting )
- not enough lead in / out for comp start / finish ( programmer error )
- comp starting / finishing on an arc ( some machines can ) ( programmer error )
- not cancelling comp and then moving to a new profile ( programmer and/or post error )