[mavruk]

Hello,

I ran into a program the other day on a Doosan VMC with a FANUC 0i controller That helically interpolated a hole. It compensated for the diameter programmatically (the diameter offset was set to zero). I've seen this when using CAM software but never when using Manual G-code entry (which is what this shop uses) I have two questions about this.

1. If you don't use the diameter offset can you still use the wear offset? seems like you would get something with a negative diameter if you tried. Wouldn't that cause an error?
2. Why would someone do this rather than just program it at the right diameter and use G41/G42?

I apologize if this is a silly question.

Thanks for your time.

[Superman]

Hello,

I ran into a program the other day on a Doosan VMC with a FANUC 0i controller That helically interpolated a hole. It compensated for the diameter programmatically (the diameter offset was set to zero). I've seen this when using CAM software but never when using Manual G-code entry (which is what this shop uses) I have two questions about this.

1. If you don't use the diameter offset can you still use the wear offset? seems like you would get something with a negative diameter if you tried. Wouldn't that cause an error?
2. Why would someone do this rather than just program it at the right diameter and use G41/G42?

I apologize if this is a silly question.

No...not silly at all

If you are in a shop that does small jobbing runs, setups & tools change often, & so on
- less chance of stuffing a part when D offsets are set to zero.

Normally, a CAM system, when clearing areas, creates a toolpath that is NOT using any compensation, the path is kept away from the edge by the tool diameter ( plus any additional allowance se by the programmer )
- the only requirement is the tool MUST BE the same diameter ( or smaller ( if smaller, there will be other obvious issues ))

If contouring, using WEAR comp, the D offset is set to zero if the cutting tool is the same diameter as programmed
- a negative offset makes the tool cut CLOSER TO the profile
- a positive make the cutter run FURTHER AWAY from the profile, similar to a roughing allowance

There are rules that still need to be followed,
- wear offset is for the use of a small adjustment range....ie using a 3/4" cutter in place of a 1" is possible, but the cutting parameters (speed / feeds / DOC / stepover) would need changing..... ideally it would be good for using regrinds
- lead in/outs must be longer than any value placed in the D offset ( on most machines, it is on a linear move )
- any radii ( on the profiles ) cannot be turned negative with the use of a large D offset value....ie an inside rad of 0.010" and you use a D+0.020....it would eliminate the rad creating a compensation error )

[mavruk]

Thank you for the your help with this. I just have one follow up question. I was under the impression that when the controller calculated the tool diameter for G41/G42 it simply took the value from the diameter offset and the wear offset and added them together. So if you had a zero in diameter and a -.005 in wear, you would end up with a -.005 diameter (which seems like it might cause problems) Is this not how G41/G42 work?

[Superman]

Thank you for the your help with this. I just have one follow up question. I was under the impression that when the controller calculated the tool diameter for G41/G42 it simply took the value from the diameter offset and the wear offset and added them together. So if you had a zero in diameter and a -.005 in wear, you would end up with a -.005 diameter (which seems like it might cause problems) Is this not how G41/G42 work?

For your example, you are correct in that instance that -0.005 offset would be applied to that path.....the toolpath would be adjusted 5 thou to the right(G41) or left (G42) of the programmed path, you may be using a cutter that is 0.010" undersize, compared to what was originally programmed to be used ( some controls use diameter input, some use radius....so adjust this thought to suit your control )

Standard usage of comp
G41 when using a +ive offset makes the path adjust to the left of the "zero" path ( ie further away when "climb cutting"), a -ive value makes the adjustment to the right
G42 when using a +ive value makes the path adjust to the right of the "zero" path ( ie further away when "conventional cutting")....It really depends on how the path is programmed, to suit the part/tool etc

...I do prefer the radius input for a mill, as you are not always machining holes, nor are you just in the XY plane )

The Oi control has one set each of Geometry & Wear offsets....and, yes, they do ADD the mating offset together to give a total offset.......personally, I avoid using the Wear page, so I have to only adjust settings on the Geometry page
- the danger with this is that the length and diameter values are intermingled, so a procedure needs to be created & rigorously followed.

On our Hardinge, I use a tool # that uses the same number for the holding the tool length offset, and a diameter # that is 30 higher than the # for the tool...... ( you may wish to make it on the same field position, but 2 pages higher )
ie T10, length is G#10 (program calls a G43 H10 ), Diameter/Radius is G#40 ( program calls G41 D40 (or G42 D40 )) so for programming I'd be using T10, H10, D40 for that tool

Later controls have separate D & H fields for the same offset number, this is much better as the T# H# D# can all be on the same line.

[mavruk]

Thank you for clearing that up for me. So you can still use wear offsets both + and - when radius offset is set to zero.