Centroid Community CNC Support Forum

Sirs,
I am having a threading issues that I need to resolve.
I am running a T39 Control with Centroid SEM 40 servos.
1.) The first issue is I am currently running a 1 1/8-12 OD thread in Steel with a single point carbide insert tool. RPM's 300. Programed with Intercon and using the provided thread information.
Report, Picture and program are attached.
The thread visibly looks good. When I check the pitch with a thread pitch gage it looks closer to the 11 1/2 pitch than is does the 12 for the full length of the thread. The thread runs 1.5" in length and I am starting it at +.200 before the end of the stock. Needless to say the nut will start for about 2 turns and then gets tight. The first thread I ran was a custom pitch metric in aluminum and I had to really work with the pitch to get the pitch to be right as well. Recently I ran a NPT in PVC and it is off too. I have double checked the Z axis for accuracy and it is within about .002" in 6 inches at the current threading location on the lathe travel and it repeats. I do not believe that I have an spindle encoder issue, because I can run the same program several times on the same part and it does not cut additional material on the extra runs. Is there a threading correction factor in the set up?
2.) The single point carbide threading tool needs to run about -.025" to get to a reasonable looking thread depth, otherwise the thread looks flat on the top. I usually run my part O.D. about .005" under size for threading. I used to run a Prototrak lathe and it ran the same way. They told me that it was the style of cutter I was using. If so is there an explanation for this.
I have a larger treading job coming up and need to get this fixed.
Thank you,
Tim

What are the chances your spindle encoder actually has 1024 lines (4096 counts), instead of the 1000 lines (4000 counts) you have entered in Parameter 34?

That would give you a uniform scaling error, where all spindle-slaved moves (such as threading) go 1.024x as far and as fast as they should, per spindle revolution.

Sir,
You are right! I adjusted the encoder count to 4096 and the 12 tpi is perfect.
Is there an explanation for the need to set the tool offset to negative value? I set it for -.017" on this thread and got a really nice fit.
Thank you for your help and the quick response!
Tim

You needed a negative offset because you were cutting with a sharp-V cutter. The minor diameter in the thread database assumes the correct thread form cutter for that thread and that includes the tip flat/radius.

Tom,
Thank you for the response and the information. I knew there had to be a reason.
Thank you,
Tim