change offset in program

[jianjianca]

quick question, a job about making 5 parts from a stock material.
program as

p001
p001
p001 (need to change tool #3 offset here)
p001
p001

change tool # 3 offset back to zero.

anybody can tell me how to change the program or make a simple marco to change the offset automatically, thanks.

it s easy to get mistake when do it manually

[Geof]

Which offset do you want to change; length or diameter? G10 is the code for entering offsets from a program.

For example:

G10 L12 G90 P3 R0.5 will enter a tool diameter offset of 0.5 or any other value you put for R.

G10 L10 G90 P3 R5.0 will enter a tool length offset of 5.0 or any other value you put for R.

Some words of caution: Using a G10 command to change your tool length offset can be very, very risky. If you make a typo you may finish up putting the tool much further down than you intended.

[jianjianca]

does g10 work for lathe machine also? how can i check if the tool length changed or not while the program runing. thanks a lot

[Geof]

Yes G10 works on the lathe. Are you trying to take a length of stock in the chuck and machine and part-off 5 complete pieces? You can do this but the easiest way is to change work zeroes not tool offsets.

[bob in windsor]

Try finding the system variable number for tool offsets on your control.For example on Fanuc 16m insert #2013=0 where you need it changed.Do it on a test run above the part first and check your offset table after it reads that line.

[jianjianca]

Yes G10 works on the lathe. Are you trying to take a length of stock in the chuck and machine and part-off 5 complete pieces? You can do this but the easiest way is to change work zeroes not tool offsets.

sorry, it s radius offset. i dont know why they change it. anyway , it s according to the real situation.

and thanks to bob, i will try to figure out the var and the address, but seems making the problem more complicated.

[jianjianca]

to geof, if i wanna use g11 to cancel the offset, do i need to add any parameter on it? thx

[Geof]

to geof, if i wanna use g11 to cancel the offset, do i need to add any parameter on it? thx

I don't completely understand this question. G10 is the code for setting offsets; in other words entering values into the offset tables. When you talk about cancelling that is related to using the offset value that is in the table.

These examples are for a Haas control running in Fanuc mode, the principles should be the same for most controls.

For example G10 L10 G90 P3 R0.03 will enter the value of 0.03 in the tool nose radius column for tool 3.

In a program you use this value when you have a tool compensation command G41 D03 or G42 D03 and you cancel the tool compensation using G40.

Similarly G10 L10 G90 P3 X-5.0 Z-5.0 will enter these values in the X and Z columns in the offset tables and when you do a tool command T303 these values will be used for the tool offset.

In fanuc I do not know how to cancel the tool offset but you can set the X and Z values back to zero using G10 L10 G90 P3 X0. Z0.

[jianjianca]

to Geof, yes, u r right, i can set it back to zero. i just checked the G Code table, G10 is to set tool offset( u already show me how to use it), and G11 is to cancel tool offset( i want to know the detail). got another problem, i found another explain for G10 code is to set the origin.

[Geof]

I cannot help you with G11 because it is not used on the Haas.

G10 can be used to set a lot of things including the origin, G54, G55 etc. It depends on the L value and P value. You should be able to find these somewhere in your explanation.

[jianjianca]

To Geof, thx alot again, i tried g11 on misubishi, it didnt work, and G10 L12 too. when i use G10 L10 G90 P10 x1. ; the tool data changed , but not the tool offset. can u tell me where i can find a table for those detail parameters.

[Geof]

I don't know where to find any online references. Here is information taken from one of my machine manuals.

L selects geometry, wear, shift or work coordinates, with a P choosing the actual entry.

L1 is wear, P1 is tool 1, P2 tool 2, etc.

L2 is work coordinate, P2 is G54, P3 is G55, etc.

L 10 is geometry, P1 tool 1, etc

The actual values are identified by X, Y, for work coordinates (L2), R, for geometry or wear.

The best way to sort it out is as you are doing testing things on a machine and finding what is entered.