Threading Question re 29.5 degrees -- Fixed

[briuz]

Hello,

When threading, on a manual lathe, it is a common practice to set the compound at 29.5 degrees and advance the compound into the thread. Does Centroid advance the tool at 29.5 degrees or is there a way to do this?


Edit to add: I just checked and the "Details" screen indicates the thread is a 60 degree thread. (I am trying to cut 1/4-20 threads.) Also, would my cutting the threads from z=-0.4 to z=0 create a problem?


Thanks!

[Reedfirst]

Load one of the intercon samples that has threading in the program. After looking at how centroid programmed the treading I was able to figure it out pretty easily.

[briuz]

Looking at threads cut with both z=-0.4 to z=0 and when cutting from z=0 to z=-0.4 I can see that it looks like it's doing the 29.5 degree cut. So, I am now looking at my tool geometry as I hand ground it to 60 degrees and used a thread gauge. My next step is to machine a block of aluminum with a 30 degree slot on each side so as to help grinding it to 60 degrees.

[briuz]

I decided to order a carbide insert threading tool instead. Hopefully it will be in by Friday. So, I'll try rigid tapping in the meantime....

[cnc_smith]

Hello,

When threading, on a manual lathe, it is a common practice to set the compound at 29.5 degrees and advance the compound into the thread. Does Centroid advance the tool at 29.5 degrees or is there a way to do this?


Edit to add: I just checked and the "Details" screen indicates the thread is a 60 degree thread. (I am trying to cut 1/4-20 threads.) Also, would my cutting the threads from z=-0.4 to z=0 create a problem?


Thanks!

In Intercon in the Threading Cycle on the Detail screen (the first screen when you create a threading cycle) the Thread Angle is the Compound Angle doubled. So for a 29.5 degree compound angle you would enter 59. The Thread Angle is not the angle of the threading insert/cutter, it is the Compound Angle x 2. On the CNC12 side if you go into the Configuration screen for Parms you can change the default value. From Main screen F1 Part, F3 Config, enter pass word, F3 Parms and change parameter 51 to 59 and this will always come in at the correct compound angle for a standard thread.

[briuz]

Thanks!

Hello,

When threading, on a manual lathe, it is a common practice to set the compound at 29.5 degrees and advance the compound into the thread. Does Centroid advance the tool at 29.5 degrees or is there a way to do this?


Edit to add: I just checked and the "Details" screen indicates the thread is a 60 degree thread. (I am trying to cut 1/4-20 threads.) Also, would my cutting the threads from z=-0.4 to z=0 create a problem?


Thanks!

In Intercon in the Threading Cycle on the Detail screen (the first screen when you create a threading cycle) the Thread Angle is the Compound Angle doubled. So for a 29.5 degree compound angle you would enter 59. The Thread Angle is not the angle of the threading insert/cutter, it is the Compound Angle x 2. On the CNC12 side if you go into the Configuration screen for Parms you can change the default value. From Main screen F1 Part, F3 Config, enter pass word, F3 Parms and change parameter 51 to 59 and this will always come in at the correct compound angle for a standard thread.

[martyscncgarage]

Briuz,
Did you get your question answered and on your way?

[briuz]

I did. Thanks!

My threads aren't yet usable but by doing a right-hand and left-hand thread I can now see that Centroid is feeding the tool at an angle (assumed 30 degrees) and my tool profile is wrong. So I ordered a carbide threading tool as the next troubleshooting step.

I also found out, yesterday, that my VFD isn't infinitely variable but really only has 10 steps between 0 and 100% of the spindle speed. (I want to look into this some more as I feel this is really weird.) This was causing problems as I initially couldn't get my spindle speed under 390 RPM. Once I figured this out, I was able to drop my spindle speed by setting the VFD's maximum frequency going to the motor to 50 hz as opposed to 60 hz. (I can get lower speeds by setting an even lower max frequency.) My current lowest speed is now slightly under 200 RPM. So, progress is being made and I'll soon have more updates to post.

Briuz,
Did you get your question answered and on your way?

[tblough]

One other thing on the thread angle setting in Intercon (and I'll admit calling it "thread angle" does cause significant confusion). Setting this to an angle larger than the angle of the thread causes the chips to curl in the +Z direction. Setting it smaller causes them to curl in the -Z direction. This assumes normal right hand threading from right to left with clockwise spindle rotation.

This is extremely useful when threading really close to a shoulder. Best practice it to stop short of the shoulder at least a chip width to prevent crashing the tool, but you can get right up to the shoulder by specifying a "thread angle" of 61º-65º degrees for a regular 60º thread. This causes the cutting to occur on the trailing flank of the insert and the chips therefore curl towards Z+ and away from your shoulder.

The gist is, depending on which flank is doing most of the cutting, the chip will form and travel on that side. Cut on the leading flank, and the chip will lead the tool. Cut on the trailing flank and the chip will trail the tool.

[briuz]

The problem was with my threading tool. I just ran a test with a carbide threading tool and was able to successfully do 1/4-20 threads. I posted Pics and info to the Centroid Acorn facebook page.

Thanks to everyone for the advice and info!