NPT + Threads in Intercon - Workflow

[lavrgs]

I have just started investigating Intercon for the lathe and wanted to know a bit more about cutting NPT threads. For standard threads my workflow is FACE - TURN - THREADS. As I enter the threads I note the Major Diameter and go back to modify the turning op to match. With NPT threads I am not clear on how the workflow should go in relation to the taper. Any hints would be appreciated...

[cncsnw]

You could make your Turn cycle turn a taper. Assuming you are doing external threads, then for the final diameter, enter the major diameter you want at the large (Z-) end of the thread, and for the taper angle enter the half angle, as a negative number (-1.7899 degrees for NPT threads).

Parameters for the Threading cycle would then be similar.

[lavrgs]

I decided to start with a simpler test. Assume tool offsets are set correctly... My test gage is a nut - not ideal but I'm just experimenting. I need to learn to use thread wires...
I cut M6x1 threads and had the proper OD, per micrometer, but the nut did not fit. I adjusted tool wear, several times to end up at -0.012 to get the nut to fit. I then cut 1/4-20 threads and had to further adjust the tool wear for that thread. After I make a "good" thread I can repeatably make it again. My question is - should I need to adjust tool wear for each different thread? Maybe the question is do I adjust the tool offset instead of wear? I want to make a M3x0.5 but thought starting bigger would be easier. My expectation was that if I can reliably make one thread all the others should be able to be made

[tblough]

The Centroid minor diameters are only valid for threading tools with the correct root flat or radius. If you are using a sharp V threading tool, you'll have to subtract another 0.108 * pitch from the minor diameter.

You need to adjust the minor diameter in the thread details page and not the tool wear if using a sharp V tool. By adjusting tool wear, you are also affecting your actual tool position which also affects your major diameter and therefore your first cut depth.

[lavrgs]

I will assume the new threads can be saved for future use. I’m using an ER11 A60 insert that doesn’t make a full profile. What type of insert would be required to create the minor diameter as programmed. Thanks for the info on reducing minor diameter.

[lavrgs]

I went back and removed all wear from the tools, went through the tool setting process again and made sure I could cut the 1/4-20 and M6x1 threads I had set up in Intercon using modified minor dimeters. Then I tried cutting M3x0.5 - Maybe M3x0.50 is too small -I was breaking off the portion to be threaded. It seems like the Z offset was a problem as it was cutting past the turned down area, I went back and double checked that setting, tried to adjust the gcode without any luck. Maybe a die is the way to go...
The reason for cutting M3x0.50 is that I have a probe coming that has that thread and I want to make a stylus,,,to help measure tool offsets.
https://photos.app.goo.gl/ejsDDGGjdXhvsJeh9 Most of the way there...
https://youtu.be/ZjUAQYs9bP4?si=vGlrvfn5Klo7vI-2

[tblough]

I cut 0-80 and M1 all the time. You need an extremely sharp tool and very small infeeds. As for cutting into your shoulder, where are you setting your Z0 for the threading tool. If you use the point of the tool, you'll have to reduce the ending Z by 1/2 the width of the tool. I set my Z0 to the side of the tool so I can use the print dimension for ending Z. Even so, i still reduce it by a little.

Many people start threads by single pointing them and finish with a die. Starting them with a single point tool in the lathe ensures they are straight and concentric. The die sets the finish size.

[lavrgs]

As for cutting into your shoulder, where are you setting your Z0 for the threading tool.


Many people start threads by single pointing them and finish with a die.

I set Z offset at the spindle side. I will try taking a few passes and finishing with a die..
I've got other issues going on that are roadblocking my progress...

[lavrgs]

For my last try, I used Fusion to generate the tool path and upon closer inspection the default pitch and depth values were very far off and the containment was wrong, making the tool cut into the shoulder.
I'm currently having some X axis problems. When I get going again, I will try first with Intercon, then see if fusion can be adjusted.