| | |
Hello.
Machine is mori seiki sh 5000 with fanuc MSG 501.
Here's the deal, i wonder if this is possible...
Machine running 4 different jobs, some with same tools, different people programming of course.
In some of the programs lets say tool T23 needs tool lenght (H) added with 0.10 (mm) in next job it needs to be -0.10..and so on..( meaby in third job it needs to be 0.15...)
Needles to say, much hassle.
Ofcourse im aware i could have several H codes, but that could cause problems later on when running the program again.
So is there any extra code that could be used just in program that could give you possibility to alter the tool lenght?
I've no idea what a Fanuc MSG 501 control is but on the controls I use, I would adjust the different tool lengths with the wear offset.
In the prog use G10.
In prog one...
G10 L11 P23 R0.1
In next prog...
G10 L11 P23 R-0.1
In next prog...
G10 L11 P23 R0.15
G10 = parameter setting
L11 = wear offset (on newer control use L13)
P23 = corresponding offset number
R0.1 = amount of wear adjustment.
Used to be G45, G46, G47 and G48 would increase/decrease moves by an offset amount. Don't recall if it was usable in G41 or G42, though.
G45 - single increase
G46 - single decrease
G47 - double increase
G48 - double decrease
These were used in place of cutter compensation a long time ago.
If you have custom macro A or B check your manual for macro variables in the 2000-3999 range, or 10001-19999 range. These allow just setting #2123=-0.1
This is the same as ChattaMan described, just a different way to code it.
Why not set the tools to a common standard and use the G54, G55, G56, etc. Z offset?
Hi.Originally Posted by ChattaMan
Very good, exactly what i was looking for.
I will try this on monday and see if it works.
Thanks alot!
ChattaMan;Hi.
Very good, exactly what i was looking for.
I will try this on monday and see if it works.
Thanks alot!
I'd like to ask one more thing.
The line with "G10 L11 P23 R0.1"
Where should i place this?
Lets say line like this after tool change.
"G43 Z10 H23"
Do i put the "G10 L11 P23 R0.1" before or after, or where should it be placed to work?
Oh and I believe if you use G91 with the G10 thing, you adjust incrementally, and G90 replaces the value absolutely.
you need to put the line G10 L11 P23 R0.1 before calling tool length compensation(G43 Hxx)
Yes before, But possibly you will need to inhibit the read ahead buffer as well. I think 4 lines are standard, and optionally it will read something like 15 lines.
Anyhow if you think it isn't working, look for a buffer inhibit G or M code in your manual and put that between the G10 line and the one with G43. It may be overly cautions for the G10, but definitely consider doing this if you use the Macro variable.
As Coupar mentions and points to.... Why bother?
Just set a tool length on the offset page and use work offsets (G54-G59) to control the zero point. No need to G10 anything....Machine running 4 different jobs, some with same tools, different people programming of course.
In some of the programs lets say tool T23 needs tool lenght (H) added with 0.10 (mm) in next job it needs to be -0.10..and so on..( meaby in third job it needs to be 0.15...)
Needles to say, much hassle.
It's just a part..... cutter still goes round and round....
Not specific to this problem, but there are others that would solved via changing offset wear via code in the program.
It may be more than 1 tool per program, and not in the same direction and amount. Or radius offsets, differing cutting conditions could require different offsets between parts of features.
Another possibility is a rotary table. Fixture offsets often do not rotate with the part. So either offset the tool, or use several fixture offsets with translated axis values.
Posting Permissions
| | |
LinkBack URL
About LinkBacks
