[theemudracer]

I am loading some tool offsets with a G10 at the front of the prg. like this.

G10 P10011 X3.4444 Z 5.5555;
G10 P10021 X4.4444 Z 6.5555;
G11

The problem is when I put a value in the wear offset it resets it to 0. after it reads the G10 again at the front of the prg.

Is there a way to keep it from resetting the wear every time it reads the G10???

[cnc-king]

I am loading some tool offsets with a G10 at the front of the prg. like this.

G10 P10011 X3.4444 Z 5.5555;
G10 P10021 X4.4444 Z 6.5555;
G11

The problem is when I put a value in the wear offset it resets it to 0. after it reads the G10 again at the front of the prg.

Is there a way to keep it from resetting the wear every time it reads the G10???

i have never seen G10 code used the way you have it defined, the Fanuc manual has it defined

Work coordinates

G10 G90 L2/L20 P1 X?.????? Y?.????? Z?.????
L2 activates G54 Thru G59
P1 = G54 Etc.

L20 Activates G54.1P1 thru G54.1P48
P value reacts the same way

Tool offsets
G10 G90 L10 P?.???? R?.????
G10 G90 L11 P?.???? R?.????
G10 G90 L12 P?.???? R?.????
G10 G90 L13 P?.???? R?.????
P is Offset #
R is Tool Compensation amount

L10 thru L13 denotes H & D Geometry and Wear Values etc

[theemudracer]

This is the way my Fanuc book says to load tool geometry. It works but it resets the wear everytime. 18-I tb Lathe.

[ChattaMan]

@theemudracer...

Why don't you set your wear offset using G10 on the line after setting your tool offset?

[theemudracer]

Because i dont trust the operators to edit any programs. We are using Capto tool holders that are very repeatable and just need to add or subtract a little wear now and then. I was hoping the operator could still do this on the wear page instead of editing the wear at the front of the prg.

[ChattaMan]

Look in your manual for which machine variable is used for geom/wear.

Maybe it's #2500 or #10000??

Get the control to read your wear offset and enter it into an unused wear offset. Then set geom offset with yer G10's. Then read the value entered in the unused offset and enter it back into the wanted wear offset after G10's.

eg.

#2599=#2511 (reads wear entered by operator and writes to unused offset)

G10 P10011 X3.4444 Z 5.5555;
G10 P10021 X4.4444 Z 6.5555;
G11

(#2511 now zero'd by G10)

#2511=#2599 (wear offset now re-entered)

Check your manual for which machine variables to use (#'s).

[theemudracer]

Very nice. Exactly the concept I was looking for. I should have thought of that. Some things are so simple after someone shows you how ..ha ha



thanks a million

[Mitsui Seiki]

Why don't you use MDI to set:
G10 P10011 X3.4444 Z 5.5555;
G10 P10021 X4.4444 Z 6.5555;
G11
instead of in the program?
Or do you have to do it for every part?

[theemudracer]

So all the operator has to do is put the correct tools in and hit the green button and add wear when necesarry. I have to make it idiot proof so to speak.

[Mitsui Seiki]

Right.

[Bluesman]

So all the operator has to do is put the correct tools in and hit the green button and add wear when necesarry. I have to make it idiot proof so to speak.

Here is how i keep th operators from blowing up our stuff all the red is offset protection, When there is no other offsets allowed then I overwrite the system varible to "0" like #12001=0 I keep all that in a seperate sup that is password protected

O8013(T01 MILLING)
(REV A. LINKED OFFSETS RAS 8-3-05)
G0G17G21G40G49G80G90G94G98M11
G0G90G10L2P6X-355.0Y-660.0Z-710.0B0.0(G59)
IF[#534NE18048323.]THEN#3000=53(WRONG PROJECT)
#30=155.56(NOMINAL TOOL LENGTH)
#31=.150(TOOL LENGTH TOLERANCE)
IF[[ABS[#10001-#30]]GT#31]THEN#3000=1(TOOL DATA ERROR H1)#1=3500(FIRST SFM)
#2=.007(FIRST FEED/TOOTH-INCHES)
#7=3500(SECOND SFM)
#8=.007(SECOND FEED/TOOTH-INCHES)
#3=2.0(CUTTER DIA-INCHES)
#4=5(NUMBER OF FLUTES/TEETH)
#5=ROUND[[#1*12]/[#3*3.1416]](CALCULATED RPM)
#6=[[#4*#2*#5]*25.4](CALCULATED FIRST FEED MM/M)
#9=ROUND[[#7*12]/[#3*3.1416]](CALCULATED RPM)
#10=[[#4*#8*#9]*25.4](CALCULATED SECOND FEE


Bluesman