Hello Guest it is June 24, 2021, 02:31:49 PM

Author Topic: gcode mastercam offset question  (Read 8536 times)

0 Members and 1 Guest are viewing this topic.

gcode mastercam offset question
« on: December 31, 2009, 11:42:00 PM »
I used mastercam 9.1 to program a 2 inch diameter circle offset to the outside with a 1/2" diameter endmill. It cuts 1.75" diameter.
I have checked the machine calibration on 10 inch moves x and y axis it moves 10 inches on each axis when told to.
It makes a round circle.
I am using the demo version of Mach3 I know this is limited to a few lines of code is it also disabled on cutter comp?
Possibly the post I am using is off? I got it from a link on this forum and it stated it was for mastercam 9.x
I would not be suprised to get a 1.5" circle which would mean the cutter comp was not working at all. Here is the G code generated by mastercam.
I read G code, sort of, circles and radius are difficult for me
Thanks for any help
%
O0000 (TESTM)
(MASTERCAM - V9.)
(MC9 FILE  - E:\ROCKING HORSE\TESTM.MC9)
(POST      - C:\MCAM9\MILL\POSTS\_MACH3B.PST)
(MATERIAL  - ALUMINUM INCH - 2024)
(PROGRAM   - TESTM.NC)
(DATE      - DEC-31-09)
(TIME      - 23:39)
(POST DEV  - NovaLab)
(NWDTOOL N"UNDEFINED" T1 D.5 F.5 L1. A45. CD1. CL.5 SD1. C0)
(NWDSTOCK X0. Y0. Z0. OTC OX0. OY0. OZ0.)
N100 G00 G17 G20 G40 G49 G80 G90
N102 (WCS: TOP)
N104 T1 M06 (UNDEFINED)
N106 (MAX - Z.1)
N108 (MIN - Z-.1)
N110 G00 Z.1
N112 G00 X-2.25 Y.5 S1069 M03
N114 G01 Z-.1 F30.
N116 X-1.75
N118 G02 X-1.25 Y0. I0. J-.5
N120 G03 I1.25 J0.
N122 G02 X-1.75 Y-.5 I-.5 J0.
N124 G01 X-2.25
N126 Z0.
N128 M05
N130 G90
N132 M30
%

Offline Sam

*
  • *
  •  987 987
    • View Profile
    • hillbillyhilton.com
Re: gcode mastercam offset question
« Reply #1 on: January 01, 2010, 12:58:13 AM »
Yes, I do believe cutter comp is turned off in the demo version. In mastercam, make sure that your cutter comp is set to 'computer', and not 'control'. That should solve your issue.
"CONFIDENCE: it's the feeling you experience before you fully understand the situation."
Re: gcode mastercam offset question
« Reply #2 on: January 01, 2010, 10:09:36 AM »
I am still testing the machine and software so have not bought Mach3. can someone please confirm that cutter comp is not just disabled but skewed in the demo version before I buy? If cutter comp was simply disabled I should have gotten a 1.5" circle 2" less .25" on each side of the diameter. I did not I got a 1.75" circle. Thank you for the response Sam, I am familiar with Mastercam and have chosen computer as my offset source.

Offline Sam

*
  • *
  •  987 987
    • View Profile
    • hillbillyhilton.com
Re: gcode mastercam offset question
« Reply #3 on: January 01, 2010, 01:48:35 PM »
You are correct, you should get a 1.5" circle if you programmed a 2" circle and cut it with a .5" cutter. Lets take out the comments in the file to have an easier look at it. There is not a cutter comp called in the code. The circle is 2.5" as coded , not 2" with comp on. If you cut it with a .5" cutter, you should get a 2" circle. You say that your getting a 1.75" circle though, so something is still wrong. You say that your steps are set correctly and the machine does truly move the commanded distance when told.The only thing I can think of that might give you a 1.75" circle would be that your using a larger cutter instead of a .5" cutter. Maybe someone else can chime in with a better explanation, and enlighten both of us. As for a note on the cutter comp...It is being modified in the newer version of Mach. I do not know the specifics on the changes, I'm sure there is a post somewhere here going into detail about comp. Sorry I can't be of any more help to you in that regard.

%
O0000
N100 G00 G17 G20 G40 G49 G80 G90
N104 T1 M06
N110 G00 Z.1
N112 G00 X-2.25 Y.5 S1069 M03
N114 G01 Z-.1 F30.
N116 X-1.75
N118 G02 X-1.25 Y0. I0. J-.5
N120 G03 I1.25 J0.
N122 G02 X-1.75 Y-.5 I-.5 J0.
N124 G01 X-2.25
N126 Z0.
N128 M05
N130 G90
N132 M30
%

« Last Edit: January 01, 2010, 01:50:08 PM by Sam »
"CONFIDENCE: it's the feeling you experience before you fully understand the situation."
Re: gcode mastercam offset question
« Reply #4 on: January 01, 2010, 03:19:20 PM »
Sam, right on all counts as far as I know, like I said I read Gcode sort of the line
N120 G03 I1.25 J0.
is the circle and it should define a 2.5" circle which should result in the machine cutting a 2" circle.
I am sure that Mastercam handles the cutter comp and therefore I am quite sure the G code is right.
I am using a 1/2" diameter cutter.
Once again I have told the machine to move 10 inches (on both x and Y axes0 in the input area on the MIDI screen code such as
G0 X10 Y0 and it moves 10 inches close as I can measure.
So where can the problem be? only thing I can think is maybe mach 3 is trying to do a cutter comp too? for a smaller cutter the other direction?
I don't know but I don't want to buy the program if I can't get it to cut proper dimensions.
On the run screen there is a tool information area it shows all 000s
fustrating

Offline Sam

*
  • *
  •  987 987
    • View Profile
    • hillbillyhilton.com
Re: gcode mastercam offset question
« Reply #5 on: January 01, 2010, 04:33:43 PM »
Quote
only thing I can think is maybe mach 3 is trying to do a cutter comp too?
No. There is no cutter comp in the code.
Quote
for a smaller cutter the other direction?
I know what your saying. Comped to the inside instead of the outside. Not possible, because there is no cutter comp in the code.
If you do a single step through the code, you can see that Mach is telling the machine the correct points to go to. The circle starts at X -1.25, and 180 degrees later is indeed at X +1.25. This is what your seeing too, correct?
If you say that your machine travels 10 inches when you tell it to, and your using a half inch cutter, the only other option that I can think of that would cause the problem is that you have it scaled down in Mach. The "scale" LED's are not flashing, are they?
"CONFIDENCE: it's the feeling you experience before you fully understand the situation."

Offline ger21

*
  • *
  •  6,292 6,292
    • View Profile
    • The CNC Woodworker
Re: gcode mastercam offset question
« Reply #6 on: January 01, 2010, 05:17:01 PM »
Cutter Comp works fine in demo mode. I've used it extensively over the years testing before my machine was running.

But, as Sam said, you're code is not using comp.

I just ran your original code, and the toolpath did indeed make a 2.5" circle. If your seeing 1.75, something else is wrong.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: gcode mastercam offset question
« Reply #7 on: January 01, 2010, 05:49:37 PM »
Thanks for the help. I did not realize mach3 supported scaling but I don't think I had it on. I will have to play with the machine more, it must be something simple that I am missing. I need to put a newer computer on the machine as the one I have on it is too slow. I am going to try cutting a rectangle next time I got to the shop. That mayh tell me something. Thanks again.
Re: gcode mastercam offset question
« Reply #8 on: January 02, 2010, 07:46:08 PM »
I figured it out, my fault. I checked my 10 inch move with a tape measure on the table, new machine, just starting so I will dial in accuracy later. I started at 1" on the tape measure for accuracy and moved 10 inches and ended up at 10 inches. Then I checked 1" travel with a dial indicator and it ended up at 0. My problem was I should have ended up at 11 inches on the tape measure and the dial indicator was only moving .9 inches this was causing my 2 inch circle to be off by 10%. oops

Offline Sam

*
  • *
  •  987 987
    • View Profile
    • hillbillyhilton.com
Re: gcode mastercam offset question
« Reply #9 on: January 02, 2010, 07:58:09 PM »
been there, done that.
"CONFIDENCE: it's the feeling you experience before you fully understand the situation."