[stuby]

Hello. I have a few questions as far as doing an american thread on a cnc. Im not sure the correct feeds/speeds. I know the feed is the distance between each thread. I.E. 1/4-20 thread has feed of .05 ( 1" divided by 20 tpi. ). But not sure speed? Also if Im wrong on the feed let me know, but I think Im right there. Anyways, thanks in advance, you guys always come through.

[Karl_T]

The best speed will depend on your lathe , tooling, and the material. On my CHNC with a carbide insert on most steels; I'd make my first one at 2000 rpm. and go from there.

[li.weifu]

45#钢
F 1.5 500RPM
F 2 300RPM

[stuby]

Well, I have an old 1988 Leadwell LTC-15 with a Fanuc-OT controller, which I have only moved out of low gear one time, so 2000 rpm sounds a bit excessive, but ill kick it up a few hundred for sure. Also, I have no idea what my book is telling me about the multiple repetitve threading cycle. I would assume that I can just move my tool incrementally negative and run the same pass again, but Im not sure if my chuck will be in the correct position to have my thread start at the same lead each time. That why I need the multiple repetitve cycle. Any input on that? Thanks a lot.

[Geof]

Does your controller recognise the G92 threading cycle? This one is a few more program lines than G76 but sometimes I find it easier to tweak final sizes.

The G92 line has the final Z coordinate, the X size for the first cut and the feed. You position your tool on the line above in the program. Following the G92 are all the Xs for cutting the thread.

An example with Z0.0 at the end of the thread is:

G00 X0.26 Z0.2
G92 X.24 Z-0.5 F0.05
X0.23
X0.22
X0.215
etc
X0.195 (would be about the final cut)

[stuby]

Geof, thank you for the advice with G92, it is working much better than before. Still one last question though. You say to position the tool in the line before you call the Threading cycle. I am cutting a 1/2-20 thread. I position my tool at X.650. Now this is the place where the tool will retract to after it cuts the thread, correct? Because when I place the tool there, and call up X.500 in the threading cycle it appears that the tool does not retract, and once the cycle is complete I have a "tear" in the thread where it looks like the threading tool passed over the surface in rapid. Im kinda stuck here. Ill post a copy of my code in the morning. thanks again.

[Geof]

... I am cutting a 1/2-20 thread. I position my tool at X.650. Now this is the place where the tool will retract to after it cuts the thread, correct? Because when I place the tool there, and call up X.500 in the threading cycle it appears that the tool does not retract, and once the cycle is complete I have a "tear" in the thread where it looks like the threading tool passed over the surface in rapid.....

On my machines the amount of retraction is determined by a Setting maybe yours has something similar, or a Parameter. But I have no idea what it might be called in your controller.

[rruybal]

If you are seeing tearing on the finish pass you may want to check the center distance of your cutter. If it isn't dead on center, but above center, it will give you a bad finish. If anything when cutting a thread you'll want to be no more that .001 bellow center. Are you using coolant? That will help the finish. The rule of thumb is that the harder the material the more passes you take to conserve your cutter and get a better finish. Harder metal more passes and slower rpm.

Hope this helps
rruybal

[stuby]

I fixed my tearing thread. Now Im trying to do a metric thread. I am cutting a M17X1.0. Correct me if Im wrong, but my feed will be 1.0, right? the 1.0 on the thread means 1 thread per millimeter right? I am in metric mode (G21) and I am just making sure I am using the right feeds. Thanks for all the help.

[rruybal]

Hi Bud,
You are correct M17 is the nominal diameter, and 1 is the pitch.

rruybal

[juergenwt]

I noticed!
You called for one thread per millimeter and in this case you are correct but the correct way is like stated by rruybal - 1mm per thread. M17x1 Metric Fine.
Point is if you take a M17x1.5 it is not 1.5 threads per mm but 1.5mm per thread.

Note: only "Metric Fine Threads" have the pitch listed, for Metric coarse thread No pitch is listed and you will have to look at a table (M12) . Metric coarse is generally the coarsest pitch
available for that size. Remember - inch thread we use Threads/inch, in metric we use mm/thread.

[rruybal]

This is for Stuby!!

Yup, you're right, juergenwt. And if Stuby needs to see more info. he can pick up a used Machiner'y Handbook.
It lists the various thrd. forms and the tables are very helpful. Especially when you find yourself with an odd or never before made Dia. & Pitch combination. All the Information you'll need is in the book. I know because I've cut 12-80 3A's and 6-90 3B's. and all we had to go on is the formulas in the book.
If you're looking to machine threads the Machinery's Handbook will prove very valuable.
See ya
rruybal