Machsupport Forum

G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: GeorgeRace on February 11, 2009, 06:57:27 PM

Title: Need Help With G40, G41 & G42 Programming
Post by: GeorgeRace on February 11, 2009, 06:57:27 PM

Hi There:
Finally have the mill running just great under Mach3.

I have a very simple Bezel Making program that I just can't seem to make work using Cutter Radius Compensation.

The GCode I am using is below.  If someone could be so kind as to patch in, where indicated, the code to make it all work it would be greatly appreciated.  I would like to use the "P" Cutter Radius so that I can easily change cutter sizes when necessary.

Thanks much,
George

Here is the program code:

N5 (File Name = Instrument Bezel Maker on Wednesday February 11, 2009)
N10 (Default Mill Post)
N11
N12  (Simple Program To Cut Trim Bezel)
N14 
N15  G91.1
N16 (Bring Down Spindle)
N20    G0 Z0.2500 F30.0
N100
N102  (Please add code below to cut INSIDE the Circle)
N103  (Use G42 P.125 for Cutter Radius)
N104
N107 (Cut Large Center Hole)
N109   X3.220  Y1.7180
N110   G0 Z0.000 F5
N116   G2 I-1.53125  J0.000 F20
N121   G0  Z0.100
N122
N123  (Please add code below to cut OUTSIDE the Bezel)
N124  (Use G41 P.125 for Cutter Radius)
N125
N126 (Cut Around The Outside of Bezel)
N130   X0.3220  Y0.0003
N135   G01 Z0.0000 F5.0
N140   G2  X0.0022  Y0.3436  I-0.0146  J0.3112 F20
N145   G1  X0.0016  Y3.0954   
N150   G2  X0.3000  Y3.4036  I0.3000  J0.0000
N155   G1  X3.0717  Y3.4036   
N160   G2  X3.3717  Y3.1036  I0.0000  J-0.3000
N165   G1  X3.3679  Y0.3817   
N170   G2  X3.0872  Y0.0066  I-0.3556  J-0.0146
N175   G1  X0.3083  Y0.0067   
N180   G0  Z3.0000 F50
N183
N185 (Stop and Rewind File)
N190   M30

Title: Re: Need Help With G40, G41 & G42 Programming
Post by: Graham Waterworth on February 11, 2009, 07:14:58 PM

With out more detail its a good guess to have it like this

N5 (File Name = Instrument Bezel Maker on Wednesday February 11, 2009)
N10 (Default Mill Post)
N11
N12  (Simple Program To Cut Trim Bezel)
N14
N15  G91.1
N16 (Bring Down Spindle)
N20    G0 Z0.2500 F30.0
N100
N102  (Please add code below to cut INSIDE the Circle)
N103  (Use G42 P.125 for Cutter Radius)
N104
N107 (Cut Large Center Hole)
N109   X3.220 Y1.5 
          G42 P.125 Y1.7180
N110   G0 Z0.000 F5
N116   G2 I-1.53125  J0.000 F20
N121   G0  Z0.100
N122   G40

N123  (Please add code below to cut OUTSIDE the Bezel)
N124  (Use G41 P.125 for Cutter Radius)
N125
N126 (Cut Around The Outside of Bezel)
          X-.250 Y.0003
N130   G01 G41 P .125 X.322 F5.
N135   Z0
N140   G2  X0.0022  Y0.3436  I-0.0146  J0.3112 F20
N145   G1  X0.0016  Y3.0954   
N150   G2  X0.3000  Y3.4036  I0.3000  J0.0000
N155   G1  X3.0717  Y3.4036   
N160   G2  X3.3717  Y3.1036  I0.0000  J-0.3000
N165   G1  X3.3679  Y0.3817   
N170   G2  X3.0872  Y0.0066  I-0.3556  J-0.0146
N175   G1  X0.3083  Y0.0067   
N180   G0  Z3.0000 F50
N183   G40
N185 (Stop and Rewind File)
N190   M30

Graham

Title: Re: Need Help With G40, G41 & G42 Programming
Post by: GeorgeRace on February 11, 2009, 07:44:35 PM

Hi Graham:

Thanks for the very quick reply.

Is still doing strange stuff, much like the results that I had.

On the inner circle, it does not cut the circle but cuts a strange loop and leaves.

On the perimeter cut is starts by cutting into what would be the finished bezel, then proceeds to go around the perimeter.

Closer than I have come, but still not working correctly.

Maybe a quick look and a small tweak will solve the problems.

Thanks again,

George

Title: Re: Need Help With G40, G41 & G42 Programming
Post by: ger21 on February 11, 2009, 09:29:50 PM

Make sure you use the latest development version, as the comp is being changed and works differently in the newest version.

Title: Re: Need Help With G40, G41 & G42 Programming
Post by: Graham Waterworth on February 12, 2009, 11:13:42 AM

Post a drawing of what you are trying to make and then I can give you a working piece of code.

Graham

Title: Re: Need Help With G40, G41 & G42 Programming
Post by: GeorgeRace on February 12, 2009, 03:27:15 PM

Hello To All:

Boy, you guys sure do know how to help a guy out!

Took the advise and downloaded the latest development version of Mach3.

After getting it installed and setup, it processes your file Graham perfectly!

Now I need to know a couple of things about how you setup the parameters.  Parts of before and after details below.

What I need to know is Why did you choose the new value for Y1.5?

N107 (Cut Large Center Hole)
N109   X3.220  Y1.7180
N110   G0 Z0.000 F5
N116   G2 I-1.53125  J0.000 F20
N121   G0  Z0.100

N107 (Cut Large Center Hole)
N109   X3.220 Y1.5
          G42 P.125 Y1.7180
N110   G0 Z0.000 F5
N116   G2 I-1.53125  J0.000 F20
N121   G0  Z0.100
N122   G40

The second group before and after below.  Where did the X-.250 come from?
Why did you choose Y for one and X for the other?

Once I understand this I think all my current problems will be resolved.

Thanks,
George


N126 (Cut Around The Outside of Bezel)
N130   X0.3220  Y0.0003
N135   G01 Z0.0000 F5.0
N140   G2  X0.0022  Y0.3436  I-0.0146  J0.3112 F20


N126 (Cut Around The Outside of Bezel)
          X-.250 Y.0003
N130   G01 G41 P .125 X.322 F5.
N135   Z0
N140   G2  X0.0022  Y0.3436  I-0.0146  J0.3112 F20
N145   G1  X0.0016  Y3.0954  
N150   G2  X0.3000  Y3.4036  I0.3000  J0.0000