Hello Guest it is April 21, 2019, 08:43:19 PM

Author Topic: Help with G-Code error  (Read 9474 times)

0 Members and 1 Guest are viewing this topic.

Offline TT350

*
  •  113 113
    • View Profile
Help with G-Code error
« on: November 03, 2007, 10:49:53 PM »
Can some one look at this code and tell me
way I’m getting an error please’

The error reads
K word given for arc in XY planeline 10

Here is the code.



G00 G43 G40.1 G17 G80 G50 G90
G20
(Hole Pocketing)
M6 T1
G43 H1
M03 S1750
G00 Z0.1875
X0.0333 Y1.2287
G01 Z0.0250  F5.0
G17
G03X0.0443Y1.2598Z-0.0857I-0.0388J0.0311K0.1000
X0.0432Y1.2701I-0.0498J0.0000Q0.0937
X-0.0541Y1.2495I-0.0487J-0.0103
X0.0432Y1.2701I0.0486J0.0103
G01 X0.0256 Y1.2986
G03X0.0443Y1.2598Z-0.1714I-0.0311J-0.0388K0.1000
X0.0432Y1.2701I-0.0498J0.0000Q0.0937
X-0.0541Y1.2495I-0.0487J-0.0103
X0.0432Y1.2701I0.0486J0.0103
G01 X0.0256 Y1.2986
G03X0.0443Y1.2598Z-0.2571I-0.0311J-0.0388K0.1000
X0.0432Y1.2701I-0.0498J0.0000Q0.0937
X-0.0541Y1.2495I-0.0487J-0.0103
X0.0432Y1.2701I0.0486J0.0103
G01 X0.0256 Y1.2986
G03X0.0443Y1.2598Z-0.3429I-0.0311J-0.0388K0.1000
X0.0432Y1.2701I-0.0498J0.0000Q0.0937
X-0.0541Y1.2495I-0.0487J-0.0103
X0.0432Y1.2701I0.0486J0.0103
G01 X0.0256 Y1.2986
G03X0.0443Y1.2598Z-0.4286I-0.0311J-0.0388K0.1000
X0.0432Y1.2701I-0.0498J0.0000Q0.0937
X-0.0541Y1.2495I-0.0487J-0.0103
X0.0432Y1.2701I0.0486J0.0103
G01 X0.0256 Y1.2986
G03X0.0443Y1.2598Z-0.5143I-0.0311J-0.0388K0.1000
X0.0432Y1.2701I-0.0498J0.0000Q0.0937
X-0.0541Y1.2495I-0.0487J-0.0103
X0.0432Y1.2701I0.0486J0.0103
G01 X0.0256 Y1.2986
G03X0.0443Y1.2598Z-0.6000I-0.0311J-0.0388K0.1000
X0.0432Y1.2701I-0.0498J0.0000Q0.0937
X-0.0541Y1.2495I-0.0487J-0.0103
X0.0432Y1.2701I0.0486J0.0103
G01 X-0.0055 Y1.2598
G00 Z0.1875
X1.2986 Y-0.0257
G01 Z0.0250  F5.0
G03X1.3095Y0.0055Z-0.0857I-0.0388J0.0312K0.1000
X1.3085Y0.0158I-0.0497J0.0000Q0.0937
X1.2111Y-0.0049I-0.0487J-0.0103
X1.3085Y0.0158I0.0487J0.0104
G01 X1.2909 Y0.0443
G03X1.3095Y0.0055Z-0.1714I-0.0311J-0.0388K0.1000
X1.3085Y0.0158I-0.0497J0.0000Q0.0937
X1.2111Y-0.0049I-0.0487J-0.0103
X1.3085Y0.0158I0.0487J0.0104
G01 X1.2909 Y0.0443
G03X1.3095Y0.0055Z-0.2571I-0.0311J-0.0388K0.1000
X1.3085Y0.0158I-0.0497J0.0000Q0.0937
X1.2111Y-0.0049I-0.0487J-0.0103
X1.3085Y0.0158I0.0487J0.0104
G01 X1.2909 Y0.0443
G03X1.3095Y0.0055Z-0.3429I-0.0311J-0.0388K0.1000
X1.3085Y0.0158I-0.0497J0.0000Q0.0937
X1.2111Y-0.0049I-0.0487J-0.0103
X1.3085Y0.0158I0.0487J0.0104
G01 X1.2909 Y0.0443
G03X1.3095Y0.0055Z-0.4286I-0.0311J-0.0388K0.1000
X1.3085Y0.0158I-0.0497J0.0000Q0.0937
X1.2111Y-0.0049I-0.0487J-0.0103
X1.3085Y0.0158I0.0487J0.0104
G01 X1.2909 Y0.0443
G03X1.3095Y0.0055Z-0.5143I-0.0311J-0.0388K0.1000
X1.3085Y0.0158I-0.0497J0.0000Q0.0937
X1.2111Y-0.0049I-0.0487J-0.0103
X1.3085Y0.0158I0.0487J0.0104
G01 X1.2909 Y0.0443
G03X1.3095Y0.0055Z-0.6000I-0.0311J-0.0388K0.1000
X1.3085Y0.0158I-0.0497J0.0000Q0.0937
X1.2111Y-0.0049I-0.0487J-0.0103
X1.3085Y0.0158I0.0487J0.0104
G01 X1.2598 Y0.0055
G00 Z0.1875
X0.0442 Y-1.2909
G01 Z0.0250  F5.0
G03X0.0552Y-1.2598Z-0.0857I-0.0387J0.0311K0.1000
X0.0541Y-1.2495I-0.0497J0.0000Q0.0937
X-0.0432Y-1.2701I-0.0486J-0.0103
X0.0541Y-1.2495I0.0487J0.0103
G01 X0.0366 Y-1.2210
G03X0.0552Y-1.2598Z-0.1714I-0.0311J-0.0388K0.1000
X0.0541Y-1.2495I-0.0497J0.0000Q0.0937
X-0.0432Y-1.2701I-0.0486J-0.0103
X0.0541Y-1.2495I0.0487J0.0103
G01 X0.0366 Y-1.2210
G03X0.0552Y-1.2598Z-0.2571I-0.0311J-0.0388K0.1000
X0.0541Y-1.2495I-0.0497J0.0000Q0.0937
X-0.0432Y-1.2701I-0.0486J-0.0103
X0.0541Y-1.2495I0.0487J0.0103
G01 X0.0366 Y-1.2210
G03X0.0552Y-1.2598Z-0.3429I-0.0311J-0.0388K0.1000
X0.0541Y-1.2495I-0.0497J0.0000Q0.0937
X-0.0432Y-1.2701I-0.0486J-0.0103
X0.0541Y-1.2495I0.0487J0.0103
G01 X0.0366 Y-1.2210
G03X0.0552Y-1.2598Z-0.4286I-0.0311J-0.0388K0.1000
X0.0541Y-1.2495I-0.0497J0.0000Q0.0937
X-0.0432Y-1.2701I-0.0486J-0.0103
X0.0541Y-1.2495I0.0487J0.0103
G01 X0.0366 Y-1.2210
G03X0.0552Y-1.2598Z-0.5143I-0.0311J-0.0388K0.1000
X0.0541Y-1.2495I-0.0497J0.0000Q0.0937
X-0.0432Y-1.2701I-0.0486J-0.0103
X0.0541Y-1.2495I0.0487J0.0103
G01 X0.0366 Y-1.2210
G03X0.0552Y-1.2598Z-0.6000I-0.0311J-0.0388K0.1000
X0.0541Y-1.2495I-0.0497J0.0000Q0.0937
X-0.0432Y-1.2701I-0.0486J-0.0103
X0.0541Y-1.2495I0.0487J0.0103
G01 X0.0055 Y-1.2598
G00 Z0.1875
X-1.2210 Y-0.0366
G01 Z0.0250  F5.0
G03X-1.2101Y-0.0055Z-0.0857I-0.0388J0.0311K0.1000
X-1.2111Y0.0049I-0.0497J0.0000Q0.0937
X-1.3085Y-0.0158I-0.0487J-0.0104
X-1.2111Y0.0049I0.0487J0.0103
G01 X-1.2287 Y0.0334
G03X-1.2101Y-0.0055Z-0.1714I-0.0311J-0.0389K0.1000
X-1.2111Y0.0049I-0.0497J0.0000Q0.0937
X-1.3085Y-0.0158I-0.0487J-0.0104
X-1.2111Y0.0049I0.0487J0.0103
G01 X-1.2287 Y0.0334
G03X-1.2101Y-0.0055Z-0.2571I-0.0311J-0.0389K0.1000
X-1.2111Y0.0049I-0.0497J0.0000Q0.0937
X-1.3085Y-0.0158I-0.0487J-0.0104
X-1.2111Y0.0049I0.0487J0.0103
G01 X-1.2287 Y0.0334
G03X-1.2101Y-0.0055Z-0.3429I-0.0311J-0.0389K0.1000
X-1.2111Y0.0049I-0.0497J0.0000Q0.0937
X-1.3085Y-0.0158I-0.0487J-0.0104
X-1.2111Y0.0049I0.0487J0.0103
G01 X-1.2287 Y0.0334
G03X-1.2101Y-0.0055Z-0.4286I-0.0311J-0.0389K0.1000
X-1.2111Y0.0049I-0.0497J0.0000Q0.0937
X-1.3085Y-0.0158I-0.0487J-0.0104
X-1.2111Y0.0049I0.0487J0.0103
G01 X-1.2287 Y0.0334
G03X-1.2101Y-0.0055Z-0.5143I-0.0311J-0.0389K0.1000
X-1.2111Y0.0049I-0.0497J0.0000Q0.0937
X-1.3085Y-0.0158I-0.0487J-0.0104
X-1.2111Y0.0049I0.0487J0.0103
G01 X-1.2287 Y0.0334
G03X-1.2101Y-0.0055Z-0.6000I-0.0311J-0.0389K0.1000
X-1.2111Y0.0049I-0.0497J0.0000Q0.0937
X-1.3085Y-0.0158I-0.0487J-0.0104
X-1.2111Y0.0049I0.0487J0.0103
G01 X-1.2598 Y-0.0055
G00 Z0.1875
G00 Z1
M5 M9
M30

vmax549

*
Re: Help with G-Code error
« Reply #1 on: November 04, 2007, 12:07:43 AM »
Its a guess ( I am not in the shop near the MANUAL) but I dont think you use the k word in an xy plane. Did you hand code it or use a CAM program??

(;-)

Offline TT350

*
  •  113 113
    • View Profile
Re: Help with G-Code error
« Reply #2 on: November 04, 2007, 01:33:51 AM »
Visualmill 5.0 cam.

vmax549

*
Re: Help with G-Code error
« Reply #3 on: November 04, 2007, 08:02:45 AM »
If you can post the dimensions of the hole I'll do one in lcam to compare. It looks like the CAM is adding in K &Q words. As a test I would edit out the K words first then see if Mach likes the Q word, if not edit them out also to see if the remaining code runs ok.

You might have to find a different post proc for the CAM package.

(;-) TP

Offline Graham Waterworth

*
  • *
  •  1,851 1,851
  • West Yorkshire, England
    • View Profile
Re: Help with G-Code error
« Reply #4 on: November 04, 2007, 09:30:06 AM »
The problem is that you are using a spiral/helical pocketing routine in visual mill, use a normal area clearing routine and all will be well.

Mach3 dose not support spiral/helical milling in the same way

Graham.
America gave us powered flight, England the steam train and Germany the car.  Who invented the first boat?

Offline TT350

*
  •  113 113
    • View Profile
Re: Help with G-Code error
« Reply #5 on: November 04, 2007, 10:05:33 AM »
Ok let me start from the beginning and this will make sense.

The other day I need a .500 thick bushing to press in
a pulley that I need to press on a shaft.

The OD was 1.5 and the ID was .625 and I need a .0005
press on the OD and ID, so I drew it up in Autodesk Inventor and generated a tool path with Visualmill and
cut the part using a .375 end mill using hole pocketing
for the ID and 2 ½ profiling for the OD.

After the bushing was cut the ID was smooth and round and dead on the # the OD had a lot of little flats around it.

I called Visualmill and ask them why the OD of my part had all the little flat segments,
they said that I could go in to machining preferences and change the settings and it would cut and arc without the segments.

So I go in and make the changes and yesterday I need to cut another part but I haven’t used VM since I made the changes.

The code that I posted if for 4 hole .4745 ID x .600 deep using hole pocketing with a .375 endmill.

Here’s a screen shot of the setting for the code posted.   
        



  

« Last Edit: November 04, 2007, 10:16:15 AM by TT350 »

Offline TT350

*
  •  113 113
    • View Profile
Re: Help with G-Code error
« Reply #6 on: November 04, 2007, 10:17:41 AM »
After getting the error I go back the machining preferences and make changes until Mach will take the code.
Here are the changes.


Here is the code that I ended up useing for the job.

I cut this code very short so I could post it.

G00 G43 G40.1 G17 G80 G50 G90
G20
(Hole Pocketing)
M6 T1
G43 H1
M03 S1750
G00 Z0.1875
X0.0333 Y1.2287
G01 Z0.0250  F5.0
X0.0357 Y1.2318 Z0.0238
X0.0382 Y1.2360 Z0.0222
X0.0404 Y1.2405 Z0.0206
X0.0421 Y1.2451 Z0.0190
X0.0433 Y1.2499 Z0.0174
X0.0440 Y1.2548 Z0.0158
X0.0443 Y1.2598 Z0.0142
X0.0440 Y1.2648 Z0.0127
X0.0433 Y1.2697 Z0.0111
X0.0421 Y1.2745 Z0.0095
X0.0404 Y1.2791 Z0.0079
X0.0382 Y1.2836 Z0.0063
X0.0357 Y1.2878 Z0.0047
X0.0327 Y1.2918 Z0.0031
X0.0293 Y1.2954 Z0.0016
X0.0256 Y1.2987 Z0.0000
X0.0215 Y1.3016 Z-0.0016
X0.0172 Y1.3041 Z-0.0032
X0.0127 Y1.3061 Z-0.0048
X0.0080 Y1.3077 Z-0.0064
X0.0032 Y1.3088 Z-0.0080
X-0.0017 Y1.3094 Z-0.0096
X-0.0067 Y1.3095 Z-0.0111
X-0.0116 Y1.3092 Z-0.0127
X-0.0165 Y1.3083 Z-0.0143
X-0.0213 Y1.3070 Z-0.0159
X-0.0259 Y1.3051 Z-0.0175
X-0.0303 Y1.3029 Z-0.0191
X-0.0345 Y1.3002 Z-0.0207
X-0.0384 Y1.2971 Z-0.0222
X-0.0419 Y1.2936 Z-0.0238
X-0.0451 Y1.2898 Z-0.0254
X-0.0479 Y1.2857 Z-0.0270
X-0.0503 Y1.2814 Z-0.0286
X-0.0522 Y1.2768 Z-0.0302
X-0.0537 Y1.2721 Z-0.0318
X-0.0546 Y1.2672 Z-0.0334
X-0.0551 Y1.2623 Z-0.0349
Y1.2573 Z-0.0365
X-0.0546 Y1.2524 Z-0.0381
X-0.0537 Y1.2475 Z-0.0397
X-0.0522 Y1.2428 Z-0.0413
X-0.0503 Y1.2382 Z-0.0429
X-0.0479 Y1.2339 Z-0.0445
X-0.0451 Y1.2298 Z-0.0460
X-0.0419 Y1.2260 Z-0.0476
X-0.0384 Y1.2225 Z-0.0492
X-0.0345 Y1.2194 Z-0.0508
X-0.0303 Y1.2167 Z-0.0524
X-0.0259 Y1.2145 Z-0.0540
X-0.0213 Y1.2126 Z-0.0556
X-0.0165 Y1.2113 Z-0.0572
X-0.0116 Y1.2104 Z-0.0587
X-0.0067 Y1.2101 Z-0.0603
X-0.0017 Y1.2102 Z-0.0619
X0.0032 Y1.2108 Z-0.0635
X0.0080 Y1.2119 Z-0.0651
X0.0127 Y1.2135 Z-0.0667
X0.0172 Y1.2155 Z-0.0683
X0.0215 Y1.2180 Z-0.0698
X0.0256 Y1.2209 Z-0.0714
X0.0293 Y1.2242 Z-0.0730
X0.0327 Y1.2278 Z-0.0746
X0.0357 Y1.2318 Z-0.0762
X0.0382 Y1.2360 Z-0.0778
X0.0404 Y1.2405 Z-0.0794
X0.0421 Y1.2451 Z-0.0810
X0.0433 Y1.2499 Z-0.0825
X0.0440 Y1.2548 Z-0.0841
X0.0443 Y1.2598 Z-0.0857
G17
G03X0.0432Y1.2701I-0.0498J0.0000Q0.0937
X-0.0541Y1.2495I-0.0487J-0.0103
X0.0432Y1.2701I0.0486J0.0103
G01 X0.0256 Y1.2986
Y1.2987 Z-0.0858
« Last Edit: November 04, 2007, 10:23:53 AM by TT350 »

Offline TT350

*
  •  113 113
    • View Profile
Re: Help with G-Code error
« Reply #7 on: November 04, 2007, 10:28:53 AM »
The problem is that you are using a spiral/helical pocketing routine in visual mill, use a normal area clearing routine and all will be well.

Mach3 dose not support spiral/helical milling in the same way

Graham.


You are saying in the "same way" did you mean at the same time?

Chris

Offline Graham Waterworth

*
  • *
  •  1,851 1,851
  • West Yorkshire, England
    • View Profile
Re: Help with G-Code error
« Reply #8 on: November 04, 2007, 10:33:57 AM »
No, Mach can do helix and spirals but only in long hand code, similar to the code you just posted that worked.

Graham.
America gave us powered flight, England the steam train and Germany the car.  Who invented the first boat?

Offline TT350

*
  •  113 113
    • View Profile
Re: Help with G-Code error
« Reply #9 on: November 04, 2007, 10:38:03 AM »
I pulled my hair out for a week trying to get the tool offsets to work in Mach and with the help Bryan and
Uday at VM we found a bug in the tool change micro
and fix that and the tool off sets work perfect now.

I all so found a bug in the drill cycles as well and we fixed that to.

I was thinking that this may be another bug.

Bug may be the wrong word to use. it was just a little
code change in the micro.