What's new
What's new

Tooling for a 1/2"-5 Acme double start internal thread 1.25" long

Is there any mileage in making a couple of special cutters with two edges correctly spaced to do both leads in a more friendly profile to take out a useful amount of material from the middle of the acme profile first. That way not only does the proper acme cutter(s) not have to work so hard, as they are basically profiling the edges rather than cutting full thread, but there is also some space for the chips to curl into as they come off.
If I'm following you I'm wondering the same thing. Run the thread with a grooving tool to depth then come again with the Acme tool, or tools if needed. Even a double tap with a shallow, then full depth groove profile, then a second tap for the acme profile?
 
Hi Clive603 and DMSentra:
Look at the two point tap in post #4 (the first picture of the three.
That home made tap is exactly what you're talking about.
It is undersized. (smaller diameter than the final thread)
It is narrower than the final thread
It only has two teeth, one for each lead so it will not drive itself into the hole but must be driven with a leadscrew.

It is a TAP...so you don't get to set it off center like a single point boring bar...when you want to nibble out your thread in steps you need to make several different diameters and run them in succession.

You have to run it in and out of your part by running the spindle forwards and backwards...you're using a rigid tapping cycle just like with any other tap.

Once you have the bulk of the material removed, you can take the final (biggest ) tap and drive it through the workpiece several times shifting the start point a bit each time to shave the leading and trailing flanks until your threadform is the proper width.

So think of it as a standard machine tap with all the teeth ground off except one (in this case one for each lead)
The smallest tap is like the first truncated threads on any normal machine tap.
The next is like a thread near the middle of the lead-in taper, and the last is like the first full tooth of a standard tap except that the cutting edge is skinnier than you need for your final threadform, so you need to start it in several different Z start points so you can shave the flanks.

It's actually not all that difficult to do...the hardest part is making the taps.
I just used a surface grinder with a wheel dressed to the correct flank angles, and a HSS drill blank .
The fixture has the double start thread of the correct pitch on it, but it's made big enough to be convenient to turn and it's just a 60 degree vee thread so it's easy to make.
The angle you see that I whacked on the end of the fixture is so I can shove it against the fence of the surface grinder and it gives me the correct helix angle so I can grind the spiral threadform onto the tap.

Finally, when you set them up to run them, you need to get the start point of each tap to be correct...so it's worthwhile to make three identical taps and then just reduce the diameter of the first two, so you can touch them all off to a common face when you set up.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Wow. The making of appropriate taps is considerably more than I can handle, I'm sure. I have used a surface grinder exactly twice, and that is only because it was payment for cleaning out a widow's machine shop situation.
 
Hi again DMSentra:
So get a tool grinding house to make some up for you.
This is a doddle for someone like Alfred Lyon at AB Tools.
With their whizz bang Anca CNC grinders they can knock out some customs for you easy as falling off a log.

You just have to tell them what you want.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Hi again DMSentra:
So get a tool grinding house to make some up for you.
This is a doddle for someone like Alfred Lyon at AB Tools.
With their whizz bang Anca CNC grinders they can knock out some customs for you easy as falling off a log.

You just have to tell them what you want.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
Thank you for your help, Marcus. I'll ping them Monday and discuss it.
 
Implmex

Sorry for misunderstanding your earlier post. I read it as meaning the tool was a double lead single tooth tap with proper Acme thread form cutting tips.

Friend Johns point was that trying to cut acme form, even if narrower to allow for final shaving to fit, was problematic due to chip crowding and other issues. Except for the final tool his were spiral grooving tools designed for good chip clearing rather than a formal thread form on the stiffest shank that could be wiggled in. Of course his work was primarily with pretty obdurate bronze so things could go totally tits up very quickly if the chips started fighting back.

Getting a professional firm to make the final sizing tap for you seems a very good idea. None of the headache of trying to figure which lead needs an extra shave when things won't quite screw together which seems endemic to doing them independently. But the initial grooves can be done one at time using the usual rotate the workpiece 180° between leads technique using a sharp clearing tool of whatever shape seems convenient.

As ever the big issue with smaller internal acme is that the full form cut is objectively way too heavy in relation to the tool dimensions. So you have to find ways of trimming out to it in cuts a tool small enough to go in can easily manage.

Easier and most expensive way is to get a set of two tooth tools made up to do the initial groove and final form. Then the only problem you have is aligning and timing when changing tools to follow the initial groove. Material makes a huge difference. Free cutting brass would need a lot less mucking around than the last piece of phosphor bronze I had to thread. 'Orrible metals "super tap-breaker" specification that was!

Clive
 
How well do you guys think a single piece double tap with a straight groove profile to full bottom depth and width, with a second tap on the same body with the full acme profile would work?
 
Hi again DMSentra:
I wouldn't personally invest in it.
I say so because the whole point of doing it with taps is so you can stuff the biggest, strongest tool down the hole...that is always a tap because a tap runs down the centerline of the hole by definition so you can pack as much material on the body of the tap as possible.
A boring bar and a threadmill both have to be smaller than the root diameter of the threadform.

The whole point of roughing it with reduced diameter and reduced profile width taps is so you can lessen the load on each tap as you force them down the hole in succession.
The whole point of making single tooth taps is so they are easier to make...they are essentially similar geometry to a single point boring bar...you just run them differently than you would a single point bar.(with a tapping cycle instead of a threading cycle)
The whole point of making one tooth per start is so you don't have to index anything and your load is balanced but your load on the tap doubles as soon as you do this.

Roughing with what's essentially a tap for a square thread is a shitty way to proceed IMO.
That's because the tools to cut square threads are weaker than any other form...you already have a problem with the weakness of the tool just because the thread is both small and coarse, so the root diameter is small and the helix angle is large, meaning the tool must take a hellaciously big chip on its way through the workpiece.

Weakening the tap further by making the roughing tap a square threadform gains you nothing in any of the domains you care about.
If you evaluate the shape you need to grind on the trailing flank of a square thread tap to give it clearance you will quickly discover that that back side helix is impossibly difficult to grind unless you whack off a whole lot of the back of the tool and fake it, so your tap becomes this wimpy little nail with no material behind the cutting edge on the trailing side.

So make it reduced profile width, make it Acme and make the first two roughing taps smaller diameter to give yourself the best chance of getting the taps through the job without twisting them into oblivion.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
If this is a quote for you, I'd no-quote it.
If you bid and got the job, I hope you put a high number on it, especially if this is new territory for you.
 
Hi Mtndew:
You raise a good point, but there are so many details missing that it's hard to judge just how difficult this may turn out to be for the OP.

First, we still don't know the following:
1) What material?
2) 5 TPI and 0.400 lead or 10 TPI and 0.200 lead?
3) Full profile or stub Acme?...Root diameter?
4) How many?
5) What kind of price?
6) What kind of gear to make them with?

Some things we can guess at, or we've been told...grinding something in house in order to make these is a non starter.
He does not appear to have been receptive to burning them or having them burned for him.
This appears to be a new challenge for him, so there's presumably no experience to fall back on.

With the gear I've got I could make them with confidence using one of the methods I've described, and I wouldn't be afraid of them at all.
I'd quote high though, and I wouldn't cry if I didn't win them.

The places I could likely lose my ass on them is if I needed to order a bunch of custom taps and the parts turned out to be 954 Aluminum Bronze, or Toughmet, or Monel, or some other weird shit that's impossibly hard to machine and I had no access to a sinker.
If I ordered custom Acme taps I could just factor the cost of the taps into the job like everybody else does too, but I'd have to have a reasonable expectation that I could get the taps through the material.

I could even model up a solid carbide single point boring tool and see if the proportions of the bar are reasonable for me to have a chance to single point them with lots of nibble passes, but we don't even know if the OP can model a bar like this in CAD.

As I say, lots of critical details we don't know.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Last edited:
2) 5 TPI and 0.400 lead or 10 TPI and 0.200 lead?

I wondered this also when I suggested Horn.

If it's 10 TPI .200" lead, then Horn 100% have solid carbide bars for 10TPI because I have some, and they are just long enough too. Would probably require some additional front relief grinding to clear the helix angle, but it's a simple screwcutting job at than point.
 
Hi Mtndew:
You raise a good point, but there are so many details missing that it's hard to judge just how difficult this may turn out to be for the OP.

First, we still don't know the following:
1) What material?
2) 5 TPI and 0.400 lead or 10 TPI and 0.200 lead?
3) Full profile or stub Acme?...Root diameter?
4) How many?
5) What kind of price?
6) What kind of gear to make them with?

Some things we can guess at, or we've been told...grinding something in house in order to make these is a non starter.
He does not appear to have been receptive to burning them or having them burned for him.
This appears to be a new challenge for him, so there's presumably no experience to fall back on.

With the gear I've got I could make them with confidence using one of the methods I've described, and I wouldn't be afraid of them at all.
I'd quote high though, and I wouldn't cry if I didn't win them.

The places I could likely lose my ass on them is if I needed to order a bunch of custom taps and the parts turned out to be 954 Aluminum Bronze, or Toughmet, or Monel, or some other weird shit that's impossibly hard to machine and I had no access to a sinker.
If I ordered custom Acme taps I could just factor the cost of the taps into the job like everybody else does too, but I'd have to have a reasonable expectation that I could get the taps through the material.

I could even model up a solid carbide single point boring tool and see if the proportions of the bar are reasonable for me to have a chance to single point them with lots of nibble passes, but we don't even know if the OP can model a bar like this in CAD.

As I say, lots of critical details we don't know.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
I was told today the parts are steel.
350pcs of this one, 350 of 2 others and 700 of another in the same quote.
I have a Hardinge CHNC2 and a small turret lathe and engine lathe to work with. If a cutter for it can be found, and if thread milling would work, the MC4VA Okuma would be used. Seems with the high helix angle milling would be out, IDK.
The owner of the company is set to call when he can, for the rest of the details.
 
I was told today the parts are steel.
350pcs of this one, 350 of 2 others and 700 of another in the same quote.
I have a Hardinge CHNC2 and a small turret lathe and engine lathe to work with. If a cutter for it can be found, and if thread milling would work, the MC4VA Okuma would be used. Seems with the high helix angle milling would be out, IDK.
The owner of the company is set to call when he can, for the rest of the details.

Thread milling internal acme is impossible in most cases. Threadmilling a two lead internal acme is extra double impossible.

Of your options the Hardinge is the best.

What about the pitch/lead?
 
Thread milling internal acme is impossible in most cases. Threadmilling a two lead internal acme is extra double impossible.

Of your options the Hardinge is the best.

What about the pitch/lead?
I figured milling was likely out of the question.
Pitch and lead is one of the details I'm waiting on.
 
Hi DMSentra:
Do you get to pick which steel?
Can it be Leadloy?
If it can, you can probably just get away with single point boring it using nibble passes.

If you never take a full width or full depth pass it's pretty amazing what you can pull off...but not in something awful like Hardox.
If the pitch and lead work in your favour, and if you get to make it out of Leadloy or 303 stainless I'd try to pull it off the easy way...IMO, this is it (if you don't have a sinker).

If you are unfamiliar with what I call "nibble threading" it's a process where you walk into the thread profile in tiny bites.
Mastercam has a utility I recently discovered courtesy of Mtndew that they call "Custom Thread".
It allows you to write code for this strategy easily and it allows you to make a threadform where the tool is not the same shape as the thread you want to make.
So you have a skinny tool ground up by a tool grinding house and bomb through your thread a bazillion times taking a tiny bite each time.
It takes longer than conventional single pointing of course, but it's pretty reliable and you can turn some pretty extreme shit with it.
Here's a picture:
dscn4698.jpg
This thread is a heavily modified 6:32 that was done using this technique.
As you can imagine, the single point bar I made for this is pretty small
Here's the little Devil:
DSCN5804.JPG
It was flimsy enough that I had to take the thread in 0.001" bites if I remember right (it was years ago). but I got it done using this technique.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Last edited:
Internal tool makes acme internal threadmills, likely a few other grinders do as well. they have 1/2-10 listed, surely they can custom make some with the right angles to double the feed rate to get that double start and proper thread form.

For custom taps check Taylor Tool, says on page 31 of their catalog they make custom acme taps and multiple lead is listed as an option.
Who knows could even be a stocked item, you're probably not the first asking for it.
 
Hi SND:
It sounds attractive, but sadly, there are two big problems with trying to threadmill something like this.

First, you're trying to basically stuff a saw into a helix and what happens is you clip the flanks of your profile.
It gets worse as the diameter of the saw gets closer to the root diameter of the thread, and it gets worse as the flank angles are reduced, so a 60 degree vee thread is less distorted by this reality, and a square thread is worst...Acme falls somewhere in the middle.
The pitch or lead together with the thread diameter also influences what you can get away with...steeper lead and smaller OD equals worse distortion, so small diameter double start threads are pretty much hopeless to try to cut this way.

Second, the threadmill must be smaller than the root diameter of the thread so it will fit down the hole.
This severely restricts how deep a thread you can cut...in this case the head of your cutter would be a maximum of 1/4" diameter and it needs to be 1.25" long to make it all the way through the part.
Shank it down so you can actually drive it into the profile of the thread and you have nothing left for a shank...it's maybe 0.050" diameter or so.

So unfortunately the details make this idea unworkable in practice.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Last edited:
  • Like
Reactions: pcd
I'm looking at this as a 1/2"-10 double start with a 5 lead. Not a 1/2"-5 with a 2.5 Lead... pretty big difference.

Pretty sure his customer effed up the call out.
I'd be asking to see/measure a sample if they can't figure it out.
 
Last edited:








 
Back
Top