Question on setting up lathe tool offsets

[SRT Mike]

Having never worked in a CNC shop before and learning as I go, I want to be sure I am doing this the right way.

Setting up a parting tool offset is giving my some trouble. I can determine the diameter quite easily of course but whats the normal method for getting the Z offset? I would *think* (could be wrong!) that since the parting bit is basically a rectangle you would want the corner point of the rectangle furthest from the chuck so you could accurately part off, say 1.234" of stock.

Do you guys just touch off on the front corner of the insert and the add on the width of the isnert? Or do you just use the front-ward corner of the insert and just add in the groove width when you do the parting operation in the G-code?

Basically I am doing some turning on a 1.5" piece of aluminum and I want to part of 0.916". I am using a parting holder with a 0.120" wide insert bit, just trying to figure the best way to setup the offset since adding 0.120 to the length I get from turning seems imprecise.

[toastydeath]

I don't know what anyone else does, but I set the Z offset of tool 1 to zero, and then either face off the part or touch it off with paper. Without moving Z, I set either the work shift or work coordinate system to Z0 at that location.

Then, I touch off every other tool with paper to the faced surface, and input the coordinates relative to the work offset.

That way, when you swap work offsets, change parts, or whatever, all your tools are still set up and ready to run. All you need to do is locate tool 1 (which ALWAYS stays at Z0) and set a new work coordinate system, or move the work shift. Bam, ready to go.

[SRT Mike]

Originally Posted by toastydeath I don't know what anyone else does, but I set the Z offset of tool 1 to zero, and then either face off the part or touch it off with paper. Without moving Z, I set either the work shift or work coordinate system to Z0 at that location. Then, I touch off every other tool with paper to the faced surface, and input the coordinates relative to the work offset. That way, when you swap work offsets, change parts, or whatever, all your tools are still set up and ready to run. All you need to do is locate tool 1 (which ALWAYS stays at Z0) and set a new work coordinate system, or move the work shift. Bam, ready to go.

Ok good - that's pretty much what I am doing right now - the only thing is if you do that with a parting tool, you will get the front of the tool, which won't account for the width of the groove the tool makes. So if you want to part off 1" of stock you would have to Z to 1.120" in the case of a 0.120" wide tool.

So is that what you would do or would you touch off the tool and then tack on 0.120" when you set the offset, so that if you went to Z -1.00 and parted off, you would get a 1" slug?

[Geof]

Originally Posted by SRT Mike ......So is that what you would do or would you touch off the tool and then tack on 0.120" when you set the offset, so that if you went to Z -1.00 and parted off, you would get a 1" slug?

This is my approach so that the length in the program is the length I part off.

[toastydeath]

I like setting my cutoff tools by grooving the part a little bit, and measuring the distance from the groove to the face. Then set Z<whatever you measured>.

That way, if I want a 1" slug, I face at Z0 and cut off at Z1.0. I try very hard to touch the tools off in the way they're going to be used.

[ctate2000]

There is no rule of thumb for this situation. I like to have the parting tool set so that the cut off length matches the length stated on the print. It makes trouble shooting the program easier when all dimensions in the program match those on the drawing. I would suggest you set Z zero by touching the face of the part then subtract the width of the parting tool from your offset. By subtract I mean to move the offset in the negative direction or towards the face of the chuck by the width of the tool. This is the way I like to do it. If the part is not the correct length just add or subtract the error from the offset. Remember when you cut off the tool can move during the process and cause length errors and make you think there is an offset problem.

CT

[Andre' B]

Or you can touch off just like your turning tool but program your cut off position like.

Z[-1.000 - #500]

Where the width of the cut off tool is in variable #500, so you still see your part length in the program and the operator can tweek tool width independant of the tool touch off.

[SRT Mike]

Thanks for the help guys - got it all set up and working like a charm (although not without slicing my fingers but good when I was putting a 3/4" drill into its collet holder!)

[Geof]

Originally Posted by SRT Mike Thanks for the help guys - got it all set up and working like a charm (although not without slicing my fingers but good when I was putting a 3/4" drill into its collet holder!)

Next time you will hold it with a piece of rag wrapped around it. Like I do so I do not duplicate the scar the goes 3/4 of the way around one of my fingers. And did you say 'oh bother' that was a silly thing to do?

[SRT Mike]

Originally Posted by Geof Next time you will hold it with a piece of rag wrapped around it. Like I do so I do not duplicate the scar the goes 3/4 of the way around one of my fingers. And did you say 'oh bother' that was a silly thing to do?

Well I certainly said something! Although there may have been a bit more color in it than "oh bother"

It was one of those nice slice cuts too - so every time I open my hand to grab something I feel the cut opening up. Its not that deep, just enough to bleed but I should know better. I have plenty of rags with blood spots on them around the lathe now, so that should help me remember next time!