Posting Diameter Offset number question

[BBIGOTON]

Does anyone know how to add to the diameter offset number. I'm trying to add 30 to my diameter offset. On V9 I used to be able to change it by changing the value on my set-up. I figured that by changing the number in the tool section of my control definition would do the trick but it didn't work. Can someone gim'me a hand?

%

O0001

*********************************

T1 - 3/4" ROUGH FLAT E.M. - 2-1/2" LG. - H1

T2 - 3/8" FINISH FLAT E.M. - 2" LG. - H2

T3 - 1/2" SPOTDRILL - H3

N100G20

N105G0G17G40G49G80G90

ROUGH LEFT END - RELIEF CUT

TOOL CHANGE

N110T1

N115M00

LOAD TOOL: 1

N120G0G90G54X-35.5822Y-1.8844S3750M3

N125G43H1Z4.M8

N130Z.1

N135G1Z-.635F75.

N140G41D1X-35.6706Y-1.796F30. <--want to add 30 to D value

N145X-35.8474Y-1.6192

N150G40X-36.589Y-.8777

N155Z-.535F100.

N160G0Z.25

N165X-35.5822Y-1.8844

N170Z-.535

N175G1Z-1.2699F75.

N180G41D1X-35.6706Y-1.796F30. <--want to add 30 to D value

N185X-35.8474Y-1.6192

N190G40X-36.589Y-.8777

N195Z-1.1699F100.

N200G0Z4.

ROUGH LEFT END - HALF

N205X-35.0731Y-1.7288

N210Z.1

N215G1Z-.635F75.

N220G41D1X-35.1615Y-1.6405F30. <--want to add 30 to D value

N225X-35.5151Y-1.2869

N230X-36.3271Y-.4748

N235G2X-36.625Y-.0843R.4049

N240G1Y.9693

N245G40Y1.1193

N250Z-.535F100.

N255G0Z.25

N260X-35.0731Y-1.7288

N265Z-.535

N270G1Z-1.2699F75.

N275G41D1X-35.1615Y-1.6405F30. <--want to add 30 to D value

N280X-35.5151Y-1.2869

N285X-36.3271Y-.4748

N290G2X-36.625Y-.0843R.4049

N295G1Y.9693

N300G40Y1.1193

N305Z-1.1699F100.

N310G0Z4.

N315M5

N320G91G28Z0.M9

N325M00

TOOL CHANGE

N330T2

N335M00

LOAD TOOL: 2

FINISH LEFT END - TOP

N340G0G90G54X-35.0961Y-1.3983S5000M3

N345G43H2Z4.M8

N350Z.1

N355G1Z-.635F75.

N360G41D2X-35.1845Y-1.3099F25. <--want to add 30 to D value

N365X-35.3613Y-1.1331

N370X-36.2103Y-.284

N375G3X-36.2382Y-.2709R.0457

N380G2X-36.4075Y-.0843R.1875

N385G1Y.9693

N390G40Y1.0943

N395Z-.535F100.

N400G0Z4.

N405X-35.0961Y-1.3983

N410Z-.535

N415G1Z-1.2699F75.

N420G41D2X-35.1845Y-1.3099F25. <--want to add 30 to D value

N425X-35.3613Y-1.1331

N430X-36.2103Y-.284

N435G3X-36.2382Y-.2709R.0457

N440G2X-36.4075Y-.0843R.1875

N445G1Y.9693

N450G40Y1.0943

N455Z-1.1699F100.

N460G0Z4.

FINISH LEFT END - BOTTOM

N465X-33.0961Y-3.3983

N470Z-1.1699

N475G1Z-1.6654F75.

N480G41D2X-33.1845Y-3.3099F25. <--want to add 30 to D value

N485X-33.3613Y-3.1331

N490X-36.2103Y-.284

N495G3X-36.2382Y-.2709R.0457

N500G2X-36.4075Y-.0843R.1875

N505G1Y.9693

N510G40Y1.0943

N515Z-1.5654F100.

N520G0Z4.

N525M5

N530G91G28Z0.M9

N535M00

TOOL CHANGE

N540T3

N545M00

LOAD TOOL: 3

SPOT 3/8-16 STI HOLES - HELICOILS - 11X

N550G0G90G54X-33.25Y0.S5000M3

N555G43H3Z4.M8

N560Z.1

N565G99G81Z-.2325R.1F30.

N570X-30.25

N575X-27.25

N580X-24.25

N585X-21.25

N590X-18.25

N595X-15.25

N600X-12.25

N605X-9.25

N610X-6.25

N615X-3.25

N620G80

N625Z4.

N630M5

N635G91G28Z0.M9

N640G28X0.Y0.

N645M30

%

 

Any help will be appreciated.

 

Alex

[BBIGOTON]

I forgot to add that I tried this:

 

ptoolcomment #Comment for tool

tloffno$ = tloffno$ + 30 <-- I added this

 

tnote = t$, toffnote = tloffno$, tlngnote = tlngno$

if tool_info = 1 | tool_info = 3,

sopen_prn, pstrtool, sdelimiter, *tnote, sdelimiter, *toffnote, sdelimiter, *tlngnote, sdelimiter, *tldia$, sclose_prn, e$

 

But it didn't work, I got the right output #+30 only on the first output of every tool offset but the ones after went back to single digits.

 

Thanx for any help.

 

Alex

[Kyle Waters]

Hi Alex,

 

Welcome to the forum! You did not mention what version of Mastercam you are using, as well as what post. If it is a newer MPMaster post, this is now located in the Control definition in the "Tool" section.

 

HTH

[Kyle Waters]

oops, I didn't read closely enough. Did you modify the control definition from within the part file, or go thru the Machine definition?

[john316]

.

 

There's a checkbox and place for a value in the CD.

 

.

[BBIGOTON]

Sorry guys, it's X3 and generic fanuc 3x post.

[gcode]

You can set this on the Tools page of the Control definition

[BBIGOTON]

Sorry guys, it's X3 and generic fanuc 3x post.

[BBIGOTON]

Kyle, John and Gcode, thank you for your suggestions but I must be doing something wrong because I changed the value in the control definition but nothing happened. I tried it out with a fanuc 3-axis and the mpmaster posts without luck. Any other suggestions?

 

Thanx guys.

 

Alex

[gcode]

Alex.

try this

Settings

Machine Definition Manager

Control Panel ( Icon tht looks like a TV)

Tool

Check Add to Tool and enter 30 in the Diamter field.

Green Check out saving at the prompts

Reload the Machine Def into your file..

It this doesn't work, try using a fresh copy of the post

[Bryan Johnson]

Alex,

Having the correct settings in your Machine Definition is one way to do this, but is far from bullet proof.

 

You are on the right track with your post edits. But you need to move your edits out of the “comment” section, and put them just before the offset is output.

 

There is a Haas post on the FTP that already has these edits. It will work for your example.

[Mgrenier]

Alex,

 

The control definition change does work. If you got the way Gcode tells you, you then have to reload the control definition for the particular MCX file you are working on.

 

Hope that helps,

[BBIGOTON]

I dunno why but my control definition is not working. What I did do though was to add this line to cutter comp: toffno$ = t$ + 30.....that worked.

 

Alex