Doug,
I have a Sherline lathe, so don't think I am bashing the product, don't use it much anymore though. Also just spent some time helping someone who was having some problems threading with his just last week. He cut 3/8-18 in 6061 AL.
So first i will make comments from experience with it.
The motor is wimpy even if you have the newer one on your lathe. You must have everything going for you, and by that I am mean razor sharp thread tool, properly set tool, all the gibs adjusted to remove play, preferably a backlash attachment mounted and adjusted, minimized overhang of the thread tool, and using the wizard to your advantage, the stock prepared by machining it to proper size ( concentric and not having say .003 runout.
24 tpi and below is reasonable to do, 18 can be iffy, 16 probably not ( but can be done if somewhat tricky about it, but the quality may be poor), forget about doing muti-start threads.
What is probably happening. The first few threads are ok and you are not getting much rpm change, but the rpm change will get progressively
worse as you cut deeper. Mach is constantly trying to provide for the rpm slowdown, but, it can only do so much. At one time one could actualy have the spindle almost stop and the thread cycle would try to fix things and the resulting thread was ,well lets say the the nut went on. The thread cycle was changed and slowdown of say 25% may mean a ruined / trashed thread. We did the 3/8-18 at 200 rpm, rpm change was around 30% max decrease for example. Thread didn't look bad but it was just a case of a poor quality thread. Yeah the nut when on!
Now besides the above, the axis just dosen't move as accurately as it should, so if you are off on a cut by say .002", that could be enough to cause an additional slow down of the spindle.
Rather than rambling I will say watch, know and learn what is happening very carefully monitoring the threading cycle and learn from it.
Also have a read of Threading on the Lathe-Mach 3Turn.
------------------------------------------------------------------------------
Here is what you can do that will help:
1. Don't use radial cutting and instead do flank cutting. use 15 degree instead of 30 degree in the settings.
2. Make sure you allow 3-5 min pitches before threading starts
3. Use finer cuts depths, maybe .004 to .007 for the first cut and then limit to .003 or .004 there after.
You can do even finer ....but depends on axis positioning accuracy
3. You can try alternate flank cutting but don't think the your Sherline is accurate enough, but it may avoid a plunge on some cuts.
4. Experiment with the material, brass will work harden for example.
5. I can say adjust the gibs to be on the tight side and well lubricated, but not kowing what size motors you have ...that could
cause skipping
6. If you have backlash you will never do accurate threading, backlash compensation can help but is not the answer, due to improper
tool location you will / may cut deeper than wanted and thus have reduced rpm during the cycle.
So don't get frustrated, you can do some nice work on the Sherline, but know it's capabilites and that only comes from
having fun playing with it.
Have fun,
RICH