View Full Version : Grinding ACME threading tool

02-10-2011, 06:02 AM
I have a couple of internal ACME threads to cut as well as an external one... One internal is left handed...

they are all 1/4" pitch around the 1 1/4" diameter..

What is the best way to grind the threading tool... I have done plenty of V threads before but never an ACME..

With V threads I just grind to the appropriate angle either 60 or 55 degrees and go from there.. But I know it is not the ideal...

Should I make allowances for the helix angle?

Should I angle the tool?

Also did Britain use the same ACME thread standard that the US uses?

The job is lead screws and nuts for my Denbigh slotter conversion..

02-10-2011, 06:29 AM
Can't help you with that one however I am going to hang in there with you and wait for an answer too, I've got the same question.


big job
02-10-2011, 06:33 AM
Its been awhile for me to, but as far as I remember the tool should be
ground 29* with both side relief. Then the tip is ground to match the
width of the thread root. Then set the compound 1/2 of that like 14.5*
set right or left for rt or lf threads. Probably should buy a acme pich gage.
I have used thin tin cut with tin snips carefully to make a templete to
grind the tool which is really a forming tool. Internal threading is the same
as external except its done backwards. I dont have a carriage stop so I
just use masking tape on the bed to thow 1/2 nut off (internal threads)
where you have to be sharp and act fast or your going to crash it. Oh
also there is no rake on the top of the tool, that depends on what kind of
tool holder you have. Then this is set dead center perpendicular to the
work and this is all I know.

j king
02-10-2011, 08:27 AM
There is a fish tail gauge that is like a regular threading gauge .It has the 60 deg. form and has the different pitch sizes to grind the tool. Works very well.You use guage to set tool square to part the same as the normal thread guage.

I usually plunge straight in and then move side to side to get smooth ,chatter free finish.

02-10-2011, 08:54 AM
Probably should buy a acme pitch gage.

I was going to say the same thing

I find gauges to be a very valuable tool when grinding threading tools

John Stevenson
02-10-2011, 09:01 AM
Might pay to make the tool out of round HSS, say a broken end mill shank.
This way you can twist it to get the correct helix angle.

UK Acme is the same as US Acme at 29 degrees, it's the newer trapezoidal threads that are 30 degrees.




Tony Ennis
02-10-2011, 09:02 AM
"Tubal Cain" posts informative videos.

#24 (http://www.youtube.com/watch?v=pxmHsDroEDI)

#25 (http://www.youtube.com/watch?v=dhec5osxSs4)

Big T
02-10-2011, 10:29 AM
"Tubal Cain" posts informative videos.

#24 (http://www.youtube.com/watch?v=pxmHsDroEDI)

#25 (http://www.youtube.com/watch?v=dhec5osxSs4)

Agree! He has some very good videos on his youtube channel.
New one shows acme threading

j king
02-10-2011, 12:05 PM
Doohh..John is correct on angle..too early to be trying to think let alone share any knowledge.

Dr Stan
02-10-2011, 12:13 PM
2X on getting the Acme gage. While I was in the Navy I probably cut just as many, maybe more, Acme threads as V form threads. A gage is virtually a must to properly grind the tool and to set the tool in the lathe.

If you have a cam lock spindle here is a tip for the internals. Turn the tool upside down and run the spindle in reverse. This allows you to cut RH threads while cutting toward the tail stock thus reducing the chance of a crash. Good trick to use any time you have to thread a blind hole.

NOTE: Do not use this technique if you have a screw on lathe chuck. :eek:

02-10-2011, 05:36 PM
Thanks everyone... One has a good TC grinder so grinding up the tool will not be difficult, it was just whether the helix angle will cause some concern was all...

But Sir John's reply of making the tool out of round HSS see's to that problem..

02-10-2011, 06:13 PM
The allowance for the helix angle is very important if you want the tool to actually cut without rubbing on the sides, the leading edge should be ground to the lead angle plus 3 - 4 degrees while the trailing edge can be at 90 degrees to the center line or even a few degrees the other way.

Spin Doctor
02-10-2011, 06:14 PM
I have to ask is an Acme thread the one Willy Coyote would of cut. I got's to know.

02-10-2011, 07:16 PM
Love the tubalcain videos. I've watched lots of them.

"Only the 2 kids in the front were interested in the theory."
"Pay attention, don't answer the phone!"

Anybody have his email?
I'd love to send him an appreciation note.

02-11-2011, 12:16 AM
The allowance for the helix angle is very important if you want the tool to actually cut without rubbing on the sides, the leading edge should be ground to the lead angle plus 3 - 4 degrees while the trailing edge can be at 90 degrees to the center line or even a few degrees the other way.

X2 on this.

Also, it can be helpful to "rough" out with a 60* tool (or something close).
Then, finish with your 29* acme. Especially if your lathe is on the smaller side. On 60* threads, almost all the cut is on the left flank (when cutting rightside up towards HS). Same cut in acme is consuming on left flank and nose.

Forrest Addy
02-11-2011, 02:19 AM
Boring Acme threads can be a trial because they are coarser in pitch and far longer in engagement than equivalent V threads. The effective cutting edge may have triple the length of of the UNC V thread plus the bar has to be skinnier in order to clear the tool for withdrawal.

A 1 1/4 -4 Acme will have an internal thread minor diameter of 0.962 to 0.967. The full depth would be 0.140". 0.950 (allows tool clearance) - 0.140 -= 0.810 max bar diameter. Acme threads may have several diameters engagement. If the bar is 0.810 dia, the thread engagement is 2 1/2", and the thread has 0.230 total length of cutting edge, tool deflection (and chatter) will be a real problem.

My solution is to use a bar as large as calculation permits. Grind the tool to length and profile and bore the thread. The tool is withdrawn for subsequent passes by clearing the tool from the work and reversing back with the tip of the tool following the work. The clearance of the halfnuts on the lathe's leadscrew will limit the effectiveness of this trick. Adjust the tool out periodically against an indicator for the next series of cuts I use a tool deliberately narrow, cutting alternate flanks to gain some width then take a few passe to go deeper. Once the tool is at full depth I can move sideways to get the full form thread space.

Using the above technique I've cut 3" 2P 1" lead double Acme lead screw nuts nut 7" long. You really have to focus. Let your mind drift or get out of sequence and Crunch!!

Needless to say internal Acme threads are a bitch to measure. Make a gage duplicating the screw to be fitted first.

The probleem is making good Acme nternal threads is tool deflection. If the bar i too limber the entry thread may be OK but those farther in may be U/S. But enlarging the bar to the max practial limit, narroeing to tool, and side cutting to reduce edge exposure you can reduce tool deflection and hopefully bore an internal thread whose lead is correct, all thread flanks bear, the thread axis is concentric to part references, and it backlash with the screw it's made for is optimal.

Greg Q
02-11-2011, 05:34 AM
For the nuts would you consider trying the acetal moulded technique that Evan posted about a few months ago? (Basically make your nut blank, saw it in half and then clamp it over a heated portion of acme stock to make it melt to a matched female thread form)


02-11-2011, 05:56 AM
It would probably work for the cross slide screw but I am thinking it would fail for the jack screw

Link to the thread for those wondering what we are talking about


Greg Q
02-11-2011, 06:12 AM
Hmm jack screw eh? It probably would be not too good to have that nut strip out its threads all at once, would it? Thinking about it now, 1 1/4" is a pretty hefty screw...I wonder what the practical maximum size is for a hot formed nut to work well?


02-11-2011, 07:19 AM
I have a graduated loupe I bought off eBay for a few quid to check the angle of tools and inspecting the cutting edge. This is some kind of form tool I found in a box of stuff, as an example.


02-11-2011, 10:47 AM
Double depth 4tpi acme=.270 in.
root dia=.980 in.
helix angle (at the root)=arctan .250/pi(.980)=4.64 degrees

I would add a couple of degrees and grind the clearance at about 7 degrees.





02-11-2011, 11:02 AM
Another thing that I've done is to grind a relief along each side of the threading tool I use a Dremel cut off wheel, this gives the chips some place to go and does away with the chips having to make a 90 turn and gives a better finish. I would post a picture but I still don't know how to, I had a photo bucket account but still couldn't post they just don't make it easy.

02-11-2011, 07:49 PM
Well I must be stupid and blind...

Ground up a tool in the TC grinder for a 1/4 pitch ACME...

And guess what....

Denbigh in their wisdom used square threads for all their lead screws..

I just assumed automatically it would have been an ACME even though it was staring me in the face all the time that is was square...

I have to make a new screw and nut for the jack so all is not lost...

02-11-2011, 11:26 PM
You might want to check it is actually square and not modified square section thread, with 10degree flanks.

02-12-2011, 01:43 AM
Well I have cut the screw for the jack..

Took awhile but the lathe handled it very easily.. I doubt whether anyone would want to pay me by the hour :) Material is 4140 OD 1 1/4" pitch 4tpi. Thread depth 1/8" I took 0.01mm per pass @ 54rpm. The tool is 3/8 round HSS mounted in a 1/2 square split holder then that was put in a 1/2 square holder.. I was able to turn the cutting bit to the required helix angle... Lots of lubricant is a must for any sort of job like this...



Black Forest
02-12-2011, 02:48 AM
I think you did a great job on that acme screw. Looks good. So where is the nut?

02-12-2011, 08:02 PM
Here is one nut...

This is the smaller one... Thread is a 1" 4TPI Left Hand.



Grinding the cutter



02-13-2011, 06:07 AM
Got some time this afternoon to finish it off... Had to make a 3/4 boring bar for the bigger nut..

Job went OK... Learnt a lot in the process..

I have to get some loctite tomorrow then I can press the nuts into their housings... They are a press fit but I will still put some loctite on them just to be sure...



tyrone shewlaces
02-13-2011, 02:19 PM
Might pay to make the tool out of round HSS, say a broken end mill shank.
This way you can twist it to get the correct helix angle.

Sounds good in concept, but if you grind the tool correctly to be installed at any particular angle, once you go to twisting it you reduce the angle of the sides and width of the flat a bit which would require a different grind so that it's still 29 deg. and proper width after the twisting. For visualization purposes, take it to the 90 degree extreme and you can easily picture that you'll have a 0 degree cutting angle and 0 width. Twisted positions in between and you'll have some other angle & width in between. This would require doing some math which is not a huge deal, but the hard part (compared to simply using the fishtail tool) is the actual grinding an accurate cutter.

This reduction may not be significant enough to take it out of tolerance depending on the pitch, but it pretty easily could too.

Just my preference, but I'd find it easier to just grind a square tool with adequate relief to suit the particular helix you're cutting that day.

For square threads the angle wouldn't change as long as you have 0 top rake, but the width still would. Looks like the OP cut his threads so he must have done OK (looks pretty good to me). But for future reference...