convert in G_code

[kiethnt]

Dear all,
Now I using MasterCam V9.1 to create 2D contour milling, in which I have some straight line and two arc. I have done to make the Toll path and post to .NC file, however when I check all statement in NC file I see that most of tool path for arc is declared in term radius of arc for example G2X11.2Y87.3R16.1.But now I want to exchange this statement to G2X11.2Y87.3 Ixxxx Jxxxx so any body know how to do this please show me or send to me any document talk about this. many thank for your help.
my email: kiethnt@yahoo.com

[Switcher]

Post a sample file here, so we can see what you need.


.

[kiethnt]

Dear Mr Switcher,
As your request let I post my sample file .MC9 and NC file here. Please show me how to change all G02 (G03) with radius Rxx to G02 (G03) with Ixx Jxx. Thank for your help.

[asjad]

He wants to generate arc's program using vector co-ordinates like i, j, k instead of R defination.

If i haven't interpreat his mean wrong:

Example: For an arc with 50mm redius program at around X0 Y0 co-ordinates

MASTERCAM 9.1 GENERATES LIKE THIS:

%
G90 G10 L2 P1 X****** Y****** Z*******;
G0 G80 G90 G40;
G54;
M06 T1;
G43 Z200 H1;
X0 Y0 MO3 S1000;
Z50;
G01 Z-2 F2000:
G01 G42 X-50 D1 F100;
G02 X50 Y0 R50;
G01 G40 X0 F2000;
G0 Z200;
MO5;
M30;
%


HE WANTS LIKE THIS:

%
G90 G10 L2 P1 X****** Y****** Z*******;
G0 G80 G90 G40;
G54;
M06 T1;
G43 Z200 H1;
X0 Y0 MO3 S1000;
Z50;
G01 Z-2 F2000;
G01 G42 X-50 D1 F100;
G02 X50 Y0 I50 J0;
G01 G40 X0 F2000;
G0 Z200;
MO5;
M30;
%

[kiethnt]

Dear Chip Sweeper,
Exactly what I means., becuse I have just start with G_code so I want to know how to convert them. Could you please show me more detail. Thank in advance

[MetLHead]

Hi keithnt,

I took your file and converted the arcs to IJ using NCPlot v2. NCPlot has tools for converting arc centers between IJK and R specified. I'm sure you would rather be able to post the program from Mastercam in the correct format, but I thought this might help.

Thanks,
Scott

[psychomill]

Keithnt...

In your post file (it will be a ".pst" file in your mill post folder of Mastercam), you should see a line that looks like this under "General Post Settings"

arcoutput : 1 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180

Your current value is probably a "1" like above. Change it to a "0" to output IJK like this:

arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180

[asjad]

I have made necessary chages in .pst file and posted here attachment .... just download and unzip and overwrite this file at C:\Mcam9\Mill\Posts ..... then try to run your run your post processer file...... i am sure it will generate your arcs in i,j,k mode .....



Goodluck!

[kiethnt]

Dear Mr Psychomill,
I have found General Post Seetting in Master Cam many time but until now I don't see where it is. Now I'm using MasterCam V9.1. Could you please show me again. Thank very much

[psychomill]

It might depend on which post file you're using... but it should look something like this in the .pst file ......
.
.
.


# --------------------------------------------------------------------------
# General Output Settings
# --------------------------------------------------------------------------
sub_level : 2 #Enable automatic subprogram support, ext enabled
breakarcs : 0 #Break arcs, 0 = no, 1 = quadrants, 2 = 180deg. max arcs

arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180
arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
do_full_arc : 1 #Allow full circle output? 0=no, 1=yes
helix_arc : 1 #Support helix arc output, 0=no, 1=all planes, 2=XY plane only
arccheck : 1 #Check for small arcs, convert to linear
atol : .01 #Angularity tolerance for arccheck = 2
ltol : .002 #Length tolerance for arccheck = 1

.
.
.
etc, etc, etc

The line in bold above is the one you want to change. Also, make sure you make a backup copy of the original post file before making changes. That way, in case you mess up, you can still get back to the original one...

[kiethnt]

Really thank Mr Dsychomill, let me try again but I think it will be OK for this time.