[AUSTINMACHINING]

Well I knew (and was dreading the day) I would need a turned part. After a lot of reading threads about making a vertical mill, I designed/machined a tool fixture based on some lathe tools I bought off e-bay. Knowing absolutely nothing about lathe work, a lot of trial and error air cutting was in order. Had a hell of a time wrapping my head around work offsets/touching off lathe tools and lathe tool geometry. The part I need to make will be from 1" 6061 round bar, but I had some soft 3/8" scrap aluminum bar to test with. I still have a lot of tweaking and learning to do, but I think I've got the major stuff figured out. My test part came out .003" over in diameter, so need to adjust my offsets a tad. I'm touching off zero on the edge of the tool block and adjusting the work offsets using G52 between the different tool locations. Here's a video of my test part. It's 1" long with .25 and .353 diameters. Operations are facing,profiling and cut off.



Attachment 257886

[LeeWay]

That has to be the most nimble lathe spindle I have ever seen. Looks good. Looks like you have the hang of it.

[SCzEngrgGroup]

I've done quite a few parts that way but still don't enjoy it. Never have gotten around to making a fixture to hold the tools. Most of my "turned" parts I now make using a 3-jaw chuck held in a vise pointing straight up to hold the workpiece, and do all the cutting with milling tools.

About the easiest way to set the X offset is to make a cylindrical cut, then measure the workpiece with a micrometer, and set your offset to half the measured diameter.

Regards,
Ray L.

[LeeWay]

About the easiest way to set the X offset is to make a cylindrical cut, then measure the workpiece with a micrometer, and set your offset to half the measured diameter.

Regards,
Ray L.

That is the best way to do it on a lathe as well.

[AUSTINMACHINING]

I've done quite a few parts that way but still don't enjoy it. Never have gotten around to making a fixture to hold the tools. Most of my "turned" parts I now make using a 3-jaw chuck held in a vise pointing straight up to hold the workpiece, and do all the cutting with milling tools.

About the easiest way to set the X offset is to make a cylindrical cut, then measure the workpiece with a micrometer, and set your offset to half the measured diameter.

Regards,
Ray L.

Ah.., thanks. That will be a lot easier than trying to touch off with a probe.

[mklotz70]

I've done quite a few parts that way but still don't enjoy it. Never have gotten around to making a fixture to hold the tools. Most of my "turned" parts I now make using a 3-jaw chuck held in a vise pointing straight up to hold the workpiece, and do all the cutting with milling tools.

About the easiest way to set the X offset is to make a cylindrical cut, then measure the workpiece with a micrometer, and set your offset to half the measured diameter.

Regards,
Ray L.

I've thought about using this method (someday) on some of my parts........how accurate or concentric is this method. I use my manual lathe to open up the center hole on existing brake rotors to fit a different hub on another application. I've been wondering if interpolating (correct term?) the hole on the mill would be accurate enough.

[mklotz70]

Ah.., thanks. That will be a lot easier than trying to touch off with a probe.

Can the probe still be used to help find the Y? I've got a Hamier and I've been thinking that I could use it to find the Y axis center for each tool(whenever I start using the mill) I'm familiar with finding X from previous lathe work. Y is an added consideration when doing mill turning.

Do you use anything like MachStdMill to help with lathe work on the mill?

[kvom]

I've made a few parts like that. For centering in Y I use the same technique as on the manual lathe. I press a thin metal rule between the work and the tool and adjust Y until the rule appears to be straight in Y. Seems to be accurate enough that then adjusting radius by measurement after a skim cut will be within .001.

For zeroing Z I just do a face cut for each part and zero at that point.

I found that I had to use MachTurn to get my lathe g-code to work. The mill screenset had problems with G2/G3 for some reason.

[mklotz70]

kvom......Thanks!

[AUSTINMACHINING]

Can the probe still be used to help find the Y? I've got a Hamier and I've been thinking that I could use it to find the Y axis center for each tool(whenever I start using the mill) I'm familiar with finding X from previous lathe work. Y is an added consideration when doing mill turning.

Do you use anything like MachStdMill to help with lathe work on the mill?

I'm using a Hamier as well. Touching off the Y was easier than X but my lathe tools are the insert type that are "cupped" at the leading edge, so it's hard to get the sphere of the probe centered without it sliding off the cutting edge. Some good suggestions are mentioned here in other posts that I will be trying. I'm using HSMworks turning to generate the tool paths and some manual gcode to move offsets around for switching to different tools. I made my tool block fixture such that I can touch off the edge of tool block with all the lathe tool offsets relative to G54. I call G52 to move the offset around for the respective tools locations. This way, when I want to use the lathe tool block, I just drop it in the vise and touch off the tool block without having to redo all the individual tool offsets. To set my Z zero, I just put the stock in the chuck and get "eyeball" close to the tool block and I'm good to go. I'm using the generic fanuc turning post (slightly modified) to generate the gcoce to run in mach3 mill.

[mklotz70]

I was wondering about how hard it would be to touch off the "cupped" edge of an insert....since that's what I plan on using. I guess if you were going to put a shim on it to have a flat surface, you might as well use the ruler technique. Maybe if it was an electronic probe it might be easier.....that way you wouldn't be trying to overcome the spring pressure of the Hamier.
I don't know much about using the offsets.......so I'll probably have more questions later