What's new
What's new

Threadmilling flange pattern on three axis lathe with basic live tool

Strostkovy

Titanium
Joined
Oct 29, 2017
Realistically the only live tool I can afford with a lathe is a subspindle that's fixed parallel to the main spindle and planar with the centerline of the main spindle. I'd only get C, X, and Z axes but that's fine for a lot of parts. Many parts in particular are essentially a flange with threaded holes around the perimeter, so I figured I could just thread mill by interpolating X and C to make a circular path (With a helix along Z). This would put the headstock in a gentle rocking motion under servo control.

However, while looking up examples of this I can't find anyone who has done it. Given it's rarity, do common cam tools support this type of operation?
 
Realistically the only live tool I can afford with a lathe is a subspindle that's fixed parallel to the main spindle and planar with the centerline of the main spindle. I'd only get C, X, and Z axes but that's fine for a lot of parts. Many parts in particular are essentially a flange with threaded holes around the perimeter, so I figured I could just thread mill by interpolating X and C to make a circular path (With a helix along Z). This would put the headstock in a gentle rocking motion under servo control.

However, while looking up examples of this I can't find anyone who has done it. Given it's rarity, do common cam tools support this type of operation?

Short answer, yes.

Longer answer, the only cam I've done this exact thing in is Featurecam, but it's totally supported there at least.

You need polar interpolation and helical interpolation on the lathe.
 
Short answer, yes.

Longer answer, the only cam I've done this exact thing in is Featurecam, but it's totally supported there at least.

You need polar interpolation and helical interpolation on the lathe.
Polar interpolation seems like the keyword I was missing.

If the lathe doesn't support it directly, can it be done strictly through G code? Or I guess a better question is, can any cam programs do the interpolation and just output a ton of G1 moves to approximate the toolpath?
 
Polar interpolation seems like the keyword I was missing.

If the lathe doesn't support it directly, can it be done strictly through G code? Or I guess a better question is, can any cam programs do the interpolation and just output a ton of G1 moves to approximate the toolpath?
This should be possible in featurecam, but I've never had to try. If I have time tomorrow I will look and see.

Polar interpolation is pretty much a given on any lathe that has a full c axis.

Helical interpolation is not so much of a guarantee, but if your cam can post threadmill paths as linear segments and you have polar, then it's an easy workaround.
 
This should be possible in featurecam, but I've never had to try. If I have time tomorrow I will look and see.

Polar interpolation is pretty much a given on any lathe that has a full c axis.

Helical interpolation is not so much of a guarantee, but if your cam can post threadmill paths as linear segments and you have polar, then it's an easy workaround.
Thank you for the information.

I'd really like to use those combined thread mill tools that also make their own hole, to avoid manual tool changes.
 
Thank you for the information.

I'd really like to use those combined thread mill tools that also make their own hole, to avoid manual tool changes.
Just checked, and yes, it's possible in featurecam to post code to threadmill axial holes even if you have neither polar interpolation or helical interpolation enabled on the machine.

Like I said before though, that would be an extremely rare combination on a live tool lathe.
 
The movements are certainly possible but accuracy and rigidity decrease substantially as you move further away from centerline. The resolution of a C-axis is .001 degrees regardless of whether your X is at .500 or 5.000.

My thoughts are that it's not going to be worth the effort, as you're not going to be able to dial in sizing on the threads. You're better off either using a Tapmatic or tapping them offline.

I once tried to mill a 24" square on a VTL with C-axis. The machine was rigid as hell, but the results were comical. The straightness of the edges were out by nearly half an inch.
 
The movements are certainly possible but accuracy and rigidity decrease substantially as you move further away from centerline. The resolution of a C-axis is .001 degrees regardless of whether your X is at .500 or 5.000.

My thoughts are that it's not going to be worth the effort, as you're not going to be able to dial in sizing on the threads. You're better off either using a Tapmatic or tapping them offline.

I once tried to mill a 24" square on a VTL with C-axis. The machine was rigid as hell, but the results were comical. The straightness of the edges were out by nearly half an inch.
That kind of gross error is much more to do with machine dynamics than it is to do with rotary axis resolution.

0.001deg resolves to a bidirectional uncertainty of 4 tenths of a thou at the corner of a 24" A/F square.

I did a lot of polar milling at ~150mm diameter with .001deg resolution in a 10" chuck Doosan and had no problems hitting +/- .05mm provided the tool was zeroed accurately in X-Y and the C axis torque was not pushed too hard, .02mm was perfectly possible with care (i.e. slowly and with a spring pass after the finish pass)

I also did a lot of polar milling at up to 400mm diameter with .0001deg resolution in the NTX and had absolutely zero problems with tolerances in that machine.
 








 
Back
Top