| | |
work shift when setting the work shift why is the distance from the tool to the turret added and then subtracted in the geometry offsets? Can't they both be "0"?
What machine and control are you using? What method do you use to touch off your tools? Do you use the work shift or G54?
The way I see it is that the G54 value is the distance from the spindle face to the part Z zero, and the tool geometry is the distance from the turret face and centerline to the tool tip (Mine is the Hardinge II+ with FANUC 10TF control)
Knowing the model, the control, and what it uses for the workshift (G54-G59 or G10), etc. would be a big help.
work shift A Hardinge 51 and 42. You touch off the end of the part go to work shift and zero out. Then you add the distance from the the tool to the turret face and you have a shift value. You then put the same value in the geometry offset. Don't you end up at the same spot if you don't add to the work shift and leave the geometry offset at zero? You then touch off the other tools to the end of the part you set their geometry offsets relative to the first tool.
work shift Oh by the way, the control is a fanuc 21 T.
Originally Posted by teamus
Are you using a probe? If not, then make your rough turning tool Z0. Who cares if the actual geometry is really .2487?Face, don't move the Z-axis, highlight the Z in the right hand column on the workshift page, type in Z0, INPUT. Touch off the rest of the tools. Done.
If using a probe, or you want the tool geometry to read what it should be, then do the above except type in the geometry of the tool instead of Z0. Say it was Z.2487. You'd type in Z.2487, INPUT. At least that is the way it works on our 18T and 21i-T controls.
All the Hardinges I've ever run used G10 for setting the workshift.
EDIT: Are either of these barfeed machines? All but one of ours are. I set the workshift for those in my program. It's easy to figure.
thanks G-code. How do you set work shift in the program?
G10P0Z-3.5
thanks again Dale
You're more than welcome. Will help anytime I can.
Work shift does not need to be used at all. If it is used, it's only used on the Z Axis.
Here is a good use of the workshift:
Running a chucking job and through the day you need to adjust for length control. You don't need to move the facing tool in. Just move the Z work shift in the minus for less stock removal and plus for more. This way you do a GRID SHIFT of the Absolute Coordinate System and all your tools move in/out the same amount. Don't try the novice method of wear offset times 6 tools in the Z to get this result. For some reason, it does not work.
NEVER MOVE THE X WORK SHIFT.
Also the Z work shift is great for running families of parts that only have a difference in the length. If there is enough of the stock sticking out, you just need to enter the amount of shift and make sure you maintain your clearances.
Don't use the Work Shift the way Hardinge tells you to. It's not needed at all.
If using a puller:
Cut off, leaving .250 sticking out of the collet/chuck
Pull to desired length
Face/Qualify/Rough Turn the diameter (this creates your Z0.0 for subsequent tools)
Touch off any remaining tools to this face.
Use wear offsets to dial in the part after taking .0005 face cuts with boring bars and such.
That's it. I run super precision parts like this all the time. Work shift is best used for length control. You do not need to use it at all in the program. Someone tell me where the benifit is in using it?
JT
You would screw yourself real quick if you started moving the X workshift.
Changing the workshift gives the same result.
Why doesn't it? What would be the difference between moving the workshift .006 and moving every tool by .006? However, I agree with you 100% on this. Dumb to stand there and offset 12 stations when making one change to the workshift is all that is needed. Definitely less chance of making a typing error.
See above comment.
Gee. It's been so long since I've looked at a manual for this type of thing that I haven't the foggiest idea how Hardinge manuals tell you to set the workshift.
Obviously you don't have probes (or ignore them). Some of our lathes have them, some don't. Almost all of our lathes are barfeeds. Let me see if I understand you correctly. A 3/4 inch 80 deg. profiling tool has an F value of 1.0. Using a probe would give you a Z-GEOM of .25 (give or take a few thousandths. As I understand it you are leaving the workshift at Z0 so your geometry is going to read in the inches...varying all over the place depending on the part length.
What do you do for the next job? Reset all your tools? Figure out the difference in Z between the last job and the current one, and then make a grid shift? If using new jaws, how do you take into consideration the difference on how deep the jaws were bored for this job versus the last one? How close are you after all this mathematical manipulation? Seems like it could get more complicated than necessary.
Okay here's the benefit. I determined after setting up the first job on one of our Daewoo Lynx lathes that I could use 6.8 for my constant. This leaves approximately 1/4 inch sticking out of the collet after cut-off. Now all I do is add 6.8 to my cut-off position (and round off to nearest .01).
We run lots of end washers. Usually make 5 per barstop. Do you want to trust your operators/set-up men to figure out where the last cut-off position will be, and then to extend the bar the correct amount before setting Z0? I don't. They never have to worry about setting a workshift because I do it for them in the program.
There is more than one way for them to set new tools once the Barstop Op has been run. One operator always figured .02 coming off the face and set the tool geometry accordingly. I prefer to MDI my rough turning tool to a known position, face and then set my new tools.
I don't set the workshift on chuck jobs. The set-up guy better be capable of that or he won't be working for us long. At least not as set-up man.
Now I am not saying your way isn't any good, or that it is wrong. Like my Pappy use to say, "There's more than one way to skin a cat."
However, I think I will stick with my way, unless you can show me where I erred in my thinking regarding how you make your adjustments from job to job. AND that it is easier and faster than my way.
EDIT: Sorry JT, but this is bugging me. Still racking my brain trying to figure out how you are going from job to job without having to re-touch all the tools. Arrrrrh. What am I not understanding?Please explain.
Last edited by g-codeguy; 05-05-2009 at 06:14 AM.
Posting Permissions
| | |
LinkBack URL
About LinkBacks
