[Brian L]

I go to set up some parts this morning, machine hasn't run in a couple weeks, but this is a repeat job, have run it several times before with the same program. Tool #2 is a 1/2" end mill to profile the end of two square bars, it comes down, does my .02" lead in arc and then stops on the second arc saying "error 505: Radius too small to span given points".

I always dump my program after a run, right back into my shop computer and re-save right over the top of the old program, so I'm sure to have any modifications I might have made during the run. I've even double checked the program to the office computer, which is the one before I ran the parts, this portion of the program is the same (I have modified feed rates and some points in the "running version"). I wrote down all the points and did the math, all the numbers jive, the I's and J's make sense.... I can't figure out why the machine (Partner 4, Centurion 5, by the way) would have any problems with the program.

Any suggestions as to why the machine wouldn't like a program it has run before succesfully?

Segment of the program that does this end where it is faulting out, it continues down to the other end of the parts, but I can't get past the second arc in the first pass, line #1030 (I do the profile three times, once at Z-.375, once at Z-.75 and a final spring cut at Z-.76....

N0960 (1/2" end mill)
N0970 T2 M06 G43 H2
N0980 M07 (Mist coolant on)
N0990 S3000 M03
N1000 G00 X0.2200 Y-3.0050
Z.1
N1010 G01 Z-0.375 F30
N1020 G03 X0.2000 Y-2.9850 I-0.0200
N1030 G02 X-0.2500 Y-2.5350 J0.4500
N1040 G01 Y-1.9450
N1050 G02 X0.2000 Y-1.4950 I0.4500
N1060 G03 X0.2000 Y-1.2400 J0.1275
N1070 G02 X-0.2500 Y-0.7900 J0.4500
N1080 G01 Y-0.2000
N1090 G02 X0.2000 Y0.2500 I0.4500
N1100 G03 X0.2200 Y0.2700 J0.0200
N1110 G00 Z0.1000
N1120 Y-3.0050
N1130 Z-0.2750
N1140 G01 Z-0.750
N1150 G03 X0.2000 Y-2.9850 I-0.0200
N1160 G02 X-0.2500 Y-2.5350 J0.4500
N1170 G01 Y-1.9450
N1180 G02 X0.2000 Y-1.4950 I0.4500
N1190 G03 X0.2000 Y-1.2400 J0.1275
N1200 G02 X-0.2500 Y-0.7900 J0.4500
N1210 G01 Y-0.2000
N1220 G02 X0.2000 Y0.2500 I0.4500
N1230 G03 X0.2200 Y0.2700 J0.0200
N1240 G00 Z0.1000
N1250 Y-3.0050
N1260 Z-0.6500
N1270 G01 Z-0.760
N1280 G03 X0.2000 Y-2.9850 I-0.0200
N1290 G02 X-0.2500 Y-2.5350 J0.4500
N1300 G01 Y-1.9450
N1310 G02 X0.2000 Y-1.4950 I0.4500
N1320 G03 X0.2000 Y-1.2400 J0.1275
N1330 G02 X-0.2500 Y-0.790 J0.4500
N1340 G01 Y-0.2000
N1350 G02 X0.2000 Y0.2500 I0.4500
N1360 G03 X0.2200 Y0.2700 J0.0200
N1370 (Operation: Outside Offset, PHANTOM, T2: 1/2" end mill, 1.05 inch Deep)
N1380 G00 Z0.1000

[kdoney]

Have you changed you unit of measure on any subsequent jobs? This sounds like a modal problem. Make sure all of you persistent modes are correct.

[Brian L]

No, I always work in inches, my CAD system automatically converts any metric values I put in. I just ran another complicated profile job a week or so back and had no issues. I am a bit baffled. I remember that the machine has some "trig help", I looked for settings for tolerances and can't seem to locate anything.... only thing I found which might be along those lines is in the parameter settings there is CAD type DXF and then CAD Epsilon .0000, wondered if the CAD Epsilon has anything to do with it....

[maxumcaptain09]

Go to MDI and enter G90 and hit start. The control may be stuck in incremental. I noticed you do not use a modal safe start line.

[Brian L]

I do use G90 in a safe line, this is tool #2, I didn't bother to copy the lines from the beginning. I have been out playing in MDI and couldn't get it to do a 1/4 circle, I was at 0,0 typed in G02 X-.45 Y.45 J.45 and it has the 505 error. Now, I type in the same values, but instead of I or J, if I use R.45 it works fine. I don't usually use R instead of I/J, but I thought I would try it.

Now, what is curious, is I only changed the I/J values that were .450 to R, in the middle I have a half arc that uses a J.1275 and I left that alone and it works. So why the machine doesn't like I/J on the .45 radius I don't know, but I can go thru the program and modify all my I/J's to R values and get it to run. Still need/want to know what the heck is going on, I have a lot of existing programs that would have to be re-written.

[Brian L]

Turns out my program is 600+ lines long and has a ton of arc's in it.... so changing everything over is not going to be practical. If anybody has any ideas on what might have changed, please jump in here.

I think, but am not 100% positive, that I had changed back to an earlier version of the Centurion software since I ran this job last, I was and am still having some erratic speed issues. But that doesn't explain why a job I programmed a week or two back, with lots of arcs, ran just fine and this program won't.

I'm a bit stumped....

[allen mullis]

I have had the same problems on programs that have run literally hundreds of cycles without fault, the one day fire the machine up and it rejects the program for that exact fault under those exact same circumstances. I ended up changing the program, sorry to say. You might try re-loading the program. I have no explanation, just wanted to chime in and let you know that you aren't the only one. Also, so you know, in my situation, I have 5 machines with either Cent 5,6 & 7 controls that run the same programs and are dedicated to the same job. Just a Fluke I guess, but I never had the problems with the Cent 7 or updated SBC Cent 6 controls, only the Cent 5 which happens to be the oldest of them all.

Turns out my program is 600+ lines long and has a ton of arc's in it.... so changing everything over is not going to be practical. If anybody has any ideas on what might have changed, please jump in here.

I think, but am not 100% positive, that I had changed back to an earlier version of the Centurion software since I ran this job last, I was and am still having some erratic speed issues. But that doesn't explain why a job I programmed a week or two back, with lots of arcs, ran just fine and this program won't.

I'm a bit stumped....

[newman55598]

Turn your trig help off.

[Brian L]

Newman, OK, how do I turn off Trig help? I looked through parameters for a long time yesterday and didn't come across an obvious one to change.

Allen, thanks for the info that I'm not loosing my mind.... I was just completely baffled that a program I've run twice and 20+ cycles each time (I get two parts per cycle, usually make 44-48 pieces each run) would have run last year and not today.

Thanks for the help guys, oh, and I did completely clean out the machine of programs, re-loaded the one I needed, thinking that maybe something had gotten scrambled, but no luck there either. I found it really odd that hand typing a line of code in MDI wouldn't work if I used I/J but yet would if I used R.

[newman55598]

This is a quote from ZZZZ that did the trick for me

The PB### parameters are 'Bite' parms and they are kind of set-up parms for the control. PB81 is the "Special Flags" parameter. Look under the MISC parameters to find it.



Special Flags:

Go to Params - F1 Setup - F1 Level and type in:

Validation Code: PROTO3 enter
Access Level: 3 enter
(Several more buttons will light up)

Under F5 MISC , page down to the Special Flags Parameter

Enter a 1 to display dots
Enter a 2 to disable Trig Help
Enter a 3 to display dots and disable Trig Help
Enter a 4 to cancel cutter compensation
Enter a 5 to display dots and cancel cutter compensation
Enter a 6 to disable Trig Help and cancel cutter compensation
Enter a 7 to display dots, disable Trig Help, and cancel cutter compensation
Enter a 16 to display a circle the diameter of the cutter
Enter a 32 to display the 3-D ball cutter tip
(Not all options work on older software versions)


Bite Parameter 81 (PB81) is the parameter the control reads. To have a program change the status of the special flags parameter, insert a line of code setting the value to the number described above. Example - PB81=2 will disable Trig Help for CAD-CAM applications.

In newer controls, the Bite Parameter PB208 will need to be set first:


These can be added to your CAD/CAM post processor to make it more automatic:

At the beginning of the post add -

P99=PB208 (this saves the value of 208 in parameter 99)
PB208=0 (this sets 208 to 0)
PB81=6 (this sets 81 to disable Trig Help and cancel cutter compensation)


At the end of the post, add the following:

PB208=P99
PB81=0

This will set things back to normal for the Conversational Programming.

[newman55598]

If you just set the special flags use option 2. When using option 6 on my machine it will not dnc. It will do one line and stop when using option 6.

[Brian L]

OK, I set the special flags to 2 and it didn't make any difference. I did some more MDI playing around, sitting at 0,0 I type in G02 X-.5 Y.5 J.5 (a 90º arc from 6 o'clock to 9 o'clock) and it says Error 505. Try it with R and it works... then out of curiosity I go the next 1/4 circle, G02 X0 Y1 I.5 and the I value works, don't need to use R. Then I do the next 1/4 G02 X.5 Y.5 J-.5 and the J value fails, have to resort to R. Do the last quarter G02 X0 Y0 I-.5 and it works just fine again.

So.... it would appear that the control, for some reason, now has issue with the J values only....

Any other suggestions?

[newman55598]

Are you still running a sim disk maybe you can reset the SRAM and reload the parameters if you have them.

[Brian L]

No Sim disk, running off of a CF card. I played a lot more today.... loaded another old program for this same operation, was the first time I ran them and had made feed and speed changes. That program ran fine, along with several other recent programs. So, I opened up my CAM software, used the same job file I had from before, and re-posted the g-code for the machine. Will wonders ever cease? It runs just fine, all the I's and J's work now. So, a lot of messing about, but it's running, and I can't tell you why it didn't from the other program. Visually on paper and the computer screen the programs look the same, but some character I can't see must be off, that's all I can assume.

So, disaster averted, got the first two parts off the fixture, need to make a few small changes to center everything better on the material and I should be off to the races. Thanks for all the help and suggestions..... Oh... I didn't go back into mdi and play with circles, the programs working and I don't wanna know if the MDI will act weird again, I'm just going to pretend that never happened....

[newman55598]

Glad to hear.

Your mdi may have been acting weird because you didn't have the appropriate gcode before your arcs.


Sent from my iPhone using Tapatalk

[allen mullis]

I guess something did get scrambled in the program, maybe down to the binary level. If that was the case, it might look fine to you and me, but look like greek to the machine. It would be interesting to see if the saved corrupted program would run in either another machine or in a back plot program without fault or if it was just specific to that machine.

No Sim disk, running off of a CF card. I played a lot more today.... loaded another old program for this same operation, was the first time I ran them and had made feed and speed changes. That program ran fine, along with several other recent programs. So, I opened up my CAM software, used the same job file I had from before, and re-posted the g-code for the machine. Will wonders ever cease? It runs just fine, all the I's and J's work now. So, a lot of messing about, but it's running, and I can't tell you why it didn't from the other program. Visually on paper and the computer screen the programs look the same, but some character I can't see must be off, that's all I can assume.

So, disaster averted, got the first two parts off the fixture, need to make a few small changes to center everything better on the material and I should be off to the races. Thanks for all the help and suggestions..... Oh... I didn't go back into mdi and play with circles, the programs working and I don't wanna know if the MDI will act weird again, I'm just going to pretend that never happened....

[Brian L]

Sorry it took so long, been busy running thru a batch of parts. I had the same trouble with more old programs, and just went to set up another part.... same situation I get an error 505 and it's a part I have run several times before. This program is small and relatively simple, face a rectangular block, profile the perimeter, chamfer and center drill, and then drill some holes. I'll attach the tap file and cut and paste in case I can't attach a .tap (I changed it to a txt file as tap isn't a valid attachment here)

If somebody would like to load and at least screen verify on a machine, I would appreciate it.... this is becoming a royal pain in the ass...

N0010 (Filename: Rear block op10.tap)
N0020 (Post processor: Milltronics Rev C with Canned cycle.scpost)
N0030 (Date:31/10/2013 Time:21:02:11)
N0040 G20 (Units: Inches)
N0050 G40 G50 G70 G80 G90
N0060 (Part: Rear block op10)
N0070 (Operation: Face, T2: 1/2" end mill, 0 in Deep)
N0080 G49 Z0
N0090 G00 X-4 Y-4
N0100 (1/2" end mill)
N0110 T1 M06 G43 H1
N0120 M07 (Mist coolant on)
N0130 S4000 M03
N0140 G00 X-0.3000 Y-0.1500
N0150 Z0.1000
N0160 G01 Z0.000 F60
N0170 X3.3000
N0180 Y-0.5500
N0190 X-0.3000
N0200 Y-0.9500
N0210 X3.3000
N0220 Y-1.3500
N0230 X-0.3000
N0240 Y-1.7500
N0250 X3.3000
N0260 Y-2.1500
N0270 X-0.3000
N0280 (Operation: Outside Offset, VISIBLE, T2: 1/2" end mill, 0.5 in Deep)
N0290 G00 Z0.1000
N0300 X3.3240 Y-1.8760
N0310 G01 Z-0.50
N0320 G03 X3.2600 Y-1.9400 J-0.0640
N0330 G02 X2.9500 Y-2.2500 I-0.3100
N0340 G01 X0.0500
N0350 G02 X-0.2600 Y-1.9400 J0.3100
N0360 G01 Y-0.0500
N0370 G02 X0.0500 Y0.2600 I0.3100
N0380 G01 X2.9500
N0390 G02 X3.2600 Y-0.0500 J-0.3100
N0400 G01 Y-1.9400
N0410 G03 X3.3240 Y-2.0040 I0.0640
N0420 (Operation: Outside Offset, VISIBLE, T2: 1/2" end mill, 0.5 in Deep)
N0430 G00 Z0.1000
N0440 X3.3140 Y-1.8760
N0450 G01 Z-0.50 F60
N0460 G03 X3.2500 Y-1.9400 J-0.0640 F40.0
N0470 G02 X2.9500 Y-2.2400 I-0.3000
N0480 G01 X0.0500
N0490 G02 X-0.2500 Y-1.9400 J0.3000
N0500 G01 Y-0.0500
N0510 G02 X0.0500 Y0.2500 I0.3000
N0520 G01 X2.9500
N0530 G02 X3.2500 Y-0.0500 J-0.3000
N0540 G01 Y-1.9400
N0550 G03 X3.3140 Y-2.0040 I0.0640
N0560 (Operation: Drill, CENTER, T13: 90 degree csk, 0.15 in Deep)
N0570 G00 Z0.1000
N0580 M09 (Coolant off)
N0590 M05
N0600 G49 Z0
N0610 G00 X-4 Y-4
N0620 (90 degree csk)
N0630 T2 M06 G43 H2
N0640 M07 (Mist coolant on)
N0650 S3000 M03
N0660 G00 X2.5000 Y-1.7000
N0670 G99 G81 X2.5 Y-1.7 Z-0.150 R0.1000 F20.0
N0680 Y-0.3000
N0690 X0.5000
N0700 G98 Y-1.7000
N0710 G80(Operation: Outside Offset, VISIBLE, T13: 90 degree csk, 0.14 in Deep)
N0720 G00 X0.1140 Y-2.1790 Z0.1000
N0730 G01 Z-0.140 F40
N0740 G03 X0.0500 Y-2.1150 Z-0.1400 I-0.0640 J0.0000 F40.0
N0750 G02 X-0.1250 Y-1.9400 I0.0000 J0.1750
N0760 G01 Y-0.0500 Z-0.140 F40
N0770 G02 X0.0500 Y0.1250 Z-0.1400 I0.1750 J0.0000 F40.0
N0780 G01 X2.9500 Z-0.140 F40
N0790 G02 X3.1250 Y-0.0500 Z-0.1400 I0.0000 J-0.1750 F40.0
N0800 G01 Y-1.9400 Z-0.140 F40
N0810 G02 X2.9500 Y-2.1150 Z-0.1400 I-0.1750 J0.0000 F40.0
N0820 G01 X0.0500 Z-0.140 F40
N0830 G03 X-0.0140 Y-2.1790 Z-0.1400 I0.0000 J-0.0640 F40.0
N0840 (Operation: Drill, CENTER, T12: 1/4" Drill, 1.5 in Deep)
N0850 G00 Z0.1000
N0860 M09 (Coolant off)
N0870 M05
N0880 G49 Z0
N0890 G00 X-4 Y-4
N0900 (1/4" Drill)
N0910 T3 M06 G43 H3
N0920 M07 (Mist coolant on)
N0930 S3000 M03
N0940 G00 X2.5000 Y-1.7000
N0950 G99 G83 X2.5 Y-1.7 Z-1.500 R0.1000 Q0.2500 F15.0
N0960 Y-0.3000
N0970 X0.5000
N0980 G98 Y-1.7000
G80 G49 Z0 M05
N0990 G00 X14.0000 Y3.0000
N1000 M09 (Coolant off)
N1020 M30

[ZZZZ]

Brian, I think your programs ran fine when you used the 5.94 software so I think the problem only happens with your 129.09 software version.. I tested the program in several software versions to see when it fails. It fails in version129.23, but in version 129.28, it works fine. Milltronics must have made changes to the software between those two versions.

Would you remind me why you changed back to the 129.09? Maybe we can find a way to make it work.

[Brian L]

Hi ZZZZ,

I was beginning to suspect that could be the problem. I was having speed issues, command 3000 rpm and sometimes I get 4500, sometimes max speed (5000), sometimes 1500. We changed a couple chips on the control panel board with no effect, and then changed back to the 129.09 software to see if the speed would become more stable, which it hasn't. To solve, or deal with that issue, I installed a digital tach so I have an exact speed read out on the front of the machine. We can stop it if speed is critical (tapping) or just use the speed over ride if it's not too critical.

I would change back, but that's a bit beyond my skill level with the computer, and my friend Marty has been busy with moving and a home remodel, he's who has helped me before on the computer side of things.

The odd thing, is if I come back in the house, use my CAM system (Sheetcam) and re-code the program using the same job file as before, the program will run without any issues and the numbers (that I can see) look identical to the saved version I have in the shop computer. I had/have the habit of only having one program in the machine, run the job, any changes made got sent back to the shop computer and latest version gets saved over the old one. The past couple days, I have left the program up on the shop computer and any changes needed, I just do it there, send it back to the machine, and never send back from the machine to the computer. So we'll see if that stops the problem until I have time to change the machine back to the newer OS.

[JohnHennessy]

how long has it been sense you shut the machine completely down? I had a Fryer with an Anilam 4000m and would get errors like that and after a fresh reboot they were not an issue... We had dirty power to that shop, lot of noise in it