Radius output

[MSL]

Hi,

How can I output all my values in radius instead of diameter? I need to output some G-codes for our grinder.

I’m using Generic Haas 4x MT Lathe post.

Thank you.

 

[Guest]

Doh!!!

Alex is correct.....

I mis-read it thinking your rads needed to be changed

Edited November 29, 2017 by Guest

[Alex Dales]

dia_mult     : 2     #Multiplier for output on X axis (Neg. switches sign of X)

 

change to 1

[MSL]

That was the first think I changed. It did not change anything.

[Guest]

I just tested this in the MPLFAN and changing from 2 to 1 did change from diametric to radius output

1. Are you certain you edited the correct post

2. Did you save the post file after the edit

[MSL]

Thank you for testing. But somehow it is not working here. I'm using metric machine definition which should not effect the output I think.

I will test with different posts to see the results.

 

[MSL]

Attached is a zip-2-go file.

Test Part.ZIP

[Alex Dales]

57 minutes ago, MSL said:

Attached is a zip-2-go file.

Test Part.ZIP

I just tested with your files and changing dia_mult to 1 changed all the X values from Diameter to Radius.

modified post attached. 

Code below.

 

ORIGNAL

%
O0010
(BUSHING)
(DATE=DD-MM-YY - 29-11-17 TIME=HH:MM - 15:59)
(MCX FILE - C:\USERS\ALEX.DALES\DESKTOP\OPEN POST MODS\EMC\TEST PART.MCAM)
(NC FILE - C:\USERS\ALEX.DALES\DOCUMENTS\MY MCAM2018\LATHE\NC\BUSHING.NC)
(MATERIAL - ALUMINUM MM - 2024)
G21
(TOOL - 1 OFFSET - 1)
(OD GROOVE CENTER - NARROW  INSERT - N151.2-185-20-5G)
(2MM BOTTON TOOL)
G28 U0. V0. W0.
G50 X250. Y0. Z250.
G00 T0101
G18
G97 S750 M3
G00 X18.268 Z-1.381
G99 G01 X16.268 F.5
G18 G2 X13.506 Z0. R1.381
X11.42 Z-.419 R1.508
X9.55 Z-2.608 R3.032
G1 X7.55 Z-2.609
G28 U0. V0. W0. M5
T0100
M30
%
 

Changed

%
O0010
(BUSHING)
(DATE=DD-MM-YY - 29-11-17 TIME=HH:MM - 15:59)
(MCX FILE - C:\USERS\ALEX.DALES\DESKTOP\OPEN POST MODS\EMC\TEST PART.MCAM)
(NC FILE - C:\USERS\ALEX.DALES\DOCUMENTS\MY MCAM2018\LATHE\NC\BUSHING.NC)
(MATERIAL - ALUMINUM MM - 2024)
G21
(TOOL - 1 OFFSET - 1)
(OD GROOVE CENTER - NARROW  INSERT - N151.2-185-20-5G)
(2MM BOTTON TOOL)
G28 U0. V0. W0.
G50 X125. Y0. Z250.
G00 T0101
G18
G97 S750 M3
G00 X9.134 Z-1.381
G99 G01 X8.134 F.5
G18 G2 X6.753 Z0. R1.381
X5.71 Z-.419 R1.508
X4.775 Z-2.608 R3.032
G1 X3.775 Z-2.609
G28 U0. V0. W0. M5
T0100
M30
%
 

 

Generic Haas SL 4X MT_Lathe.zip

[MSL]

Thank you very much Alex and JParis for the help. Sorry my bad, I was outputting from wrong post.

[Colin Gilchrist]

58 minutes ago, MSL said:

Thank you very much Alex and JParis for the help. Sorry my bad, I was outputting from wrong post.

I hate it when that happens!

Also note, if you happen to put a copy of the PST file in the same folder as your Mastercam File, and that PST file has the same name as the PST that is linked in the Machine Definition that is loaded in your Mastercam File, then Mastercam will grab the "Local" copy of the Post file, even though it "shows" the correct File Path in the Machine Group Properties. (I've been bit by that many times.)

If you are ever in doubt, as to "which Post" is being run, you can "override" the Post being used.

Press the "G1" button to Post the Operations. When the Post Processing Dialog Box pops-up, use CTRL + SHIFT + ALT + P. This will enable the "Select post" button, and you can override which Post is being used to output your NC Code "on-the-fly". Just ignore the warning message that pops up...