What's new
What's new

Power tap 1/2-10 2G acme on cnc mill or setup another Op on bridgeport

cgrim3

Cast Iron
Joined
Dec 4, 2020
Location
Baltimore
Hi all,

We are about to machine a part that gets a 1/2-10 2G acme thread. Material is 4340 steel and is .675 thick but the hole will be thru. I contemplated on thread milling it but I bought a tandem acme thread tap instead.

We have a tapping holder and the rigid tapping option on the machine. Would you rigid tap it on the cnc mill or take the part over to the bridgeport, indicate the hole, and then run the tap down there by hand?

I've rigid tapped many threads before but never an acme thread before so any suggestions would be appreciated.

I kind of regret not going for the thread mill. Already bought and paid for the tap though.

Thanks,

Chris
 
That sounds like a really bad idea. Acme taps are fragile. Maybe there's somebody braver and with more experience that will say go for it, but not me. By hand. Carefully and with decent veggie or lard based tapping oil.
 
I think I might just eat the cost of the tap and just buy a thread mill. I thought maybe a tandem acme tap could be rigid tapped on the cnc mill but don't want to risk breaking the tap and scrapping the part. I see scientific cutting tools makes acme thread mills. May give them a try.

Another thing that worries me about hand tapping it on the bridgeport is that the acme threaded hole has a perpendicularity tolerance of .003 to one of the datums. By hand tapping it, you may not be able to hold that tolerance. That is why I wanted to rigid power tap it or to thread mill it.

Maybe I'll see if I can return the tap to MSC and I'll buy a threadmill from scientific cutting tools

Any other thoughts on rigid power tapping it? Spindle is 20 hp
 
Maybe my lack of acme tapping disqualifies this opinion, but I'd just tap the thing.

While it is an acme and not a regular UN form, it isn't much coarser than a 1/2-13.

It looks like they have plug taps (non-tandem) that size. Your part is thin, I think that'd be fine.

If given a tandem tap, I'd also think it would be fine. Although you need more clearance underneath.


I have tapped a 1"-5 hole with an acme tandem tap, was only one hole and the tap was used. Worked just fine.


I'm not sure what you're worried about in a bridgeport? Just chuck it up in a collet, once the threads start cutting it should pull the quill down. I'd hardly call that "hand tapping", the machine would keep it straight. Might as well drill the hole while you're there, if you decided to do it there. But I'd do it on the cnc if you're already milling the part anyway.
 
I think I might just eat the cost of the tap and just buy a thread mill. I thought maybe a tandem acme tap could be rigid tapped on the cnc mill but don't want to risk breaking the tap and scrapping the part. I see scientific cutting tools makes acme thread mills. May give them a try.

You can't thread mill an internal acme on a 3 axis machine, unless *maybe* its a really tiny pitch, and a massive diameter.

You can not do it and maintain any semblance of thread form, or even close to a proper thread form.

You can actually make a reasonable approximation with a key cutter. The pitch is always too
high, and the included angle makes it impossible.

5406273439_f4d39b8453_c.jpg


5409772338_1967d5dea4_c.jpg
 
You can't thread mill an internal acme on a 3 axis machine, unless *maybe* its a really tiny pitch, and a massive diameter.

You can not do it and maintain any semblance of thread form, or even close to a proper thread form.

You can actually make a reasonable approximation with a key cutter. The pitch is always too
high, and the included angle makes it impossible.

5406273439_f4d39b8453_c.jpg


5409772338_1967d5dea4_c.jpg


So the threadmills offered by companies like Vardex and Scientific Cutting Tools do not cut "true" acme threads? I believe what you are saying but am confused as to why. I get the pictures and see the difference but if it wasn't possible, then how are these companies offering thread mills for internal threads?
 
So the threadmills offered by companies like Vardex and Scientific Cutting Tools do not cut "true" acme threads? I believe what you are saying but am confused as to why. I get the pictures and see the difference but if it wasn't possible, then how are these companies offering thread mills for internal threads?

Look at the fine print for those threadmills and see if you can find a disclaimer about use in a 3 axis machine. Odds are you won't find one, but the fact is that it's not possible to generate a true acme threadform in most sizes with a coaxial threadmill.

Tilted spindle in a 5 axis is a different matter.

So they can sell those threadmills no problem, up to the user if you make a bad thread in a 3 axis mill.
 
I think I might just eat the cost of the tap and just buy a thread mill. I thought maybe a tandem acme tap could be rigid tapped on the cnc mill but don't want to risk breaking the tap and scrapping the part. I see scientific cutting tools makes acme thread mills. May give them a try.

Another thing that worries me about hand tapping it on the bridgeport is that the acme threaded hole has a perpendicularity tolerance of .003 to one of the datums. By hand tapping it, you may not be able to hold that tolerance. That is why I wanted to rigid power tap it or to thread mill it.

Maybe I'll see if I can return the tap to MSC and I'll buy a threadmill from scientific cutting tools

Any other thoughts on rigid power tapping it? Spindle is 20 hp
Hello cgrims3,
If you only have the one part to do, you can specify the Rigid Tapping process in Peck form and if parameter bit 5200.6 is set to "1", Single Block will be valid between Pecks to allow swarf to be removed, if that's a consideration.

Rigid Tapping via the Manual Hand-wheel is also possible through parameter setting.

Regards,

Bill
 
Learn something every day- I never considered that you couldn't thread mill an Acme on a 3-axis. Anyway, for just a few parts, I'd put a spring loaded tap guide in the mill (point sits in back of tap) and run it in by hand. Should meet the .003.
 
One thing I've done a couple of times in the past, threadmill with a standard
threadmill for the front end of the tandem tap.. Gets you going nice and straight,
and then just drive it by hand, or your choice of electric/battery operated toys.
 
Wow I honestly never knew that about acme thread mills. Learn something new everyday.

I think we will just do a peck tapping cycle on the cnc mill and see what happens. We have the really good emuge tapping fluid so that will help.

We buy a lot of emuge since we do a lot of stainless, titanium, and inconel. I tried to see if emuge sells acme thread taps and was disappointed to see that they do not sell them
 
So I talked to a nice man at Scientific cutting tools he seemed fairly knowledgeable and he said that a specific acme thread mill made just for 1/2-10 can cut a 1/2-10 acme thread on a 3 axis machine. Refer to the first table in the attached link. Now I am really confused...

Is there some kind of literature on acme thread mills that somebody could point me to? Maybe that will help clarify things.

I am not doubting what people on this forum say. In fact I believe you Bobw and gregormarwick. The man on the phone might not have known and just told me that you can.

https://sct-usa.com/wp-content/uploads/2019/07/2019_sp_acmethread.pdf
 
Blows my mind how they did this over and over everyday 100 years ago with only a fraction of the resources we have now, and here we are today with all kinds of fancy cnc technology, carbide threadmilling cutters, the latest and greatest in taps and unlimited information to look up on the internet... and its still a huge challenge to tap a simple acme thread today.
 
Blows my mind how they did this over and over everyday 100 years ago with only a fraction of the resources we have now, and here we are today with all kinds of fancy cnc technology, carbide threadmilling cutters, the latest and greatest in taps and unlimited information to look up on the internet... and its still a huge challenge to tap a simple acme thread today.

I am using an acme tap for the job. We are running the job early next week. I am in the middle of programming it currently. This entire acme threadmill thing just has me interested though.

The devil is in the details as they say
 
So I talked to a nice man at Scientific cutting tools he seemed fairly knowledgeable and he said that a specific acme thread mill made just for 1/2-10 can cut a 1/2-10 acme thread on a 3 axis machine. Refer to the first table in the attached link. Now I am really confused...

Is there some kind of literature on acme thread mills that somebody could point me to? Maybe that will help clarify things.

I am not doubting what people on this forum say. In fact I believe you Bobw and gregormarwick. The man on the phone might not have known and just told me that you can.

https://sct-usa.com/wp-content/uploads/2019/07/2019_sp_acmethread.pdf

I'm 99% sure I used a 1-5, with the specs from that site you just linked. I'm looking for my drawing to
check it, but I can't find it, it was years ago, and my file names aren't always spot on. I know the
customer I did it for, but I'm digging through folders named "Bent 5/8" shit".. "round thing with some
plates" "Some handle thing" "Pointer things". "-20206 goofy block", "Disc with legs"... "3.5 inch shit"
"Some goofy shit".. "Some goofy shit 2"... "Stupid little fucking I-Beam"...

OK. so maybe I should open a folder and see whats in there.. "Stupid shit the tray sits on"... "Base of the stupid thing"
"Dumb ass thing", "Stupid angles on the tray", "Stupid handle", "Stupid piece of shit with big ass slots" "Stupid plastic shit"

My organization skills are not good. So I looked in the folder "Delrin bushing and some other garbage bullshit".. And I have "Fucked up angled piece of tube" "Half moon POS" "Long shitty bushing" "Retarded fucking handle thing" "Short crappy bushings" and "That long bitch"...

I'm pretty sure that was the job that I modeled up that acme thread, but I'm not finding it there, I think it was
the thread that went down the middle of the "Retarded Fucking Handle Thing".

I don't know where it is.

Model it up. I just went and looked in my Acme tap drawer. It was a 1-5. The flat at the crest blows
out the entire thread form. You could cut that Acme thread with a key cutter just as accurately as with
an expensive "Acme Threadmill".


And honestly. If it just has to work.. Fine.. I'm down with that.. But if it *HAS*!!!!! to be
right, you aren't going to do it with a threadmill.

And for the record. "Functional" and "To Print" are 2 completely different things.

----------

Internal acmes are a pain in the ass no matter what. Especially as they get bigger and deeper.
Get 'em close with your choice of toys, and then chase it with a tap to get them pretty and
proper.
 
So I talked to a nice man at Scientific cutting tools he seemed fairly knowledgeable and he said that a specific acme thread mill made just for 1/2-10 can cut a 1/2-10 acme thread on a 3 axis machine.
Hello cgrim3,
That would be quite understandable in my opinion.

The same as one can model the result and see the interference when using a Thread Mill that had the geometry of an Acme Thread Profile, it could also be modeled to achieve geometry for the Thread Mill that will cut the correct profile in the part. Effectively, the interference with the modified geometry of the Thread Mill, results in the correct profile of the Thread form cut in the part. But depart from cutting a 1/2 diameter and the profile would be incorrect due to different interference.

Regards,

Bill
 
The man on the phone might not have known and just told me that you can.

https://sct-usa.com/wp-content/uploads/2019/07/2019_sp_acmethread.pdf
Hello cgrim3,
Having had a look at the chart via the link above you Posted, I think it may be a case of the guy telling you that "you can", rather than what will result in reality.

I'm sure it could be done accurately with a custom profile for a particular diameter and lead, but the fact that there are Thread Mills listed for a range of Thread Diameters with a common Leads (3/8 - 7/16 x 12 and 1&3/8 - 1&3/4 x 4), I doubt that any special profile has been developed, as one cutter profile isn't going to satisfy multiple diameters (different helix angles).

They may have modeled the profile correctly for the Thread Mills for specific diameters and lead, but if so, why would they not do that also with the different Thread Diameters that share the same Lead?

Regards,

Bill
 
It should be possible to acme thread with a single point thread mill that does not match the profile of the thread. Think more of an involute than line for the tap profile. as it cheats the spiral the 'involute' becomes a straight line in the material. Technically I think it would be the anti-involute in mathmatical terms.
I have thought about this geometry some for a 3 or 4 lead screw.

a skim pass with a lollipop and then a riffled wobble broach is my other idea.
 








 
Back
Top