Need help with lathe threading

Actually its hard to tell because at 400 RPM = 400 Hz (and the equivalent 1.25 ms pulse widths) halscopes 1 ms sample time will likely lose pulses unless they were perfect 50% duty cycle (which they are not with real encoders)

The first image (~333 RPM) does have exact 60 pulses per index

I'll be happy if I could thread somewhere between 200-300RPM but it's cutting a finer pitch at those speeds.
What else can I try?
Could a PP cable be an issue?
Should I try moving phase A to another pin?

I've already tried 3 different PC's thinking latency was the problem.
But I'm using a vintage laptop with the best latency of the bunch @15k

What percent error do you show? The first Halscope plot at ~333 RPM
looked correct (exactly 60 pulses per index), maybe there is some other
issue (maybe with Z)

The encoder component should be able to work properly up to about
3000 RPM with you current 10KHz base thread.
Not sure if the BOB OPTOs will limit this further

PCW wrote:

What percent error do you show? The first Halscope plot at ~333 RPM
looked correct (exactly 60 pulses per index), maybe there is some other
issue (maybe with Z)

The encoder component should be able to work properly up to about
3000 RPM with you current 10KHz base thread.
Not sure if the BOB OPTOs will limit this further
 

Where should I be looking to see the error percentages?
I've never had any issues with Z, it moves exact distances according to my indicator.

What I mean by error percentages is:

What is the actual measured pitch error?

If you "thread air" and vary the spindle speed do you notice any
roughness in Z motion?  Because for the pitch to be too fine,
you would need to lose either encoder counts or perhaps Z axis steps
and both should be audible.

Note that you could possibly lose Z axis steps when threading and
not in normal motion because the Z axis "gearing" to the spindle
will result in a rougher than normal trajectory (especially with
a fairly low resolution encoder)

The pitch I'm trying to cut is 1.954 and what I get is 1.5 @200RPM

I just tried adjusting the spindle RPM while it was cutting air and there is no jumping or jerkiness or any weird noises.
Follows the spindle buttery smooth in the range of 0-150RPM

If I go past 150 it seem to follow at the same speed regardless if it's 200 or 400 RPM.

Is it possible that Z is limited in feeding speeds and simply can't keep up with the spindle RPM past 150?
Here is my Z setup

 

Yes, that could definitely be it, though I would have expected
a following error if the commanded position was so far ahead
of the actual position.

Are the following error limits set to large values?

I have my config files attached in my first post.
I'm not getting any errors on the screen.
Where should I look for error limits?

I'm probably wrong, you don't get a following error because
LinuxCNC bounds the geared commanded velocity to 5 mm/sec
even though that will only allow threading a 1.954 pitch thread
at about 153 RPM max...

So if you want to thread faster, you need more Z velocity

Thank you for your help PCW, I will play velocity numbers and post back tomorrow.
Hopefully with good news, fingers crossed!