Question about Wear Offsets

In our shop we mainly are not doing production work, and really only use our controllers for height offsets and zero pickups, any other changes we do in cad/cam.

My question is with wear offsets, i've seen them on controllers and want to know how they work.

Couple of questions.

Say i am using a .625 cutter, with it being on size, i leave the wear offset to zero. Say i want it to cut a 2d profile .010 oversize. Would i enter +.010 in the wear offset? or +.005? (do you enter the full amount or half?).

OR, what if you are using an undersize resharpened cutter and want it to still cut on size. Say the program is programmed with a .625 cutter, but the cutter is .615 (.010 undersize). Would i put a - or + wear tolerance of .010? The cutter is already a -.010, so i'm assuming i would enter a +.010 to 'fake' a .625 cutter?

I'm sure it's simple when practiced, but i've never used this featuer.

The amount is determined by your controller's setup.
Typically the offsets contain the diameter of the tool, and in that case the wear is also expressed as a diameter.
There is also a way to set your controller to radius ( less common but available ), which now uses the wear values as radius deviation.

So, assuming diameter values, if you want to cut your feature .01 oversize you'd want +.01 in your wear. Of course that means you're cutting the entire outline of the feature such as a diameter or full profile etc...

Ditto for resharps, you enter the actual deviation in the wear which is typically minus value.

That is assuming however the useage of cutter comp ( G41/42)

One last note, I have seen some Haas-s using negative offsets ( not workoffsets!!!, cutter offsets ) Why that is I do not know, but guessing at compatibility with some older systems. IOW a 5/8 cutter had a diameter value of -.625 in the diameter page. Obviously if that's what you use then the values remain the same but the signeage reverses.

SeymourDumore said:

One last note, I have seen some Haas-s using negative offsets ( not workoffsets!!!, cutter offsets ) Why that is I do not know, but guessing at compatibility with some older systems. IOW a 5/8 cutter had a diameter value of -.625 in the diameter page. Obviously if that's what you use then the values remain the same but the signeage reverses.

Click to expand...

I know about that one. Only bit me in the back side once but it was enough to make me remember it. The one thing is it can actually become a usefull tool but only in an extreme circumstance which I've only ever had once.

This also depends on whether your using part line programing (letting the operator select the cutter) of if your letting the cad/cam package figure the diameter. assume part line, you have to have a value in the geometry table then either shift your comp in geometry or wear. Now using pre determined cutter size the only place you can adjust from is in the wear page (no need to enter anything in geo unless its just operator preferance. adjusting wear is also going to depend on if the control is set for radius or diameter. I keep all mine set for diam since this leaves less chance for error. If you need .001 then adjust .oo1 radius would be if you need .001 then adjust .0005.

If you look in your tool offset page when entering in your tool dimensions it should say Radius or Diameter. This will tell you how much you need to adjust your wear. It will not always say this in the offset page. It's worth a look.

SeymourDumore is correct it usually depends on which way your control is set up. However most of the experience that I have had with using the wear offset is you have to look at the wear as a part of the tool. So if you have a .625 in your Geometry the machine works using .625 now if your wear is -.01 the Geometry and Wear add together to create .615 diameter thinking the tool is smaller it will cut a pocket larger with a ID profile and cut the part smaller with a OD profile.

This should be no different then using a wear in your Z offset. If your tool length/geometry is 7.0" and you have a -.05 in your wear the machine calculates the tool to be 6.95" long.

Stevo

So if i understand correctly, if my cutter is 10 thou undersize, i put in -.010 to the wear offset, and the controller knows the cutter is say .615.

Basically you start with your programmed size and what ever you put into the wear offset + or - it changes the control to that cutter size. So with a .625 cutter, if i had a wear offset of +.010 it would think it is .635 dia, and if i have -.010 it thinks it is .615?

I just have to get my head around that, because if i have a .615 cutter i think to myself "i have to add .010 to get it back to .625" and therefore would use a +.010 wear offset... but that is wrong? you use the wear offset to tell the control what the cutter dia IS

Do i have it?

You said it right in your second paragraph then contradicted yourself in the third paragraph. Adding .01” to your wear will add to your tool. Just think about the actual word “WEAR”. If your tool is running and it starts to wear you tell the machine in your wear offset that it has worn down .01”. Down is smaller, smaller is a negative #.

You should always put the actual diameter of the cutter in your geometry. Doesn’t matter if it is .615 or .635. Now program the proper dimensions. Now when you need to adjust as the tool wears -.01makes the tool smaller, +.01 makes the tool larger.

As I said earlier take your geometry and add the wear. Proper math will tell you were your tool is at.
.625 + -.01=.615dia.
.625 + +.01=.635dia.

I don’t know any other way to explain it. Hope this helps.

Good luck,
Stevo

thanks guys, think i've got it!