Acme threading

[fishinchip999]

I have some acme threads to machine. The threading is not an issue but I now have a thread that calls for a "quick start". I understand what this is but have not been able to find information about the dimensioning of the quck start feature. Does anyone know where I might be able to get some info?

[Konrad]

>>The threading is not an issue but I now have a thread that calls for a "quick start". I understand what this<<

Sorry no help to you, perhaps you can explain me what this is?


Konrad

[Geof]

"Quick start" Is this what is known as a Higbee thread start?

[tobyaxis]

Originally Posted by fishinchip999 I have some acme threads to machine. The threading is not an issue but I now have a thread that calls for a "quick start". I understand what this is but have not been able to find information about the dimensioning of the quck start feature. Does anyone know where I might be able to get some info?

Machinery's Handbook

[fishinchip999]

Goef, yes it is what is known as a higbee start. I did find the info I need on this and Toby, if you can point it out in the handbook it would be much apprciated as I was unable to find my answer in there. Thanks all for replying

[tobyaxis]

You will find it under Acme Threads>>> American National Fire Hose Connection Screw Thread.
Here is a Zipped Screen Shot.
Enjoy!!

[Geof]

I did a bit of searching for specifications of a Higbee cut without much success. Here is one thing I found:

Sandvik Coromant calls it "thread deburring" or "turning off of the thread" which removes 3/4 of the first thread for a burr free finish - easy with CNC - they include sample programs for doing it in their threading application guide (pg.35). The first thread root is turned off 270 degrees (with a cut off blade) and the tool retracted to give a tangental cut out from the root through the crest of the thread.

I also have this one in my files:

I will try my best to explain how it is cut.
First what you want to acheive is to remove the part of the thread which is usually a small fin on the turned 45 degree angle portion of the part blank up to where it is a full profile 60 degree thread form.
To do this you use a grooving tool after you are done with the threading cycle. First off you must calibrate your threading and grooving tools to the face of the part (or zero.This is where an important trick lies hidden. The center or tip of the threading tip has to be calibrated so it is equal to the leading edge of the groove tool and the groove insert must be as wide or wider than the base of the thread form (an 1/8" wide insert will work up to 8 pitch. etc) Lets say you are doing 10 pitch threads 1" thread length. Now with your regular threading cycle when you program your length you will get 1 full inch of thread and your first full thread length will be z-.100" (a starting length to be deburred) Now program your grooving tool(also in the same threading cycle as used to thread with) to a depth of z-.100" and you are starting to get a deburred thread. You will only need a couple of deburring passes to remove the burr (so play with the starting x value). But there is more to explain !! Spindle rpm and the machines rapid traverse rate will determine the amount of angle of ramp on the deburred thread. The machines rapid rate will stay constant so for a squarer ramp run slower rpms and a tapered ramp more rpms. Only one more tip if after calibrating the tools you have to adjust the z length of cut you must offset the z length equally on both tools. Possibly use G32

But apart from the 270 degree length of the cut there is no mention of specs.

However I remember from a long time ago doing higbee cuts using a milling machine and the cutter diameter was twice the thread pitch or something like that, maybe three times. The cut face met the crest of the thread at about 45 degrees.

Remembering this takes me back almost half a century to when I was doing my apprenticeship in a place that made fire fighting equipment. I made a fixture for higbee-ing external threads by putting a hole through the side of an internally threaded part and clamping it on the machine table with the cuttere in the hole. Then you just screwed the piece up to the cutter to higbee the end. We didn't call them higbee of course they were just called blunt start threads; and we didn't work to any specifications I can recall.

[tobyaxis]

Geof,

This sounds like he will need the mating part to check the Threads.

[gramsay]

I run a CNC lathe at work and I primarily cut premium threads. Most of the threads that I cut do have what you are calling a "quick start" except we call it thread clipping. To do it we use a .250" grooving tool and a G32 treading can cycle. As far as exact measurements go to set it up I'm not really sure. The tool basically starts at the face of the part and feed into the thread and tapers out after about one full pitch. I know that it is pretty tricky to program and actually quite difficult to set up in the machine.