Thread Milling Steel

[JWB_Machining]

Hey,

So I'm trying to thread mill steel with a Rockwell hardness of C 24. I'm using a thread mill that takes one insert. The question is what feeds and speeds should I use. I created the program on my Haas TM-1 using Visual Quick Code - I.D. Threading.

I'm attempting to thread 1" major Diameter with 14 TPI. The currently drilled hole is 15/16. When I first Ran the Program I had a Spindle Speed of 400 and a Feed of 10. This caused a great thudding sound as the cutter arced into my work piece. So I stopped the program and backed away and thought that maybe My tool was spinning too slow and was banging into the work piece as the tool moved around the helix. I set the spindle speed up to 1000 hoping to correct the problem but the same thing happened, loud thudding and a shaking table.

Any suggestions on what feeds n speeds I should be using? Also how would I determine this information from the Machinery's handbook, if possible.

Thanks Guys.

[Geof]

Check that there is enough clearance for your thread mill; the holder may be contacting the inside of the hole.

Possibly take your speed higher; the threadmill is obviously smaller than 15/16" so its periphery is around 3". You should be able to run at 400sfm which is 1600rpm.

Drop your feed to about 2ipm; you only have one cutting edge which is not going to be able to handle much chip depth.

[JWB_Machining]

Thanks Geof I'll give that a try. But how is 1600 rpm mean 400 sfm? My Thread mill has a Diam of .5", if it had inserts on two sides.

So SFM = .262 x DIA x RPM = .262 X .5 X 1600 = 209.6? Right

Or is the Dia in this case not my cutter diameter but the diameter of the hole I'm cutting?

[Geof]

Originally Posted by JWB_Machining Thanks Geof I'll give that a try. But how is 1600 rpm mean 400 sfm? My Thread mill has a Diam of .5", if it had inserts on two sides. So SFM = .262 x DIA x RPM = .262 X .5 X 1600 = 209.6? Right Or is the Dia in this case not my cutter diameter but the diameter of the hole I'm cutting?

I was simply using 15/16 as the thread mill diameter, it cannot be larger than that. If it is 1/2" then you can almost double the rpm as your calculation showed.

Your mention of 1/2" as the diameter raises another possibility for your bumping.

Does the threadmill sweep out a diameter of 1/2" or is this what you measured it to be. Probably the diameter that the cutting edge sweeps is larger than the diameter of the threadmill body.

If you entered a diameter for the threadmill that is smaller than its sweep diameter the program will be running it way too deep.

The information with the threadmill should give you its effective diameter.

[JWB_Machining]

Hey, Yeah the thread mill sweeps out to 1/2" inch. It's body is slightly smaller than that. I used the settings you gave though and that threaded properly. But You're saying I could have increased the RPM to 3200?

Also After I threaded this hole I was able to screw in a 1'-14 screw perfectly fine. However when I went and felt the threads and the hole was flat in one corner, the thread mill didn't cut part of the hole. So I'm thinking that my 15/16 hole wasn't exactly a circle. When I drilled it out me n my boss were just running this as a test piece before we make the important one and all we did was center drill it then run a 15/16 into it on our manual lathe. At the begining of this there seemed to be quite a bit of chattering. Could this be the cause of my imperfect hole? Should we have center drilled, then used a half inch drill then the 15/16 drill? Or was this a result of the Program Arcing in and out of the hole? And this imperfect hole would cause an issue when I probed it to get my offsets right?

[Geof]

Originally Posted by JWB_Machining Hey, Yeah the thread mill sweeps out to 1/2" inch. It's body is slightly smaller than that. I used the settings you gave though and that threaded properly. But You're saying I could have increased the RPM to 3200?.....

Yes, I said you should be able to go up to 400 sfm (although this may be a bit on the high side). Your calculation a few posts up using 1/2" diameter and 1600rpm gave 209.6 sfm; so to get 400 sfm using 1/2" you need slightly less than 3200 rpm.

Regarding your 'flat' and description of drilling the hole, for best results you should interpolate the hole in the mill, it is not really necessary to drill. If your hole is interpolated using the same work zeroes as the threading things will be concentric.