What's new
What's new

Hardinge T42 Work Shift vs Work Offset Question (Fanuc 18T Control)

Nerdlinger

Stainless
Joined
Aug 10, 2013
Location
Chicago, IL
Hi Everyone!

Our 1990's Hardinge Conquests have all been programmed using G10P0Z____ to set work shifts. On these machines the negative Z value represents the distance from the face of the part to the spindle nose, so maybe something like G10P0Z-2". I believe the same applies to when the part gets handed over to the sub...the G10 value represents the distance from the back face of the part to the main spindle nose, so maybe something like G10P0Z-14". Anyways, a new programmer/setup person we have is pretty baffled by this and is dying to use G54 for the main and G55 for the sub. It "looks" like the machine can handle that as there ARE registers available for G54, G55, etc.

Honestly, I have never used G54 in a lathe so I am not sure how to think about it/test it out but does anyone know if those Hardinges can operate either way? Come to think of it...does it have to be either or can you actually use BOTH work shift AND G54 at the same time? Feel free to add in any personal preferences on the use of either.

Thank you for any help!
 
Use one or the other, not both. Bad things can happen if you use both together.

Personally I would never use G10 if work offsets (G54-G59) were available in a lathe.
 
I am sure that you have G54/55 available, and I use G10 P0 exclusively in all my lathes, but I would Shirley recommend NOT trying to use "both" for whatever reason that would come up.

I would expect that - to go to using G54/55 that you would need to cycle G10 P0 X0 Z0 in MDI, and then never use it again - or you would likely end up with "both" at some point, and that would likely give < positive results.

As a safety, it would seem wise to actually have a G10 P0 Z0 in your header on all programs in case you run a legacy program through it sometime.

Not sure what the new guy thinks is better about G54, but my guess it is related to using CADCAM in stead of FingerCAM?


----------------------

I am Ox and I approve this here program.
 
I’m still relatively new to the Fanuc thing. This maybe useless trivia but my miyano lathe which is quite a capable machine (Fanuc 21T controller) doesn’t have work offsets in spite of them being mentioned in the Fanuc 21t programming manual. I guess they’re not implemented by all builders.

So as a result I happily use the Ox method.
 
Personally I would never use G10 if work offsets (G54-G59) were available in a lathe.
G10 is a method of setting G54 - G59; it's not a substitute for setting those offsets. It depends on the arguments included with G10 in the Command Block as to the Offsets it sets.
This maybe useless trivia but my miyano lathe which is quite a capable machine (Fanuc 21T controller) doesn’t have work offsets in spite of them being mentioned in the Fanuc 21t programming manual. I guess they’re not implemented by all builders.
G54 - G59 Work Offsets are options that have to be paid for. Many MTB include them as if a standard feature, but if you dug deep enough, you would find a cost associated. Fanuc include all features available for the model control the manual is for, whether they are included with your particular machine's build of not.

The Work Shift that is available when the Control is not equipped with G54 - G59 is tantamount to G52 and when G54 - G59 is available, will be added to all offsets G54 - G59.

Regards,

Bill
 
G10 is a method of setting G54 - G59; it's not a substitute for setting those offsets. It depends on the arguments included with G10 in the Command Block as to the Offsets it sets.

I know what it is and what it does. I just prefer not to use it if work offsets are available.
 
I know what it is and what it does. I just prefer not to use it if work offsets are available.
It is not just a preference, rather a good programming habit.
There has to be a good reason why G54 etc were introduced.
 
G54,55, etc work offsets do seem to make more sense in a mill.

With my sub spindle it’s still pretty easy to keep track of things. With z=0 at the finished part face in the main spindle. To pull and part off let’s say the sub comes forward 11” to grab the part. Once pulling and parting are done and the sub returns home that part’s face is now at 11” and the finished rear end is at 11” minus part length.
 
I am sure that you have G54/55 available, and I use G10 P0 exclusively in all my lathes, but I would Shirley recommend NOT trying to use "both" for whatever reason that would come up.

I would expect that - to go to using G54/55 that you would need to cycle G10 P0 X0 Z0 in MDI, and then never use it again - or you would likely end up with "both" at some point, and that would likely give < positive results.

As a safety, it would seem wise to actually have a G10 P0 Z0 in your header on all programs in case you run a legacy program through it sometime.

Not sure what the new guy thinks is better about G54, but my guess it is related to using CADCAM in stead of FingerCAM?


----------------------

I am Ox and I approve this here program.
Thanks, Ox! We will try that. The G10 method is what is specifically called out in the manual and it never caused any problems for me but if switching to G54 will make him more comfy it doesn't bother me...as long as we are consistent, per your recommendation. I will post back if this works. Thank you, again!
 
Thanks, Ox! We will try that. The G10 method is what is specifically called out in the manual and it never caused any problems for me but if switching to G54 will make him more comfy it doesn't bother me...as long as we are consistent, per your recommendation. I will post back if this works. Thank you, again!


Actually, as was posted above (Bill maybe?) your guy can write to the G54/G55 with G10, in stead of writing to the Grid shift, and then he would need to call the G54 and G55 in the program as he goes. (Same thing only different is all)

One of the big benefits of useing Grid Shift IMO is that it is active at all times, even when you power up.
I rather doubt that G54 works that way - but I have never tried it on one of these machines?

On my mills - I want it to dump the offset when done (but it doesn't), and on my lathe - I want it to keep it active (for tool touch off and whatnot) and Grid Shift does that, and IDK if it does on G54 or not.

But with possibly mixing the two - between new and legacy programs, scares me.

I guess even if you have values in your G54's and your legacy program does NOT call G54, and if the control does NOT keep it after M2/M30, then you shouldn't have to worry about doubling up in that direction, but I would want to test that and see.


-------------------

Think Snow Eh!
Ox
 
So just to wrap this up, G54-59 offsets were an option back then. Some of our Hardinges have them and some don't. The ones that don't only have a single "work shift" register under offsets/settings - setting - w.shift (if I remember correctly.) Per above advice, it appears you can use either or even both but using both is asking for trouble. Thank you again for your help! :cheers:
 
using both is asking for trouble
G54 etc,. if available, are always there. Therefore, if workshift is being used, we are actually using both. Moreover, workshift uniformly applies to all of G54-G59, which one may not expect.
It is, therefore, best to avoid using workshift, if G54 etc are available.
 








 
Back
Top