[Ovrclck350]

Hello all,
I've been browsing this forum for a year or so now and finally decided to join up. I look forward to picking your brains and maybe helping out some myself.


I currently am having an issue with thread milling. I'm running some smaller parts out of Nitronic 60 and after lots of frustration breaking taps while tapping from the back spindle , I decided to switch over to thread milling. This particular tapped hole is also a zero chamfer hole, so I know that was a bit of my problem. I know there's probably a few different ways on this machine to do so (I do have the live 30-tooling option).

Currently I'm using this approach for a 1/4-28 thread mill with a .180 diameter.

[Live tooling on=2847RPM]
G0 X0.0
G1 Z.350 F10.0 [IPM]
G1 X[.036*2] F1.0 (FEED INTO shoulder for .251 major diameter)
W[-[.03571*2]] H[-[360*2]] F1966.0
G0X0.0
Z-.1

It's working, but the tool life isn't what I've been expecting. I actually added a roughing pass instead of just going full depth for my pass, but every once in a while the mill will snap. It will do so right before it completes it's first full 360-degree rotation.

I've seen someone mention using G32, but I'm a bit reluctant to do so primarily because I envision it stressing the tip of the tool and deflecting off-center as it tries to feed straight in. Also, I'm not sure that my spindle will let me program a 4-5RPM rotation.

I have some smaller shanked mills coming in tomorrow and I believe my next attempt will be similar to:

G0 X0.0
G1 Z.350 F10.0 [IPM]
X[.036*2]W-.03571H-360.0 ~F1000.0
W[-[.03571*2]] H[-[360*2]] F1966.0
G0X0.0
Z-.1

I assume that giving it a full lead to shoulder into the part may help it seat a bit better.

In any case, does anyone have any tips or tricks to thread milling with the back spindle? Would G32 or G92 be of any use at all? I know that G12.1 programming is an option, but I have used very little G12.1 programming, although I did manage to write an ellipse sub program to mill an adjustable ellipse on the back side of a part. I wish I could just do a true helix into the shoulder as I would on a mill but I'm hesitant to try it until I understand the G12.1 programming a bit more. If it's as simple as throwing the code in, and spitting out mill-style G2/G3's then I'm all for it. I just worry because my X is in Diameter and I'm not sure how that affects anything.

Thanks in advance. I have another issue regarding interpolation I'll address in a seperate thread tomorrow when I have more time.

[MikeMc]

In G12.1 the machine takes straight mill cammands. So you can lay the part out in your CAM software (or long hand), plug it into the machine, and under G12.1 it thinks its a mill.

I've never tried to thread mill with the L-20, the guys at Citizen told me I couldn't, but then, they told me I couldn't do a lot of things I have done with these machines.

[glenthemann]

is there any reason youre not using a single point threading tool such as a micro100 and G76?

[MikeMc]

Since he mentioned breaking taps, I assumed the thread is an ID thread.

[Ovrclck350]

Yes, I failed to mention, it is an ID thread.

So can a G76, G32, or G92 be used setting up at X0, but INSIDE the part and set to come out of the part? As long as I set it up at X0, will I run into an issue where it tries to clearance too much and hit the opposite shoulder? Remember, I'm using a .180 diameter thread mill inside a .213 hole.

Mike, I take that to mean that the machine will not need the X-dimensions doubled then (when I'm in 12.1 mode)? Going to X-.125 would take me to a .250 diameter circle as opposed to having to program to go to X-.250?

[glenthemann]

Is it a blind hole? how much of a lead out must you have? we do id threading the way I described, but there are a bunch of circumstances.

In G12.1 the center of the face of the material is your x0.y0. plug in your values as you would on a mill. I personally havnt used this and I dont know if you can feed in z as well at the same time for helical enterpolation. But I dont see why not.. then again.

[Ovrclck350]

Zero lead out. It's a Zero Chamfer, zero taper straight 1/4-28 hole .350 deep. It mills into a hole that has an ellipse milled through it (like a cross hole, only it's an ellipse). Our taps would break and alarm out, even with G84 tapping to depth, after just a few parts. We actually found a tap that would work...at least for a while, but it deforms the ellipse a bit as it bites through the hole. Normally we could live with that, but this particular ellipse has is .238 x .177 and has a .05mm tolerance in both major and minor diameter directions. It's hard enough to actually mill consistently with such a small endmill (.125 is the max due to the corner radius) due to wear, etc that with the addition of the tap deforming it thread milling was a much better solution.

And it's working...it's just that it's not seeming to like feeding into the shoulder at .350 depth. I switched mills and am going to try helixing into the shoulder over a 1.25 thread lead. Then I'll go back to start and helix into full diameter over a 1/2 thread lead. Hopefully that will solve my problem.


As for the G12.1 programming, I only ask because if I recall correctly I had an issue with another part on the back end. It's the piece that slides into the above mentioned ellipse, so it's a rod with an ellipse on the back. If I do remember, I had to actually alter my sub-program to double all my X dimensions yet keep the Y dimensions the same, which is the opposite of my sub-program that mills it from the live tooling on the main tool rack (where I had to double Y for diameter). So I'm just curious if the X-dimensions would need to be doubled. I've had a problem with this machine before milling a circle from the top of the part. I've meant to post about it...but if I set the circle up in Z, the hole comes out oblong. If I set it up in Y, it comes out perfect.

As for the ellipse sub-program, I'm pretty proud of it. One command line in the program after "setting up" the tool and you can not only adjust the size and position, but also adjust for overall tool wear and individual axis wear. It'll cut any ellipse, any size, with any endmill and has adjustable roughing/finishing axis steps, adjustable depth steps, adjustable roughing and finishing feeds. With just a few X/Y/Z swaps, it'd be useful on a mill as well.

Is it a blind hole? how much of a lead out must you have? we do id threading the way I described, but there are a bunch of circumstances.

In G12.1 the center of the face of the material is your x0.y0. plug in your values as you would on a mill. I personally havnt used this and I dont know if you can feed in z as well at the same time for helical enterpolation. But I dont see why not.. then again.