Output the Work Offset values in program header

[rogkick]

Hi Guys,

Is it possible to output the work offset values in the program header? (Fanuc 4AX HMC)

Would be really handy for me if I could.

 

Thanks.

[Jeremy Grigsby]

You can use a G10 to automatically write to any work offset or tool offset values.

G90 G10 L2 P1 X5. Y6. Z7.

 

This overwrites g54 with the specified values

 

G91 G10 L2 P1 X.1 Y.1 Z0.

 

This incrementally updates G54 by .100 in x and .100 in y

 

G91 G10 L11 P2 R.001

 

This adds to the tool length wear offset(L11) of tool 2(P2) by the value of 0.001(R.001)

 

L10 tool length offset

L11 tool length wear offset

L12 tool radius offset

L13 tool radius wear offset

 

specifying G91 is an incremental update to value, G90 replaces with specified value

 

I don't know if this is what you were looking for.

[Jeremy Grigsby]

Upon reading you post again, I imagine you must have been talking about outputting from mastercam. I guess you could always do a manual entry?

[rogkick]

Thanks Jeremy

I am aware of the G10 ( we don't have the additional offset in control ), and what I was looking for was for example in a program header:

O0000(PLUNGE PART)

(DATE=DD-MM-YY - 06-03-13 TIME=HH:MM - 14:16)

(MCX FILE - C:\USERS\BOMBARDIER\DOCUMENTS\MY MCAMX6\RESTART_THINNER STOCK_FIRST SIDE BSCKUP.MCX-6)

(NC FILE - C:\USERS\BOMBARDIER\DOCUMENTS\MY MCAMX6\MILL\NC\PLUNGE PART.NC)

(MATERIAL - 17-4 PH 1150)

( T23 | 20MM. PLUNGE DRILL CRB | H23 | XY STOCK TO LEAVE - .5 | Z STOCK TO LEAVE - 0. )

(G54 X ... Y .... Z ...)

(G55 X ... Y .... Z ...)

etc

basically hard writing the values into the header, so the operator has them as a reference in the program and not just a setup sheet.

Does that make sense?

 

Thanks?

 

Edit: Manual Entry yes, but can it be output via the Post?

[Jeremy Grigsby]

What would actually be output as values? Machine coordinates?

[rogkick]

These values here in the picture would be what I would like.

[Jayson Kramer]

My Haas and Fadal post shows what fixtures are be used, Example of header from fadal:

 

TA,1

%

O1334 ( SCFV07D133-1-OP4-OPISIT REV: )

( SCFV07D133-1-OP4-OPISIT )

(MACHINE TOOL : FADAL FORMAT 1 )

(DATE - 24-02-13 )

(TIME - 14:37 )

(*)

(MATERIAL: )

(STOCK SIZE: X = 6.4996 Y = 11.9996 Z = 2.5 ) This is automatic

(HOME POSTION COORIDNATES ARE THE FOLLOWING)

(X= )

(Y= )

(Z= TOP OF PART)

(*)

( TOOL - 4 DIA. - .5 1/2 BALL ENDMILL )

( TOOL - 6 DIA. - .25 1/4 BALL ENDMILL )

(*)

(USING FIXTURE OFFSETS: E1 ) This is automatic

[cadman2112]

There is a post on the FTP that will buffer out the G10 info shown above.

 

You "could" modify the final output to achieve what you desire I believe.

[Josh Kinney -Elite Engineering]

It can be done. You can also buffer out the Tool Plane name. It gets complicated pretty quick.

 

Here's our HMC Code. Currently it doesn't buffer the tool plane(It will when I get time...). The VMC post's do (Below):

 

 

%

O0123 (12-4054)

(POST REV 1.1)

(NH4000DCG - HMC)

(MCX FILE - 421Z6302-1228--B_MFG.MCX-7)

(DATE - MAR-07-2013)

(TIME - 11:03 AM)

(USER ID - 725)

(OPERATIONS - 50/60/70)

 

 

#510=1(OPTIONAL N SEQ START)

 

IF[#510EQ1]GOTO3000

M0

(USING OPTIONAL N SEQ START)

M0

(YOU ARE STARTING PART WAY THROUGH)

N3000

 

(*** TOOL LIST ***)

(T1 - RTA401 - B3463 - 3/4" ENDMILL - D0.7500 - R0.0300)

(T2 - RTA1 - I321 -3" FACE MILL - D3.0000 - R0.0313)

(T8 - B3470 - 1/2" END MILL - 0.094" RAD - D0.5000 - R0.0940)

(T4 - O600 - 1/4"-90 SPOT DRILL - D0.2500)

(T5 - D1236 - #16 DRILL - D0.1770)

 

 

(*** USER DEFINED WORK COORDINATES START ***)

 

G90 G10 L20 P1 X0. Y14.5309 Z9.7 B0. ( G54.1 P1 B0. FACE)

G91 G10 L20 P1 X0. Y0. Z0. ( G54.1 P1 B0. INCREMENTAL WORK SHIFT )

 

G90 G10 L20 P2 X7.1324 Y14.5309 Z6.5741 B0. ( G54.1 P2 B312.67 FACE)

G91 G10 L20 P2 X0. Y0. Z0. ( G54.1 P2 B312.67 INCREMENTAL WORK SHIFT )

 

G90 G10 L20 P3 X1.0837 Y9.8565 Z10.643 B0. ( G54.1 P3 B180. FACE)

G91 G10 L20 P3 X0. Y0. Z0. ( G54.1 P3 B180. INCREMENTAL WORK SHIFT )

 

G90 G10 L20 P4 X-6.4215 Y9.182 Z8.7367 B0. ( G54.1 P4 B227.33 FACE)

G91 G10 L20 P4 X0. Y0. Z0. ( G54.1 P4 B227.33 INCREMENTAL WORK SHIFT )

 

G90 G10 L20 P25 X10.779 Y11.6573 Z0. B0. ( G54.1 P25 B270. FACE)

G91 G10 L20 P25 X0.002 Y0. Z0. ( G54.1 P25 B270. INCREMENTAL WORK SHIFT )

 

 

(*** WORK COORDINATES END ***)

 

GOTO #510 (JUMP TO SEQ)

 

 

M01

N1(Sequence #1.)

(TOOL# 1 - RTA401 - B3463 - 3/4" ENDMILL - DIA. - .75)

(MAX - Z-3.1249)

( PALLET CHECK - PALLET1 )

/M500C1

G00 G17 G40 G80 G90 G53 Z0.

T1 M6

 

 

 

Our VMC Code add's another layer of Complexity:

 

%

O0123 (OP60FIX)

(POST REV 1.1)

(DURACENTER 5 - VMC)

(MCX FILE - SIDE ARMREST STRUCTURE_10.09.2012-OP50-OP60.MCX-6)

(DATE - MAR-08-2013)

(TIME - 6:56 AM)

(USER ID - 725)

(OPERATIONS - 50/60/70)

 

 

#510=1(OPTIONAL N SEQ START)

 

IF[#510EQ1]GOTO3000

M0

(USING OPTIONAL N SEQ START)

M0

(YOU ARE STARTING PART WAY THROUGH)

N3000

 

(*** TOOL LIST ***)

(T4 - O2364 - 1/2-90 SPOT DRILL - D0.5000)

(T7 - D1229 - 1/4" DRILL PARABOLIC - D0.2500)

 

(*** OVERWRITE MACRO ADJUSTMENTS ***)

 

G90 G52 X0. Y0. Z0.

 

(*** USER DEFINED WORK COORDINATES START ***)

 

M01 (MAKE YOU SET YOUR VISE LOCATIONS FROM THE CHART)

 

( OP50 - G54 VISE ORIGIN )

G90 G10 L2 P1 X0. Y0. Z0.

( OP50 - G54 PART LOCATION IN RELATION TO VISE ORIGIN )

G91 G10 L2 P1 X0. Y0. Z0.

( OP50 - G54 INCREMENTAL WORK SHIFT )

G91 G10 L2 P1 X0. Y0. Z0.

 

( OP60 - G55 VISE ORIGIN )

G90 G10 L2 P2 X0. Y0. Z0.

( OP60 - G55 PART LOCATION IN RELATION TO VISE ORIGIN )

G91 G10 L2 P2 X0. Y0. Z0.

( OP60 - G55 INCREMENTAL WORK SHIFT )

G91 G10 L2 P2 X0. Y0. Z0.

 

(*** WORK COORDINATES END ***)

 

GOTO #510 (JUMP TO SEQ)

 

 

M01

N1(Sequence #1.)

(TOOL# 4 - O2364 - 1/2-90 Spot Drill)

(MAX - Z-.115)

T4 M06

[Josh Kinney -Elite Engineering]

That is un-edited code. I set my WCS to the top of my vise body, then my toolplane to whatever location I want as my zero. We have a sub plate with known vise location and a chart that says what those locations are.

 

So here's the breakdown.

 

WCS is set to "Top" (Or whatever is the top/center of vise body)

 

OP50 is the toolplane name in MasterCam

 

54 is set as the work offset.

 

The G90 G10 line is always zeros.

 

The G91 line is the distance (Incremental) between "Top" and "OP50" Toolplane.

 

The next G91 G10 is just a place for the operator to make adjustments.

 

Slap the vise on the subplate with correct jaws/tooling, type the location values off the chart into the G90 G10 lines, load tool offsets from the presetter, load tools in the machine, load the code. Hit CYCLE START.

 

( OP50 - G54 VISE ORIGIN )

G90 G10 L2 P1 X0. Y0. Z0.

( OP50 - G54 PART LOCATION IN RELATION TO VISE ORIGIN )

G91 G10 L2 P1 X0. Y0. Z0.

( OP50 - G54 INCREMENTAL WORK SHIFT )

G91 G10 L2 P1 X0. Y0. Z0.

[GoetzInd]

We use a buffer to accomplish this. Zoober had a good post explaining how to do it if you are post savvy. Otherwise your re-seller can do it.

 

Mike

[Josh Kinney -Elite Engineering]

I used the method in Zoober's post that was written by Jim @ CNC. The hard part was the addition of buffering stoolplname.