1 1/4"- 4 TPI Acme lead screws

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.
 
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.

 
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.
 
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
 
Greeting's, should you have tried using a follow-rest.
 
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.
 
It's obvious you do great work, the designer's must know how difficult the part is hence the .005 tolerance.
 
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.
 
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.

 
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.
 
Back
Top