# 1 1/4"- 4 TPI Acme lead screws



## P. Waller (Jun 15, 2018)

Some may be interested in doing such a job, I was handed one this morning and this is how I do it. It is only 12 parts in 360 brass hex stock and the time estimate from my employer is 21.45 hours for the lathe work. My methods may not be the same as how the guru Youtube "how to" video producers may do it but it works for me and the machines available.

The part is 23 5/8" long but the thread is only 10 3/8 long.
Sample




A sample was supplied by the customer.
Measure the sample Pitch Diameter over wires, the .25" lead is wider then the spindle on many micrometers so a .100" gauge block spans the 2 top wires.




My employer was not going to spend several hundred dollars on ring gauges for a small job so I made one at the lower PD limit that would fit the sample.





Face to length and center drill the threaded end, put the chamfer for the start of the thread on before the threading operation saving a tool change later.





The threading starts Monday, will update then.
Used a Vardex horizontal insert internal threading bar at 375 RPMs, will use a Kennametal Top Notch tool for the external threads, I suspect that it will have to be run somewhat slower.

This is done in a Romi/Bridgeport 15 X 40 lathe which is a sort of CNC Manual hybrid built in the 1990"s, these are very nice machines with VERY easy to learn conversational controls, knowledge of G Code is not required for the most part unless the work requires a feature that the conversational input will not do. They have a lot of safety features in the software that will not run a program if there are obvious tool conflicts or math errors. They are the perfect machine for a hobby shop but a bit to expensive even at 20 years old at $10.000-$20.000 used.


----------



## Chuck K (Jun 15, 2018)

Why are you using hex material instead of round bar?


----------



## Rooster (Jun 15, 2018)

Looking good, keep us posted.
Chuck, if you look at the first pic you can see the hex on the far end.


----------



## Chuck K (Jun 15, 2018)

Got it....my mistake.


----------



## P. Waller (Jun 15, 2018)

Chuck K said:


> Why are you using hex material instead of round bar?


That is what the customer wants, I suspect that the hex is a drive feature to fit machines that may be well over 70 years old.

This is a guess of course, it is a rare occasion that I know what the part does.


----------



## P. Waller (Jun 19, 2018)

Was instructed to finish another job Monday morning and resumed the lead screw job today, most of the finish diameter turning is done. Tomorrow the threading begins using 2 Kennametal Top Notch tools, a full radius 1/8" wide insert for the undercut and a 4 TPI Acme insert. Both of these tools have had a portion of their ends milled away in order to clear the live center on small threads such as these, they are 1" square shanks.





Whilst the 12 parts were running (5 hours)  I had the time to assemble a .4"-.7" Mitutoyo dial bore gauge that I received by UPS this morning. The excellent Mits quality that I have experienced over the last 30+ years aside from the case, it is well made but will not fit the assembled tool with its 8 ball anvils. I only use the boxes that tools come in when the tool has many small parts such a a dial bore gauge, anvils, spacers and such.
$370.00 from MSC. Normal Mits quality tool. The acme thread pitch gauge from SPI cost me $96.00 but few people buy them, it has a 1TPI leaf, who makes such threads (-:


----------



## P. Waller (Jun 20, 2018)

Finished this afternoon and the threads turned out nicely as one would expect with 360 brass, 265 Rpm's.

The thread lead is .25" which is right around 66 inches per minute feed rate at that speed, the next spindle rpm is 375 which would be 94 IPM, this machine has a max feed rate of 100 when in a rapid move. I chose not to run a 20 year old machine at 95% of its maximun feed (-:

The first pass was .006" DOC, all passes afterwards were .004" DOC, the last 2 finishing were .001" DOC with 2 spring passes.

Did not check the time but it was slightly longer then the estimated 21 hours


----------



## Rooster (Jun 20, 2018)

Very nice looking threading job P.Waller. Wonder why 360 brass was requested and not 954 alum. bronze. That's a big shaft/screw for such a soft material.


----------



## P. Waller (Jun 20, 2018)

Rooster said:


> Very nice looking threading job P.Waller. Wonder why 360 brass was requested and not 954 alum. bronze. That's a big shaft/screw for such a soft material.



I do not know but suspect that they would rather have the screw wear out then the nut, The customer is a 100 year old company and these are replacement parts for machines that may be 70+ years old and the original parts were brass. We just copied the sample.

The Top Notch tools are excellent, one tool will hold many inserts, 30 Deg. metric trapezoidal threads, Whitworth, American buttress threads, unified and metric 60 Deg. V-threads, square and full radius grooving and thin wall parting. A bit pricey for a hobbyist but versatile if a shop does a good deal of  small runs.
https://www.kennametal.com/en/products/20478624/62318451/56148232/56148278/56148748.html


----------



## Richard King 2 (Jun 21, 2018)

LOVE this thread!!  only thing I can comment on, is the lathe is sitting on 4 x 4's and not level aligned...sighhhhhhhhhhhh.


----------



## P. Waller (Jun 21, 2018)

Richard King 2 said:


> LOVE this thread!!  only thing I can comment on, is the lathe is sitting on 4 x 4's and not level aligned...sighhhhhhhhhhhh.


Just a picture of the same machine found on the web, these lathes are so short and stout that there is no need to level them, the only way there could be twist in the bed is if it was screwed tight to an uneven floor.


----------



## P. Waller (Jun 21, 2018)

This is how simple the programming on these machines can be.

Press the MDI (manual data input) button and the screen in the background appears.

Line 0000 is already there, it is a date and time stamp
Line 0010 Is the tool change call
Line 0020 is optional, I put a rapid move in well outside of the part  because otherwise it will rapid right to the start position and I do not like that
Line 0030 is optional, a program stop which stops it at the first move, this is a personal choice.
Line  0040 is the thread cycle which opens the screen in the foreground
The actual G-Code is generated by the control and may be easily viewed and edited if required. There are certain operations that the software will not run in this mode, such work requires CAM or Fingercad.

Enter 1 for for OD threads
Enter the lead 4 TPI = .25
Enter the thread Depth, I used the MH thread data
Enter the Doc of the first pass
Enter the DOC of all but the last 2 finish passes
Enter the DOC of the finish passed
Enter the number of spring passes
Enter the distance that the tool moves outside the major diameter
Enter the angle at which the tool approaches the work, I do not believe that this is important but that is a point of much angst for many hobbyists
Enter the Z position where the thread starts, in this case it is a straight thread so the thread began .200" before Z 000, if a tapered thread start at 000
Enter the End Z position where the thread ends in the undercut
Enter the start diameter, this will be smaller then the end diameter with a tapered pipe thread
Enter the end diameter

Press enter and thread away.
This assumes that you know enough that you have already turned the stock to size, chosen the tooling and set it, prepared the work holding, order of operations, compiled the thread data and chosen a spindle speed.

It merely takes the drudgery out of repetitive operations such as this, anyone that is proficient at running a manual lathe would be knocking out parts in one day.


----------



## P. Waller (Jun 22, 2018)

Began an interesting job today, 21" long 3/4" diameter bars of 304 SS with 3/8" of Monel weld built up on one end, the machining instructions are to turn the welded end to 3/4" and remove the washer.
The parts looks roughly like so, I made a mistake with the drawing whilst editing the dimensions so the finished length is 20.188"




Turned the welded ends today, an interrupted cut in welded material is not tool friendly and knocked the corners off of half a dozen CCMT inserts.
This is 80 parts by the way.







The next step is to drill centers in each end then turn the entire length to .625" Dia. then thread the end opposite of the weld. I would do this in a collet chuck 1/2 way from each end with a live center, this will leave a visible line at the center but will be well within the +- .005" tolerance.

I have nearly convinced my employer that it would be far faster to rough turn them leaving .005" on a side and then send them out for centerless grinding then face to length and thread afterwards. I do not want to turn such a long small diameter bar to finished diameter, 80 times, this would be fussy and slow. The time estimate for the lathe work is 81 hours.

This is the lathe running, when the proprietary $600.00 CRT display that is 20+ years old quits just unplug the VGA cable and plug it into a $60.00 15" flat screen led monitor, this is far less expensive and far easier on the eyeballs.
Technology is awsome.


----------



## P. Waller (Jun 23, 2018)

The centerless grinding shop can not finish them before the proposed delivery date so I am going to try turning 19" of  3/4" bar to .625" +-.005" in one setup, I suspect that this will end in tears.

A 5C collet chuck held in an adjustable 3 Jaw with a live center in the tail stock end, adjusted the TS to remove as much taper as possible and a test part was within .001" on each end, it was however .003" big at the center which is well within the tolerance. Could easily program a taper in/taper out  but this slows things down a good deal.
Tail Stock removed




The finish was excellent, very consistent with no streaks or smears. Used a DCMT insert with the smallest nose radius that I  could find. A novice may wonder why I do not just take a skim cut at the end and remove the taper at the center of the part. This may seem intuitive but often causes problems in practice, a very shallow depth of cut on such a long thin part will often result in chatter and/or a less satisfactory surface finish


----------



## Rooster (Jun 23, 2018)

Greeting's, should you have tried using a follow-rest.


----------



## P. Waller (Jun 23, 2018)

Rooster said:


> Greeting's, should you have tried using a follow-rest.


Not really, there isn't one for this machine and if we were to build one it would be a third axis which as far as I can tell the control would not support.
However if such a machine was dedicated to producing the same part every day for a long period of time it would be a consideration indeed. This is a short run machine doing several hundred identical parts one week and 20 completely different parts the next week.

This job is 80 parts total and I have a time estimate of 1 hour per part which will not likely happen, if I can keep the the center within the window of tolerance in a reasonable time it will be fine.

If turning it in one setup takes entirely to much time I will turn it to center from each end, this will leave a visible mark at the end of cut but as long as it is within the +-.005 call out it will not be an issue. Experience tells me that I will end up turning it from each end in order to make time.

You do not know until you try.


----------



## Rooster (Jun 23, 2018)

It's obvious you do great work, the designer's must know how difficult the part is hence the .005 tolerance.


----------



## P. Waller (Jun 25, 2018)

Rooster said:


> It's obvious you do great work, the designer's must know how difficult the part is hence the .005 tolerance.


More likely someone has done this part in the past and it was not very profitable for them, when asked to do it again at the same price they said NO.

It then gets shopped around until someone is found that will, this means you're it much like the childrens game Tag.

The upside is that if you are willing to eat dirt on occasion for a large customer they will throw a great deal of profitable work your way.

You may have to eat it for a while however.


----------



## P. Waller (Jun 30, 2018)

One of todays jobs, modify an off the shelf stainless threaded insert, the original internal thread is 5/16-18 the external thread of 1/2-13 remains unchanged

The customer wants the internal thread drilled and tapped to 1/8-28 BSPP which leaves a wall thickness of about .015" at the bottom of the grooves making them difficult to hold for tapping.

I held them in a 1/2" 5C collet in a turret lathe, drilled and taped 29 of them and did not spin one part when machine tapping, it went way better then I had anticipated, about 1 1/2 hours in all, if the internal thread was 1/8 BSPT all bets would have been off.









Then made an installation tool that fits inside the locking tangs from 360 brass, if 100's or 1000's of them would need to be installed I would have used a prehardened steel for the tool instead of brass, only 24 parts are used for this job however.


----------



## Rooster (Jun 30, 2018)

I'm assuming you mean 3/8-28, parts turned out nice. So that's what an old Hardinge looks like, also noticed 5 chucks on the turret and 5 chuck keys on the bench.


----------



## P. Waller (Jun 30, 2018)

Rooster said:


> I'm assuming you mean 3/8-28, parts turned out nice. So that's what an old Hardinge looks like, also noticed 5 chucks on the turret and 5 chuck keys on the bench.


Actually 1/8-28 BSPP is 1/8-28 British Standard Pipe Parallel, BSPT is British Standard Pipe Tapered, many machines and components made in Europe use BSPT for fluid couplings. BSP threads are 55 Deg. included Whitworth.

We are not a production shop, I use what drill chucks are lying about, different chucks different keys. This can be annoying as one may imagine.
That Hardinge lathe could well be 40+ years old, a most excellent machine and is nearly silent at 4000 RPMs, you could buy 10 import lathes today for what that machine cost in 1970.


----------



## Rooster (Jun 30, 2018)

No offence of any type meant, i just looked at my MOLO book and now see the thread size. As far as the Hardinge goes, i agree that older american built machinery is far superior. I my-self have a wonderful Atlas 618 that is about 65 years old that i would not trade for a dozen imports.


----------



## P. Waller (Jun 30, 2018)

Rooster said:


> No offence of any type meant, i just looked at my MOLO book and now see the thread size. As far as the Hardinge goes, i agree that older american built machinery is far superior. I my-self have a wonderful Atlas 618 that is about 65 years old that i would not trade for a dozen imports.



No offence taken, British Pipe threads are uncommon in the US so not widely known outside of industry, a plumber in the US that threads NPT all day long every day could not visually determine the difference, I have been turning threads for 30+ years and could not  tell the 1TPI and angle difference by eye.

If you can do that you are a Wizard (-:


----------

