Hello Guest it is July 18, 2019, 05:34:35 AM

Author Topic: Wear Compensation - Mastercam 9.1  (Read 5028 times)

0 Members and 1 Guest are viewing this topic.

Wear Compensation - Mastercam 9.1
« on: February 15, 2012, 11:22:43 AM »
Hello,

I am trying to get wear compensation to work on my 3axis cnc router.  But every time I turn it on and I 0.01" or -.01" in for diameter wear in Mach3 it does not change the cut size of the part.  I have tried wear and reverse wear in mastercam.  Is there something special you gotta do in mach3 to get wear compensation to work? 

Here is my program:

%
O0000 (TEST)
(MASTERCAM - V9.)
(MC9 FILE  - C:\MCAM9\MILL\MC9\MONEY CARD.MC9)
(POST      - C:\MCAM9\MILL\POSTS\_MACH3B.PST)
(MATERIAL  - ALUMINUM INCH - 2024)
(PROGRAM   - TEST.NC)
(DATE      - FEB-15-12)
(TIME      - 11:21)
(POST DEV  - NovaLab)
(NWDTOOL N" 1/16 FLAT ENDMILL" T1 D.0625 F2. L3. CD2. CL1. SD2. C0)
(NWDSTOCK X0. Y0. Z0. OTC OX0. OY0. OZ0.)
N100 G00 G17 G20 G40 G49 G80 G90
N102 (1ST BOXES)
N104 T1 M06 ( 1/16 FLAT ENDMILL)
N106 (MAX - Z1.)
N108 (MIN - Z-.15)
N110 G00 Z1.
N112 G00 X4.875 Y8.7813 S22500 M03
N114 Z.1
N116 G01 Z-.15 F50.
N118 G42 D21 Y9.0938 F105.
N120 G02 X5. Y9.2188 I.125 J0.
N122 G01 X8.9688
N124 Y7.25
N126 G03 X9. Y7.2188 I.0313 J0.
N128 G01 X11.9688
N130 Y1.5313
N132 X1.0313
N134 Y9.2188
N136 X5.
N138 G02 X5.125 Y9.0938 I0. J-.125
N140 G01 G40 Y8.7813
N142 G00 Z1.
N144 M05
N146 G90
N148 M30

Offline BR549

*
  •  6,874 6,874
    • View Profile
Re: Wear Compensation - Mastercam 9.1
« Reply #1 on: February 15, 2012, 11:28:35 AM »
Mach3 does not do wear comp. It does do tool comp. 

Just a thought , (;-) TP
Re: Wear Compensation - Mastercam 9.1
« Reply #2 on: February 15, 2012, 11:55:20 AM »
Well even when I turn on cutter compensation it does not seem to work correctly.

Here is that program with cutter comp turned on.  And In mach3 I told it the cutter was 0.055" dia.  It cut the part as if there was no compensation turned on.  0.0313" larger per side.

%
O0000 (TEST)
(MASTERCAM - V9.)
(MC9 FILE  - C:\MCAM9\MILL\MC9\MONEY CARD.MC9)
(POST      - C:\MCAM9\MILL\POSTS\_MACH3B.PST)
(MATERIAL  - ALUMINUM INCH - 2024)
(PROGRAM   - TEST.NC)
(DATE      - FEB-15-12)
(TIME      - 11:55)
(POST DEV  - NovaLab)
(NWDTOOL N" 1/16 FLAT ENDMILL" T1 D.0625 F2. L3. CD2. CL1. SD2. C0)
(NWDSTOCK X0. Y0. Z0. OTC OX0. OY0. OZ0.)
N100 G00 G17 G20 G40 G49 G80 G90
N102 (1ST BOXES)
N104 T1 M06 ( 1/16 FLAT ENDMILL)
N106 (MAX - Z1.)
N108 (MIN - Z-.15)
N110 G00 Z1.
N112 G00 X4.875 Y8.8125 S22500 M03
N114 Z.1
N116 G01 Z-.15 F50.
N118 G42 D21 Y9.125 F105.
N120 G02 X5. Y9.25 I.125 J0.
N122 G01 X9.
N124 Y7.25
N126 X12.
N128 Y1.5
N130 X1.
N132 Y9.25
N134 X5.
N136 G02 X5.125 Y9.125 I0. J-.125
N138 G01 G40 Y8.8125
N140 G00 Z1.
N142 M05
N144 G90
N146 M30
%
« Last Edit: February 15, 2012, 11:59:09 AM by Smackre »

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Wear Compensation - Mastercam 9.1
« Reply #3 on: February 15, 2012, 12:08:19 PM »
You have .055 for the diameter of tool #21?
Gerry

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

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Wear Compensation - Mastercam 9.1
« Reply #4 on: February 15, 2012, 12:31:04 PM »
Ger21,

Why would it be tool#21?

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Wear Compensation - Mastercam 9.1
« Reply #5 on: February 15, 2012, 12:57:35 PM »
N118 G42 D21 Y9.125 F105.
Gerry

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

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline BR549

*
  •  6,874 6,874
    • View Profile
Re: Wear Compensation - Mastercam 9.1
« Reply #6 on: February 15, 2012, 01:23:01 PM »
Tool #21 is what the Gcode specifies for the Tool COmp call. There seems to be a problem in your MC post as in the notes it specifies T1 and in the tool change call it specifies t1 but IT CALLS TOOL #21 as the comped tool #

(;-) TP
« Last Edit: February 15, 2012, 01:26:17 PM by BR549 »
Re: Wear Compensation - Mastercam 9.1
« Reply #7 on: February 15, 2012, 08:38:20 PM »
Thanks for the help guys.  Fixed the D# and all is well now.  Now if I could just get my smoothstepper to stop kicking out on me!