Lathe Tool Offsets How To?

[Cartierusm]

So I understand tool offsets are very important in lathe work. I have all indexable tooling so it shouldn't be too hard, but I'm not sure how to do it. This is the idea I have of how it will work. I take my most common tool make a skim cut and a face cut, zero out the Mach3 DROs, that will be 0,0 minus the radius of the tip of the tool, then take the next tool holder and tool, then slide the tool until the tip touches the skim cut (diameter of the work piece) and that would also be X0, the move the carriage until the tip of the tool touches the face of the work pieces and then use what the DRO says as the Z offset. Continue to do this for all tooling and enter the values into my program.

Is that the way it should be done or is there an easier and/or more accurate way? Thanks.

Similar Threads:

• Lathe Tool Offsets
• CNC lathe tool and work offsets
• Newbie- Origin and tool offsets Lathe
• CNC Lathe Tool Offsets, just a few questions...
• Question on setting up lathe tool offsets

[arobustus]

That sounds about right. Except that when you teach the diameter it's not "X zero", it's the diameter. Oh and don't subtract the tool radii unless you are going to add them back in with the program. Some people use the longest tool to create Z Zero, for the sake of safety. Just take care when you first start the program. Turn the overrides (I'm assuming it has them) down to zero & ease into it. You will know very soon if you have done it right.
There is no more accurate way. There are some easier ways but they generally involve special equipment that you did not mention.
-plh

[LeeWay]

I have hand coded all my main parts that I turn. I do use 3 tools on most of these. I do use gang tooling. One is the center drill, then a drill and then either a parting tool or modified boring bar. Both the last two are mounted in a QCTP.

I cut brass and plastics. When I first setup this lathe to do this, I found the best way for me to hit 0,0 was to use the cutoff tool bumped to the edge or corner of my typical 9/16" brass stock. Then manually I jogged to the center for the center drill and then the drill bit. Once I fond these X and Z distances, they remained a constant on all my parts. The Z changes depending on what I am turning, but the offsets originally hand coded are always the same.
The exception is when I use the boring bar in 1.25" dia. plastic. It still keeps the same X0 as the 9/16" brass rod, but then I hand coded the BB position. The other two tools remained the same.

I now have Dolphin turn and will need to change things up a bit to turn other things using it. I will, however make a single plate that holds all my original tools in the same location. Then I just swap out this tooling plates wen I want to run production. Should make it all kinda quick change.

At that point, I will really need to know how to set the offsets. Thanks for the thread. I was going to start one like this myself eventually.

Here is an older video of my lathe. It's about twice as fast as this now with even better results.

"http://www.youtube.com/watch?v=aprdDeekio8&feature=channel_page"]YouTube - Home Made CNC Lathe

[Gmaan]

The way I do it is this:
touch on the diameter of the stock or take a light cut(better to cut)
Measure the cut diameter
set your tool dia offset to this value then subtract either the diameter or radius of the cut part to modify the previous measured value. This will set your tool to the proper value to cut any diameter you require.
I measure all my "Z" lengths from the face of the chuck with a 1-2-3 block and set the tool "Z" value there.
I shift my work offset "z" register what ever distance my stock is from the 1-2-3 block.
I use this method so I can set tools and use them for any job on the machine. I just need to shift my "Z" value in the work offset register as required.
I can set tools and use them for many different parts. In all cases my tools are measured and set from the machine home position to the face of the 1-2-3 block and c/l of the spindle.

[Cartierusm]

arobustus, I'm a little confused, In Dolphin when I'm first setting up a tool in Dolphin tooltable, when I enter a value for radius (let's say .0156") it automatically enters values for Z and X offset, so for Z it puts .0156" and for X it puts -.0156". Is this correct and I should just leave it?

Leeway, nice job on the custom lathe. I was thinking of doing the same if this little lathe I bought doesn't work out. How in the world did you manage to setup the drill bit exactly center, must have taken forever to make sure it was square, parallel and in the center. Kudos.

[LeeWay]

Leeway, nice job on the custom lathe. I was thinking of doing the same if this little lathe I bought doesn't work out. How in the world did you manage to setup the drill bit exactly center, must have taken forever to make sure it was square, parallel and in the center. Kudos.

That part was actually rather easy. I installed the drill bit in the spindle and then bored the tool holder with it. It could not help but be centered.

[olddaphon]

That part was actually rather easy. I installed the drill bit in the spindle and then bored the tool holder with it. It could not help but be centered.

thst is a sweet idea for setting the center, thank you for that.

[Cartierusm]

No kidding, duh, thanks, once you mention it LOL.

[dschedler]

What is the most accurate way to find your X offset for drills and taps on a gang tool lathe?

[g-codeguy]

What is the most accurate way to find your X offset for drills and taps on a gang tool lathe?

With the correct size material for the holder mounted in the collet. Or...Hardinge Brothers has a 1 inch bar with a .625 diameter in the front followed by a .750 diameter. Anyone with a CHNC should have this bar or you can order one directly from Hardinge. This is the most accurate way if you indicate the bar for run out before bringing the holder onto the bar.

[dschedler]

With the correct size material for the holder mounted in the collet. Or...Hardinge Brothers has a 1 inch bar with a .625 diameter in the front followed by a .750 diameter. Anyone with a CHNC should have this bar or you can order one directly from Hardinge. This is the most accurate way if you indicate the bar for run out before bringing the holder onto the bar.

I currently use the correct size stock for the holder mounted in the collet as you described. I didn't know Hardinge made that I'll have to look into it. What about a floating tap holder? When I use this method, there is no way I can think of to compensate for the play in the holder. In other words, how do I know the holder is centered in it's "range of float" (if that's even a term lol).

[LeeWay]

Not the best way, but trial and error works without any setup tools. Just about anything you do extra after that is geared toward better accuracy.

[g-codeguy]

I currently use the correct size stock for the holder mounted in the collet as you described. I didn't know Hardinge made that I'll have to look into it. What about a floating tap holder? When I use this method, there is no way I can think of to compensate for the play in the holder. In other words, how do I know the holder is centered in it's "range of float" (if that's even a term lol).

Set the work holder that the floating holder is going to be mounted in the way you normally would for a drill. I don't know what kind of floating holder you are using. We have a few adjustable holders for this type of machine. Next mount the tool. You shouldn't have moved the turret after lining up the work holder with the bar. (Or simply move it back to X0 for that tool.) Then indicate the tapered angle on the tap collet for zero runout, and then snug it down. Double check to see it didn't move. This is for an adjustable holder such as we use.

I purchased a very nice floating holder several years ago. It has never seen any service as it is too long for the machines we have with the exception of the SL-35 and possibly the 51 Conquest. There is no adjustment to the head on this tool. Set the work holder on zero like for a drill, mount the floating holder, and go to work.

[dschedler]

Set the work holder that the floating holder is going to be mounted in the way you normally would for a drill. I don't know what kind of floating holder you are using. We have a few adjustable holders for this type of machine. Next mount the tool. You shouldn't have moved the turret after lining up the work holder with the bar. (Or simply move it back to X0 for that tool.) Then indicate the tapered angle on the tap collet for zero runout, and then snug it down. Double check to see it didn't move. This is for an adjustable holder such as we use.

I purchased a very nice floating holder several years ago. It has never seen any service as it is too long for the machines we have with the exception of the SL-35 and possibly the 51 Conquest. There is no adjustment to the head on this tool. Set the work holder on zero like for a drill, mount the floating holder, and go to work.

The tap holder I have bolts directly to the slide, and is one unit. I can take it apart, but the through hole is a double-d. I'm thinking that this holder is a POS and can only be lined up by eye....which sucks!!!

[isaacvargas]

please. please friend. help me.
I want to setup or configure mach3 to work with gang tooling.. please friend.

please help me. I want to work with gang tooling..

thanks a lot friend.

have a nice day. leeway.

fabatecperu@gmail.com