Error in my G code, post processor, controller settings, etc. Help!
I get error code: 9 N 0 SYNTAX ERROR
I have done some research but it's inconclusive. One thing I read was I could have it in ASCII mode rather than ISO mode or something, but I cannot find out how to change that.
I am using the generic post for fanuc from autodesk in inventor CAM thing.
My code looks like:
It shows up on the controller a little differently, as in this picture:Code:: (PGM, NAME="4") ; T5 D=4 CR=0 - ZMIN=-1 - FLAT END MILL : G90 G40 G94 G17 G71 M26 ; FACE3 :T5 M6 S1511 M3 H0 M8 G0 X-8.4 Y-50.132 Z15 Z5 G1 Z-0.6 F500 G18 G3 X-8.8 Z-1 I-8.8 K-0.6 G1 X-11 X-61.8 F1000 G17 G2 Y-46.501 I-61.8 J-48.317 G1 X-11 G3 Y-42.871 I-11 J-44.686 G1 X-61.8 G2 Y-39.241 I-61.8 J-41.056 G1 X-11 G3 Y-35.611 I-11 J-37.426 G1 X-61.8 G2 Y-31.98 I-61.8 J-33.795 G1 X-11 G3 Y-28.35 I-11 J-30.165 G1 X-61.8 G2 Y-24.72 I-61.8 J-26.535 G1 X-11 G3 Y-21.089 I-11 J-22.905 G1 X-61.8 G2 Y-17.459 I-61.8 J-19.274 G1 X-11 G3 Y-13.829 I-11 J-15.644 G1 X-61.8 G2 Y-10.199 I-61.8 J-12.014 G1 X-11 G3 Y-6.568 I-11 J-8.383 G1 X-61.8 G2 Y-2.938 I-61.8 J-4.753 G1 X-11 G18 G2 X-10.6 Z-0.6 I-11 K-0.6 G0 Z15 G17 M9 M26 G0 X0 Y0 M30 M2
Attachment 487805
The post processor I used is as follows:
Attachment 487807
I cannot find the exact post processor used on my desktop, if anybody knows the location for inventor let me know!
Any tips?
it makes me think there might be an EOL issue, like does one flavor of g-code use a different end of line (is this the correct terminology?) character than others?
Re: Error in my G code, post processor, controller settings, etc. Help!
SYNTAX is what is written (or the way it is written)in your code is NOT expected in the control...
-Usually a program starts with an Oxxxx
-mix of : & ; at beginnings of lines. Usually ; symbolises EOL
-control may not like quotes "". I would delete these 1st
Re: Error in my G code, post processor, controller settings, etc. Help!
Yes, there is no way that is going to run like that, words like (Faces3) and (Flat End Mill) and all things that are not related to the program will have to be in Parentheses (--) or just remove all the junk not related to the program and try it againOriginally Posted by michaelwoodcock
Is it by design that you are using a different work plane G18 and G17
Mactec54
I agree, the program has syntax errors because of the reasons you mentioned. The control cannot execute blocks it doesn't recognise.
Parentheses (or brackets) would help run the program.
Re: Error in my G code, post processor, controller settings, etc. Help!
Thanks guys! Mactec, I am not sure on the different work planes g18 & 17, I didn't intend for the code to come out this way, I just took it exactly as output from inventor - it seems I may have to hunt for a post that doesn't do this, or make one myself.
Years ago, when I had done my own linuxCNC conversion, I imported the code directly from inventor and never had to alter anything. I hope I can find a post, or make my own to get there with the fanuc21 controls
Re: Error in my G code, post processor, controller settings, etc. Help!
Any Fanuc Post should work, there are quite a lot wrong with that format for it to work on a Fanuc controlThanks guys! Mactec, I am not sure on the different work planes g18 & 17, I didn't intend for the code to come out this way, I just took it exactly as output from inventor - it seems I may have to hunt for a post that doesn't do this, or make one myself.
Years ago, when I had done my own linuxCNC conversion, I imported the code directly from inventor and never had to alter anything. I hope I can find a post, or make my own to get there with the fanuc21 controls
The G17 / G18 has come from how the cam software has been processed when you are doing your Tool Path, so that part needs to be looked at, the Postprocessor will output a Program to how the Tool Path has been created
Programming
G17 XY-Plane
Programming
G18 ZX-Plane
Programming
G19 YZ-Plane
Mactec54
Re: Error in my G code, post processor, controller settings, etc. Help!
The G17/G18 is NOT the issue creating the SYNTAX error. That is caused by a programming choice (views) when creating the toolpath.
The post proc. you are using is not compatible with your control, it nearly seems a heidenhain output as the semi-colon ; is used as a comment (on a fanuc it is an EOL marker)
I don't know the purpose of the colon : ... did you type any of the code ?
The colon : does not belong in fanuc code.
A good sign if a character is not usable is to not use any character that is not on the control keypad.
PS.. M30 and M2 do the same thing, only one is required
Re: Error in my G code, post processor, controller settings, etc. Help!
No one referred that the G17 G18 was the cause of the SYNTAX error, you seem to be behind the 8Ball.
Mactec54
Re: Error in my G code, post processor, controller settings, etc. Help!
This is no valid fanuc G-Code.
Normaly after a charakter there must be a number.
Re: Error in my G code, post processor, controller settings, etc. Help!
I got a post that seems like it should work, but I still get the syntax error. The code I have now looks like:
I'm having a fun time learning these controls, could be a little more intuitive but it's workable. I should mention this is not to run an actual part, I'm just messing around with the different post processors to find and edit one that will work with my machine. As soon as I can get the machine moving under GCode I should be able to teach myself the rest (it's been almost 10 years since I've run a part)Code:% O0004 (MACHINE) ( VENDOR EMCO) (T1 D=4. CR=0. - ZMIN=-1. - FLAT END MILL) N10 G90 G94 G17 G49 G40 G80 N15 G21 N20 G28 G91 Z0. N25 G90 (FACE1) N30 T1 M06 N35 S3500 M03 N40 G54 N45 G00 X75.4 Y1.811 N50 G43 Z15. H01 N55 G00 Z5. N60 G01 Z-0.6 F960. N65 G18 G03 X75. Z-1. I-0.4 N70 G01 X72.8 N75 X0. N80 G17 G02 Y5.584 J1.887 N85 G01 X72.8 N90 G03 Y9.357 J1.887 N95 G01 X0. N100 G02 Y13.131 J1.887 N105 G01 X72.8 N110 G03 Y16.904 J1.887 N115 G01 X0. N120 G02 Y20.677 J1.887 N125 G01 X72.8 N130 G03 Y24.45 J1.887 N135 G01 X0. N140 G02 Y28.223 J1.887 N145 G01 X72.8 N150 G03 Y31.996 J1.887 N155 G01 X0. N160 G02 Y35.769 J1.887 N165 G01 X72.8 N170 G03 Y39.543 J1.887 N175 G01 X0. N180 G02 Y43.316 J1.887 N185 G01 X72.8 N190 G03 Y47.089 J1.887 N195 G01 X0. N200 G02 Y50.862 J1.887 N205 G01 X72.8 N210 G18 G02 X73.2 Z-0.6 K0.4 N215 G00 Z15. N220 G17 N225 G28 G91 Z0. N230 G90 N235 G49 N240 G28 G91 X0. Y0. N245 G90 N250 M30 %
You did.... when you queried why he had it in his prog.No one referred that the G17 G18 was the cause of the SYNTAX error, you seem to be behind the 8Ball.
It had NO BEARING on his issue... WTF did you have to mention it ?
It is of no interest to you (or anyone else) on that part of his code
Michael... that looks a better fanuc code
... try single stepping thru the prog.
Re: Error in my G code, post processor, controller settings, etc. Help!
It was just a question I was asking him, so stop pretending suppernut
This is what I posted I guess you can't read, (Is it by design that you are using a different work plane G18 and G17)
Mactec54
Re: Error in my G code, post processor, controller settings, etc. Help!
What Emco Mill do you have
Mactec54
Re: Error in my G code, post processor, controller settings, etc. Help!
I have multiple, but this particular mill is the PC mill 55. It has Fanuc 21 controls on a windows PC.
Thanks for the tips guys! I just went through each post processor that they had available for fanuc controls one by one and I found one that worked. To be specific I downloaded them to my own location on the PC and refered to those, it seems that the fanuc post processor that is installed be default with inventor (or HSM works or something, I have tons of autodesk stuff installed) did extra stuff, although I'm not sure. The working post outputs strictly the code with no comments or fancy stuff.
The only thing I have been unable to figure out (Haven't looked much into it yet) is it gives an error code to the extent of "F value out of range" (not verbatim but you get the idea). I went in and changed the F value (Feed value, right?) manually from 960 to 100 then the machine accepted the code with no errors. If I remember correctly the F value should be in mm/min? I'm puzzled as to this error as the machine should be capable of 2000mm/min max feed.
But for now all is working and I'm happy
When you guys suggest things like single stepping through the code, I understand what you guys mean but I'm lost with this interface at the moment. I almost gave up and just retrofitted to linuxCNC, but now I'm going to learn a thing or two about the controls on this machine since I've got the post processor figured out (except for the f value)
Re: Error in my G code, post processor, controller settings, etc. Help!
Yes, the interface when it gives you trouble, they are a pain, I have a modified PC120 and an older 140T.I have multiple, but this particular mill is the PC mill 55. It has Fanuc 21 controls on a windows PC.
Thanks for the tips guys! I just went through each post processor that they had available for fanuc controls one by one and I found one that worked. To be specific I downloaded them to my own location on the PC and refered to those, it seems that the fanuc post processor that is installed be default with inventor (or HSM works or something, I have tons of autodesk stuff installed) did extra stuff, although I'm not sure. The working post outputs strictly the code with no comments or fancy stuff.
The only thing I have been unable to figure out (Haven't looked much into it yet) is it gives an error code to the extent of "F value out of range" (not verbatim but you get the idea). I went in and changed the F value (Feed value, right?) manually from 960 to 100 then the machine accepted the code with no errors. If I remember correctly the F value should be in mm/min? I'm puzzled as to this error as the machine should be capable of 2000mm/min max feed.
But for now all is working and I'm happy
When you guys suggest things like single stepping through the code, I understand what you guys mean but I'm lost with this interface at the moment. I almost gave up and just retrofitted to linuxCNC, but now I'm going to learn a thing or two about the controls on this machine since I've got the post processor figured out (except for the f value)
Mactec54
Posting Permissions
Reply with Quote