Some help needed with threads

Morning,

I'm making some antenna parts (I'm a radio ham) and need the create some threads.

The issue I have is what size to drill the holes to tap for the following sizes;

3/8 - 24

5/8 - 24

Had a google and the best I come come up with is;

3/8 - hole 9mm

5/8 - hole 15mm

The threading on the outside of the parts I'm assuming I use 3/8 (9.52) and 5/8 (15.875mm) barstock respectively and run a die around it.

I hope this makes sense.

Thanks

3/8" x 24 TPI is a UNF (Unified Fine) thread tapping drill is 8.5mm
5/8" x 24 TPI does not exist in anything I can find the nearest UNF thread is 5/8" x 18 TPI tapping drill 14.5mm

(See Andrews reply below - 5/8" x 24 is probably UNEF - not a size I've come across before)

Threading a bar just start with nominal size so 3/8" dia and 5/8" dia.

3/8" an 5/8" BSW or BSF are much coarser than the TPI you have given. The nearest metric threads would be
10mm x 1 IsoMetric Fine and 16mm x 1mm IsoMetric Fine. Tapping 9.2mm and 15mm drill respectively.

If you are making both threads, internal and external unless there is a good reason ie matching existing kit just go for what you have or can easily get hold of. I would go for standard IsoMetric coarse as these are the easiest to get these days (unless you are in the States) but don't know if you can alter the bar sizes to suit?

John

Edit: Add ref to later post

Edited By Journeyman on 19/05/2021 09:28:43

The threads need to be better specified as does the material being used. I'd guess that the 3/8" thread is UNF and the 5/8" thread is UNEF and the material is brass?

For 3/8" UNF I'd be drilling 8.70mm giving a thread depth of about 70%. For 5/8" UNEF the minor diameter is 0.5799", giving a thread depth of 0.0226". For 70% thread engagement I'd drill 15.1mm.

For external threads I prefer to screwcut in the lathe, but you are correct that the nominal OD of the threads is 3/8" and 5/8" respectively. Barstock is normally a thou or two undersize which helps the die to cut.

Andrew (G8IUV)

You have not said what thread form you are using.

For Whitworth threads (55° ) with this pitch the thread depth is 0.02668". Subtract twice this from the outside diameter to give the core diameter. The tapping drill should be slightly bigger than this.

For Unified threads (60° ) the figure for internal thread depth is 0.02255".

So for Whitworth that gives 3/8- (2x0.02668) = 0.32164", 8.17mm. So Ø8.2 or slightly larger. 9mm may give a weak thread but be easy to cut, it depends on the material, how easy you want the thread cutting to be and what loads it is being subjected to.

Repeat as required for the 5/8 and similarly for Unified if that is what you are using.

Martin C

Smileys again!

Edited By Martin Connelly on 19/05/2021 09:22:49

I would stick to metric if you don't have the original bits

Starting from scratch with imperial, not recommended

And stick to cheap stock parts

6mm 8mm 10mm 12mm

Hi All,

Ok the material is stainless steel and the threads I believe are

5/8-24 UNEF for the SO239 connectors

3/8-24 UNF (thats all I can find.) for the end of the antenna whips

Chris

Unfortunately the American antenna people have not yet caught up with Metric!!!

What I have been doing in more recent times is finding the closest fitting metric size and retapping that hole with a metric tap

Then metric threaded stuff goes straight in

I have my fingers in my ears so I can't hear any of you screaming

Yuk! Depends what type of stainless, but most likely austenitic, ie, the 3xx series. Of these 303 and 316 are easy to machine although 316 has a propensity to work harden, but avoid 304 as it's 'orrid stuff. For tapping in stainless steel I drop the thread engagement to nearer 50%, so that gives 8.9mm for 3/8" UNF and 15.3mm for 5/8" UNEF. For external I'd definitely screwcut. But if dies must be used then ensure that the die is rigidly aligned with the work, at least to start with. Trying to start a die by hand in stainless steel is a receipe for disaster, or at least wonky threads.

The SO239 connectors are a blast from the past, must be 40 odd years since I've used one.

Andrew

Whilst the above advice is to use metric drill bits, a 19/32" may be easier and cheaper to obtain than a 15.1mm, particularly second hand.
It equates to 15.08mm and will likely drill a tad oversized anyway, assuming the flutes are still in good order.

Bill

Boring the hole may be cheaper still

I feel, Jason, that you personally would spiral mill an oddball diameter like that on the CNC since the actual size and finish are not so critical. Do you ever do thread milling? Constant pitch threads like this are well suited to CNC thread milling because you only need one tool for many diameters and pitches and for both left and right hand threads.

Martin C

I've not tried it yet as I have not had the need, infact I don't find I thread cut a lot in the lathe so even less likely to need it with something set up on the mill. But if a job comes up where it's needed would not mind giving it a go.

I have spiral milled a few holes but again if the item is on the lathe then may as well just bore it at the same time. For example last week I did the piston for an IC engine the underside of which had a circular bore to form the skirt and then two other pockets beyond that shaped to suit the wrist pin, I did do the CAM for the circular bore but ended up doing it on the lathe while I was turning the OD and just doing the two odd shaped deeper pockets on the CNC

Ady1

In a less enlightened age, you would have been burned at the stake as a heretic .They may even now be marching to your door .

If you are lucky, you might get away with a hair shirt.

Chris I find this chart very useful *link*

http://pages.cs.wisc.edu/~bolo/workshop/thread.html

H

To find the tap drill size for 60deg unified threads just subtract the reciprocal of the thread pitch from the nominal o.d. of the thread. For example: 3/8-16, subtract 1/16 from 3/8 and you get 5/16 which is the proper tap drill for that thread. It works with metric threads as well except you subtract the thread lead. For example: M10x1.5 you would use an 8.5mm tap drill. This will get you approximately 75% thread depth in most cases.

I am also a ham radio operator. KX4VI 73 OM

Greg

Still standard fare on almost all modern Ham Transceivers , not only on the HF Antenna connection, but even on VHF and UHF - in fact, the SO239 was known as a UHF connector..

5/8 X 24 is indeed UNEF - Tapping drill 14.75mm

3/8 X 24 is UNF - Tapping drill 8.5mm

both diameters give 60-70% thread depth, it says here. Where?

On the Tracy Tools chart next to my PC! Though as you are using stainless-steel I'd follow Andrew's advice and drill slightly over-size, being careful not to work-harden the surface.

Thanks everyone!