What's new
What's new

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

DMSentra

Cast Iron
Joined
Sep 12, 2008
Location
Eugene Oregon
I'm finding nothing on tooling for this, and a few major cautions that it isn't doable in tap form. I'd be using the alternating cut P3 in G76 if single pointing. But right now I'm fairly stumped on a tool for it??
 
I'm a novice when it comes to acme, even less experienced with double start.

I did a quick google and didn't come up with any double start taps, saw lots of chinese 1/2-5 taps though.

However, ebay got me closer, but not the size you need. I have to believe somewhere out there makes (or will make) a 1/2-5 double start. I found a 3/8-8 double start finishing tap: https://www.ebay.com/itm/3045767456...V+Vidli|tkp:Bk9SR9SR7K3RYw&LH_ItemCondition=4

That isn't terribly helpful, but maybe gives you hope. Otherwise hopefully someone can say where to get a proper insert and holder.

The manual machinist in me says you'd take a standard acme 5tpi bar and grind extra clearance underneath the leading edge of it, and program it like you said.
 
An internal 1/2"-5 acme? I don't think you're going to find any tooling out there unless you make your own. That bar is going to be awful small and flimsy.
My fist instinct was to check Vargus and Carmex, but the only 5 pitch acme tool they offer is for a 1" and larger.
 
Hi DMSentra:
I'm with Mtndew on this... a 1/2" OD double start Acme tap is going to be fragile as hell, and a single point boring bar to go 1.25" deep is going to be worse.
I am assuming the pitch of this double start thread is 0.2"...do I understand correctly then, that the lead is 0.4"?...or is the lead actually 0.2 and the pitch 0.1?

If it really is a 0.4" lead and 0.2" pitch, you have an impossibly big chip to take in one bite from a tap.
It's also going to dive into the hole at a ridiculous rate...almost 1/2" per turn.

I had a similar problem (but smaller) to deal with years ago...3mm double start Acme with 1.5 mm pitch (3 mm lead), but I had to cut the thread in PEEK, so fairly forgiving compared to metal
Here's how I solved it:
I ground a bunch of two flute single point taps in increasing diameters.
DSCN5443.JPG
Here's the grinding jig with a tap in place.
I fed them into the bore one after another and then moved the start of the biggest tap forward in small increments until my threadform was wide enough so my threaded spindle could get through:
DSCN4235.JPG

I called it good at that point.
I then automated it on the CNC lathe and made a bunch.
(Lots of you have seen these pictures before...my apologies in advance for boring you with the repetition)

This is a workable way for plastic...I'm not so sure you could do it for a metal thread, but I've never had to try.

If it was me, and I had to make a thing like this in metal. I'd make an electrode out of Tellurium copper and burn it on the sinker.
Like this:
DSCN2205.JPG
No fuss and easy to do.
Easy to control too, and no freaky special tap to try to find.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Last edited:
I would check with Widel to see if they would make you a set of taps to git there.
I have very little experience tapping Acme, but the time that I did, I am purty sure that I got the tap from Widel.

But with dbl start and all, I would expect this to be at least a 2 part rough/finish, if not even 3 part?

And I would buy 2 pcs each on the taps so that I wouldn't need the 2nd one.

Or better yet, let someone that does Acme every day run it!
That sounds like the best plan to me. :o


--------------------

I am Ox and I approve this here post!
 
  • Like
Reactions: ARB
Hi Ox:
You wrote:
"And I would buy 2 pcs each on the taps so that I wouldn't need the 2nd one."

So do you have the same experience as me?
Buy just one and break it at the first try.
Buy two and the first one works perfectly for the whole run.

I think it must be a commandment from the God of machining...if you just buy one tool it will ALWAYS break.
Especially if it's expensive and hard to get.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Last edited:
I'm a novice when it comes to acme, even less experienced with double start.

I did a quick google and didn't come up with any double start taps, saw lots of chinese 1/2-5 taps though.

However, ebay got me closer, but not the size you need. I have to believe somewhere out there makes (or will make) a 1/2-5 double start. I found a 3/8-8 double start finishing tap: https://www.ebay.com/itm/304576745692?itmmeta=01HT5DV12ZKTD6RRDYG7EQ78AY&hash=item46ea3050dc:g:85UAAOSwIyNi4J-V&itmprp=enc:AQAJAAAA4PF+PFDvTnZZiH0F9Uz1jqZlvHXxOAtOhzgDM9XA9ZhTBiEmlGxZyx89vgIO1Rj6nl0eBo6KX9sJ/IcwLC/r0X7mfsw8bqVbsxul2qaB2StNQkGH107TpwLsPBdf8JiwJiQp0U9njafFGKtXHz76nE3bPKos4uekZ8wBKiIELMX+2USHW4RL+vcdCY8HmOAxziYDhTEQS1dOWXSqzJcgdFmCl5D5eR+qctDYydgv5mLDmDlRYDObqzn0mgiA43fgiIlXBrg1wB0E9FgpoQLGslCCrfqansNOGy1AEV+Vidli|tkp:Bk9SR9SR7K3RYw&LH_ItemCondition=4

That isn't terribly helpful, but maybe gives you hope. Otherwise hopefully someone can say where to get a proper insert and holder.

The manual machinist in me says you'd take a standard acme 5tpi bar and grind extra clearance underneath the leading edge of it, and program it like you said.
Relieving the rear of a standard bar is pretty much what I'm thinking now too. So far.
 
Can you buy a bronze nut and attach it to whatever you're working on?

What are you cutting?
The job is 350 pcs, and she can't tell me what material. LOL Still working on that. The small hand vise product pictured shows a silver screw(also 350 pcs), but I'm thinking guide her towards a bronze nut if possible. Nuts also get knurled on the OD.
 
Hi DMSentra:
What's the root diameter?
That will tell you how big the tool can be if you intend to try to single point it.
It will also tell you how big a chip a full depth tap is going to have to be able to take.

Look at the tool's constraints...that will tell you how much risk you're going to embrace when you first stuff that tool into the hole.
If you have any input into the material choice for this, press for 660 bronze or something else that's easy to cut and chips in crumbs instead of strings.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Agree that the huge chip with acme is going to be a major problem.

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.

(My late friend John used to single point acme threads for CVA lead and feed screws and I recall him being quite adamant that trying to cut an accurate internal acme with a full profile cutter was asking for trouble. Especially a small one.

Had a graphic illustration of his skills when an expensive replica cross slide bronze feed nut and screw for a Churchill Cub lathe ordered from a well rated company by a friend didn't match. At all!

Expensive company didn't want to know. "We CNC'd the screw and used a set of acme taps so they must have been right when they left us. You've damaged things.".

John took one look at the pair. Said "Idiots cut the screw to maximum book and used a standard tap. Thats never going to work. But I've got the tool to fix it in that size." Tool had the largest shank that would get down the bore with a minimum extension rather too narrow acme profile on the end. 3 minutes juggling about to get it all aligned on his Kerry AG lathe and another couple of minutes taking shave cuts off each side resulted in what we reckoned as a good fit but John considered bit slack.

As I recall under 1/2 thou backlash something I might be able to manage on a lucky day when on top form (= never) yet John did it with that totally casual ease that separates the expert from mere mortals. He showed us his set of tools and only the last one had an acme like profile. John said the art was in getting a groove of the right pitch and depth first because the chips will invariably bugger up things and you need enough metal left on the sides to skim it right. Not forgetting the extra skim on the first turn which always tends to come out a bit thick as the clearances are taken up as the tool comes under load.

I asked why not just cut the acme male deeper to make some clearance and got the look reserved for total bodgers.)

Clive
 
Hi DMSentra:
What's the root diameter?
That will tell you how big the tool can be if you intend to try to single point it.
It will also tell you how big a chip a full depth tap is going to have to be able to take.

Look at the tool's constraints...that will tell you how much risk you're going to embrace when you first stuff that tool into the hole.
If you have any input into the material choice for this, press for 660 bronze or something else that's easy to cut and chips in crumbs instead of strings.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
Going over this more I'm wondering if it's not a 1/2"-10pitch double and they are calling it a 5 pitch in a mix up. There isn't even one single 1/2"-5 acme tap or thread bar for single lead that I can find. I see some 1/2"-6tpi acme. The root for a 1/2"-5acme looks to be at 0.28"? That won't work at all near as I can tell. But I sure don't know much about this stuff either.
 








 
Back
Top