Fanu 0i MD VMC work coord & tool lengths 'philosophy'

[bspear]

Fanuc 0i MD


My first time on a Fanuc mill after Heidenhain, spent a couple of hours trying to get my head 'round the work shift and tool length setting and need to get a definitive on what trumps what and what needs to be initially zero'ed or reset to avoid offsets on offsets etc.


Once a code is run and g43's and g54 etc are called I presume the last one called remains active if I switch to any manual movement?


Are there any codes I need to watch for at the end of progs which clear work/tool offsets?


Before I set a work shift, how do I ensure no other workshifts are active, should I call that workshift first in MDI? will reffing all axis clear the workshifts? G53 or a manual ref?


Before I set a work shift, I presume I need to activate a zero tool length?
Or again can I clear the active tool H?


Any suggested workflows gratefully received.


BTW, I'm manually setting - no electronic gizmos. Because of the safeties and switches on the machine side the workflow is a bit long winded so was going to make up my own BT40 tool gauge for measuring tool lengths but couldn't see any ref to DIY gauges on line, see any reason why not?


Cheers, bspear

Similar Threads:

• Newbie- want to write to work coord systems from within the program G10? Help
• Need Help!- Tool measuring probe return 10mm difference in X and z lengths of tool
• Confused about setting up tool lengths
• Need Help!- Setting tool lengths.
• Coord rotation and multiple coord systems

[generaldisarray]

if using regular G54- and G43 -41-42 they dont stack. if you call G54 and then G55 it doesnt add to the first one.Its absolute. so long as your in absolute G90.
At the end of an operation and before a tool change, different MTBs do it different ways. you will just have to find out how your machine wants it.
Most are ok with just a
G0 Zx
G91 G28 Z0.
to cancel active tool length and go home

You dont typically ever cancel an active Work offset by calling G53. Unless you have a specific need I guess. Like a part change position at the end of a cycle that
G91 G28 X0. Y0.
wouldnt get you.
But I typically would either stay in the current coordinate system and just give it the Xx Yx of where I want it to end up.Or call a new coordinate system with those numbers in the register so The program would read.
G0 G90 G5x X0. Y0.
That way that part change position would persist and I could speed programming. It was only an issue on one machine that had a funky setup that g28 x0y0 would make the slides stroke full range - then + and still not be centered in the operators door.

Its really not that complicated.

[generaldisarray]

I thought I should answer your questions directly, instead of rambling

Fanuc 0i MD


My first time on a Fanuc mill after Heidenhain, spent a couple of hours trying to get my head 'round the work shift and tool length setting and need to get a definitive on what trumps what and what needs to be initially zero'ed or reset to avoid offsets on offsets etc.

initially, the machine must be zeroed. but I think an Oi D is absolute, right? Powers up referenced?


Once a code is run and g43's and g54 etc are called I presume the last one called remains active if I switch to any manual movement?

Usually. Unless you press reset. Usually


Are there any codes I need to watch for at the end of progs which clear work/tool offsets?

No, you dont have to cancel tool length at the end of an operation. Ref return to home has always worked for me. Robodrills are the only machine I have ever seen that require something close to that. They require a G49 immediately prior to a tool change, Even if they are on Z ref position.


Before I set a work shift, how do I ensure no other workshifts are active, should I call that workshift first in MDI? will reffing all axis clear the workshifts? G53 or a manual ref?

Just make sure you are using the Machine position registers as the source for your values. If the machine supports a measurement function, it will most likely be using the proper values


Before I set a work shift, I presume I need to activate a zero tool length?
Or again can I clear the active tool H?

You dont necessarily HAVE to use a Z value in you work offsets. It depends on how you want to run it.(work shift is an inaccurate term, as other Fanuc controls have a actual work shift)
If you are doing a simple one tool job, there is no need to go through any more work that just touching-off your tool on top of you part, with a slip of paper. Leaving you work offset Z at zero.

If you have an entire magazine of tools that you use on multiple different jobs, Then you should be setting them either to the table and using the Z offset to move the ref surf UP to the part Z origin
Or
Setting them off of the gage line or some thing like that and using the Z offset to move the Z ref surface DOWN to the part origin

To distill that a little. The Z work offset register is the DELTA from where the TOOL is referenced to where the PART is referenced.


Any suggested workflows gratefully received.


BTW, I'm manually setting - no electronic gizmos. Because of the safeties and switches on the machine side the workflow is a bit long winded so was going to make up my own BT40 tool gauge for measuring tool lengths but couldn't see any ref to DIY gauges on line, see any reason why not?


Cheers, bspear

[bspear]

if using regular G54- and G43 -41-42 they dont stack. if you call G54 and then G55 it doesnt add to the first one.Its absolute. so long as your in absolute G90.
At the end of an operation and before a tool change, different MTBs do it different ways. you will just have to find out how your machine wants it.
Most are ok with just a
G0 Zx
G91 G28 Z0.
to cancel active tool length and go home

You dont typically ever cancel an active Work offset by calling G53. Unless you have a specific need I guess. Like a part change position at the end of a cycle that
G91 G28 X0. Y0.
wouldnt get you.
But I typically would either stay in the current coordinate system and just give it the Xx Yx of where I want it to end up.Or call a new coordinate system with those numbers in the register so The program would read.
G0 G90 G5x X0. Y0.
That way that part change position would persist and I could speed programming. It was only an issue on one machine that had a funky setup that g28 x0y0 would make the slides stroke full range - then + and still not be centered in the operators door.

Its really not that complicated.

Cheers, I understand the offsets wouldn't stack but it was more about avoiding setting one whilst another is active particularly on the 43s - does g49 work OK on the 0i md?

Sent from my SM-A300FU using Tapatalk

[generaldisarray]

Like I said. I have only ever seen G49 required on one machine, ever. Robodrills.

If you think about it. Why would you want to ever not have an active tool length offset. When you are not at Z home position? That is inviting a crash.

Your first move away from Z home should be with G43. When you finish a operation it will be with G28 Z0, cancelling your tool length offset.