3/8-12 ACME THREADMILL

[dprovost71]

Having trouble threadmilling a 3/8-12 acme internal. The go gage goes before the no go. We're using a 4 flute thread mill from Scientific. The specs on the threadmill look ok. Program looks good. We've got taps on order but I'd like to figure out why this isn't working. Would a single point do the trick?

 

Thanks,

[crazy^millman]

quote:

---

The go gage goes before the no go.

---

What is the P.D. call out on both gauges?? It has been my experience on ID threads the go gauge should go then the no-go should not go so have you said this backwards?

[Columbo™]

Crazy millman is right, the go should go first unless the P.D. is bad.

[dprovost71]

Whoops---yes the no go goes before the no go.

[dprovost71]

And yes the PD must be bad. Have you threadmilled an acme thread before. Gages have all been verified.

[dprovost71]

I keep mistyping here. the no go "goes" before the go....

[Goldorak]

check your O.D. of threads (should be 3/8) the NOGO have a smaller od than the GO

 

your pitch diameter is oversize and od is too small so NOGO pass and GO don't

[crazy^millman]

Ok Check the gauge for burrs or nicks. Also make sure someone did not swap heads on the gauges I have seen people trying to be funny take the heads and swap them. Easily checked over gauges pins with a Micrometer or if you are lucky enough to have an anvil thread Mic for Acme Threads.

 

HTH

[dprovost71]

As I said gages are good. They've been verified. For some reason the tool "is" cutting oversize. We not even to the proper thread depth. Should we try a single point tool? If you haven't threadmilled an acme thread of this size then we might be treading water here. If you have ...what kind of tool did you use?

[dougm]

are you sure you are not "recutting"

the width of the thread

the helix angle in relation to the

thread depth seems to great to have clearance to me

[Columbo™]

quote:

---

As I said gages are good. They've been verified

---

Was the tool checked????

[Guest]

General reasons a threadmill cuts oversize

 

#1 Incorrect Tool definition

#2 Incorrect geometry

#3 Value in overcut box

#4 Tool overhang tool long and on recut cuts too much stock

[gcode]

There are acme threads and stub acme threads

IF you've got a stub acme cutter and acme gages

or visa-vesa you'll be chashing youself in circles for days... been there, done that

[gcode]

quote:

---

General reasons a threadmill cuts oversize

---

#5 incorrect pitch value ... it should be 1/12=.0833

[dprovost71]

We've checked the tool and all parameters in the program look good. I looked in the micro-100 catalog and geometry for a lathe tool matches what we have but our threadmill is a 4 flute. .028 flat into the 29deg incl angle. A stub acme tool has a .033 flat. The lathe tool is obviously a single point tool. Again...its not the gage.

[dprovost71]

The only thing I see in John's post that might come close is #4 the tool overhang. Its a .150 shank the OD is .27 but we're going about .75 to.8 deep. The tool was indicated for runout and it was within .0003

[dougm]

again

on a thread that small you are recutting

the flank of the thread. the .270 cutter

does not have clearance on the helix of the thread

thats why the no-go goes and the go does not

[dprovost71]

That's sounds like a good explanation to me. That would mean Scientific doesn't quite have the correct geometry for a threadmill situation.

[dougm]

Dprovost71

can you measure the root width of the part you cut?

you would need to regrind the cutter to compensate

but the thread angle (29 degree) would still be

wrong .

Im not sure if this can be done

[dprovost71]

I was thinking the same.We did slice the part to see the groove. I was thinking an impression could be taken and measure that. I kind of got thrown into this and there's a lot of disconnect as to who has done what and when.

[Michael Sullivan]

Old thread I know.....Was there any luck with cutting this thread? any tips? I need to cut 50 pcs of 17-4PH .9 deep

 

Thanks,

 

-Mike

[Tim Johnson]

I can't answer for acme threads but I've seen unc/unf threads do this several times. Every time it has been an oversized hole.

[DProvost]

Ok...we had to have scientific modify the flat on the tool. It took a couple of times to get it right. I will have to look it up and post what the flat ended up being.

[DProvost]

The flat on the 4fl threadmill was modified to .021 to make it work. CUTTING OD.270 DIA

;.150 DIA RELIEF DIA. Not sure of your depth you would need.

[Michael Sullivan]

Thanks again for your help David!