# Making a Cross Feed Screw for a Lathe or Mill



## 4GSR (Dec 9, 2017)

I am posting pictures of the setup I use to cut a thread on a rod or bar to use for a feed screw for a lathe or mill.  Fairly straight forward.
Make sure you have enough material sticking out of the chuck as shown, even if you have to start out with a longer piece of material.  Oh, Make sure the chuck you are using has a good firm grip on the screw.  It slipped on me and cause havoc before I could get the lathe stopped.  The threading insert shattered into several pieces.  I destroyed two inserts doing this job.  Most of the blame was me, not the machine!  Running the spindle at about 125 RPM! And missing my number on the thread dial! I was trying to keep from going into back gear, which I managed not to. I did get it threaded okay.
Notice I have the tool bit just behind the follow rest jaw for cutting a left handed lead thread.  Also notice I have the compound set at 90 degrees or parallel to the screw being cut.  The reason for doing this, is to allow "side stepping" the threading tool once you get to the depth you need for the thread being cut.  Example, I'm cutting a 10-pitch Acme thread, the basic depth is 0.060"  deep.  You add 0.010" to the depth for root clearance for a total of 0.070" deep.
One more thing, I generally try to use a piece of 1144 T, G, & P Stressproof for making screws.  I have used drill rod for screws too.  Try to stay away from 1018, 1215, 12L14,(reason being, they are too soft) or other unknown steels.  Some steels can turn your project into your worst nightmare, too. 




The tool block I'm using is one my dad made many years ago, I guess in his shop class at school.  We modified it a time or two to fit the tooling we had on hand at the time when it was used.  It's the only tool post arrangement I can use properly with the follow rest.  The Aloris style tool post just will not work for this application on the 9" SBL. 


Leave the live center loose in the tailstock so it will allow the follow rest to self align with itself while cutting.  Again, make sure you have running clearance of the cutting tool and tailstock so you don't crash.  Oh, as always, use your favorite cutting oil/ fluid for cutting the thread.  I did not use the one's shown in the picture.  I used a combination of Mobilmet 766 and Trim cutting oil.  Don't be afraid to use lots of cutting oil!

L
	

		
			
		

		
	



Start out taking about three passes taking a .010" depth of cut per pass.  Back off to 0.005" per pass until about 0.050" depth is obtained.  On a smaller lathe such as 9" SBL, this is about as deep as you can get without it taking more power than the lathe can put out.  Got to remember South Bend didn't put anything larger than a 1/4 HP motor on the 9" workshop lathes!  And that is what I have.  So, this is where you side step the threading tool side to side by about 0.005" in both directions.  This should get you enough room to get the threading tool to depth.  Once the depth is reached, again, start side stepping the threading tool to get a nice clean thread. 
Check the pitch diameter of the thread using thread wires, not the nut.  More than likely, the thread will still be slightly over sized on the pitch diameter.  Continue side stepping the threading tool until you get the pitch diameter in spec.  DO NOT GO DEEPER WITH THE THREADING TOOL!  The reason for not doing this, is the standard threading inserts off the shelf are ground to the nominal root width of the internal thread, not the external thread.  FOR an external thread, the root width varies with the Outside Diameter of the thread and class of fit for the thread.  For example, this thread I'm cutting calls for a root width of 0.0332" for the external thread.  Internal thread root width is 0.0319".  The other thing I didn't mentioned earlier, I usually run a insert width one thread pitch smaller, not always, but most of the time. As on this thread, an 12-pitch insert.  Just means having to side step the threading tool a bit more in the threading process.  


Polish the thread flanks with some 180 grit emery cloth by taking several passes until the thread starts getting very shiny as I did on my cross feed screw.

F
	

		
			
		

		
	



Finally, the finished thread.

If I forgot anything, I'll come back and add an edit to this post.

Ken


----------



## mikey (Dec 10, 2017)

Came out nice, Ken! Does the follow rest on the SB9 normally bolt to the right side of the carriage? That sure makes life easier if it does.


----------



## 4GSR (Dec 10, 2017)

mikey said:


> Came out nice, Ken! Does the follow rest on the SB9 normally bolt to the right side of the carriage? That sure makes life easier if it does.


On the South Bend lathe, that is correct.  If you notice in the pictures above, the follow rest jaw is almost on center of the cross slide.  Back in the day, this was done so you used the "straight" tool holder used with the rocker tool post to thread with.  Boy, has things have changed.

Something I forgot to mention in my original post, I cut all of my cross feed screws and most others here on my 9" South Bend lathe.  It has very accurate lead screw with nearly no noticeable wear or lead error.  I can't say that with other lathes I've had over the years.  I have a piece of material bought to make a new lead-screw for my Rockwell lathe in the future.  I'll probably do it on my new to me 15" Sheldon lathe.  It has a unworn lead-screw on it.  Still have to mount a follow rest on it.  I have one that will be modified to fit that I will use to make the lead-screw.   The 9" SBL just doesn't have a hole big enough thru the spindle to do a 1" OD lead-screw.  Darn!

Ken


----------



## markba633csi (Dec 10, 2017)

Hi Ken, why could you not use an Aloris style tool post for that job?  
Mark


----------



## 4GSR (Dec 10, 2017)

markba633csi said:


> Hi Ken, why could you not use an Aloris style tool post for that job?
> Mark


The small AXA size of the DMT model I have stuck out too far off the compound.  It didn't matter if I put it to the left or the right of the center of the follower rest.  You don't have this problem with most newer lathes and follow rest.   And if it wasn't for the follow rest being on center of the cross slide I probably could make it work.  Also there is not enough travel in the compound to get the tool bit in the right place using the Aloris style tool post.

Ken


----------



## markba633csi (Dec 10, 2017)

Aha OK.  I assume both the SB9 and the light ten would have the same issue.  Good to know if'n I was to buy one
M


----------



## 4GSR (Dec 10, 2017)

markba633csi said:


> Aha OK.  I assume both the SB9 and the light ten would have the same issue.  Good to know if'n I was to buy one
> M


Yeah, the 10K and probably the 10L would too.

Ken


----------



## petertha (Dec 10, 2017)

Very nice. Are you also going to turn-thread the nut, or is that a more convoluted operation?


----------



## 4GSR (Dec 11, 2017)

petertha said:


> Very nice. Are you also going to turn-thread the nut, or is that a more convoluted operation?


It's done.  I didn't write up anything on it.  Still have some mill work to do it.

Ken


----------



## NEL957 (Dec 11, 2017)

Ken 
Very nice job on the screw.
Nelson


----------



## tertiaryjim (Dec 12, 2017)

I seem to be missing something with your thread depth formula.
The book calls for  1/2 the pitch plus 0.010" thread depth for a ten pitch or coarser thread.
This would be 0.060"  for the ten pitch thread.
I understand that you used wires to get the correct pitch diameter but why do you need the 
extra 0.010" root clearance?


----------



## 4GSR (Dec 12, 2017)

tertiaryjim said:


> I seem to be missing something with your thread depth formula.
> The book calls for  1/2 the pitch plus 0.010" thread depth for a ten pitch or coarser thread.
> This would be 0.060"  for the ten pitch thread.
> I understand that you used wires to get the correct pitch diameter but why do you need the
> extra 0.010" root clearance?



Oops!

You are correct!  My wrong.  It did work.  The old screw thread was at approx. .070" deep too.  Couldn't measure it exactly.

I did check the nominal thread depth at .060" per my thread program, but when I started checking the root diameter to the major diameter with tolerance, I was coming up with a depth from .0575" to .06515-.070" deep. I added .010" to the .060" thinking it didn't already have the .010" clearance added.  So I cut it a little deeper than it should have been.  My apology for my mistake.
Here is a snapshot from my program.


----------



## tertiaryjim (Dec 12, 2017)

Since you used wires to check the thread and it wasn't a centralizing thread there shoudn't be any problems.
It's just more room for oil to flow in for lubrication.

I have seen free to use programs, like you show, on the net. They sure are nice.
They showed me a number of incorrect ideas I have of threads.
Sometime in the future I would like to make a acme tool gauge for internal threading  or perhaps a measuring tool
that uses trig to get the tool tip width ( flat ).
I was thinking a 20tpi acme could be handy, standard only goes to 16tpi, and that program gave all the information for internal and external threads,
including the tool flats.
Found a paragraph in The New Machinists Handbook 1955 edition, page 10-8, that gives a formula which uses trig and a simple measurement
to get the tool flat or another gauge that uses a depth mic. So, another project is to make a tool holder that clamps to the jaws of a dial indicator or a mic to get the measurement at a known distance from the flat of the threading tool.


----------



## 4GSR (Dec 12, 2017)

tertiaryjim said:


> Since you used wires to check the thread and it wasn't a centralizing thread there shoudn't be any problems.
> It's just more room for oil to flow in for lubrication.



Exactly!

My thread program is in the Downloads section of this forum if you want a copy of it.  I used basically the same output information that another manufacturer uses for the software they sell.  Every one of the formulas used in my program came from one of several AISI/ASME standards on screw threads, Acme, and Stub Acme threads.  And also the Federal screw thread standards, too.  All readily available for a price.  A co-worker of mine helped on the excel file contents to make it into what you see. The program will take any number of threads.  The only thing you would have to do is add a thread wire size for a 20 pitch Acme thread to get the M.O.W. to come out correct.

Ken


----------



## gi_984 (Dec 12, 2017)

Hi Ken,
Looks good.  I'm considering making a short crossfeed screw for one of my machines as well.  What are your thoughts on using 4140?  Especially on thread quality compared to threading the 1144 stress proof?
Chris


----------



## Mikelkie (Dec 12, 2017)

Nice job, I've been making screws for industry various sizes and lengths up to 4 metres and when screw cutting these i made up
split collars reamed to the required size with 1 or 2 tangential socket screws for locking on the bar and one on the side that goes between the jaws of the chuck to take the load of the cutting force, that way one does not need to over tighten thus saving scroll
overload and avoid slipping


----------



## 4GSR (Dec 12, 2017)

gi_984 said:


> Hi Ken,
> Looks good.  I'm considering making a short crossfeed screw for one of my machines as well.  What are your thoughts on using 4140?  Especially on thread quality compared to threading the 1144 stress proof?
> Chris


I think you would be much happier with the results using 1144 T,G, & P Stressproof.  Don't get me wrong, I've machined a lot of stuff out of 41xx materials and work with this grade of material almost every day of most of my life in the design work I do in my real job.  Occasionally run into a piece or two that will stress relieve itself after machining.  Mainly on long parts.  If you're look at the wear properties verses 1144, it will last longer.  The real drawback on 41xx grades, it's hard to find it with a ground OD without sending it out to a grind shop and have it centerless ground.  If you are looking at wear issues, look at using drill rod if the OD is not over 2".  It's expensive!  But will yield you with a screw that will last a lifetime.  I have on my Sheldon lathe I made over 35 years ago.  Has zero wear in the screw and maybe .005" in the nut.  Of course I keep it oiled once in a while and clean it every ten years.   I've had 3" OD lead screws made years ago out of 1144 stressproof that got very good life.  They ran in a bath of oil with a bronze half nut.  Ususally get about three to four years out of an nut on the trepanning machines they were on.  The leadscrews, well I've seen ones in near new shape that were well over ten years old and still running.  Much for the ranting.


----------



## petertha (Dec 13, 2017)

So pardon my dumb questions, but I'm so impressed with this:
- when I hear people making the lead screw nut & having to buy an expensive reverse thread tap, did you alter the tool orientation & cutting direction on like a boring bar style tool?
- on the lead screw threading, when you said you went to either side a bit for a smaller progressive bite, does that mean the threading tool advances straight in, or the compound still has some angle?
- what type of insert holder/tool did you use for both ID & OD operations
- what do you recommend for an anti-backlash arrangement on the nut, do you have a pic of that


----------



## RandyM (Dec 13, 2017)

So Ken, do you use a thread gage? And if so, what kind? I see there are the individual blades and the plate style. Any pros or cons to either?


----------



## Mark_f (Dec 14, 2017)

Ken,

All the thread calculator programs say the thread depth is .060". Where did the extra.010" come from?


----------



## 4GSR (Dec 14, 2017)

mark_f said:


> Ken,
> 
> All the thread calculator programs say the thread depth is .060". Where did the extra.010" come from?



Go to post #11. *tertiaryjim*   caught my mistake and the next few post I go thru what I did and explain.

Ken


----------



## 4GSR (Dec 14, 2017)

petertha said:


> So pardon my dumb questions, but I'm so impressed with this:
> - when I hear people making the lead screw nut & having to buy an expensive reverse thread tap, did you alter the tool orientation & cutting direction on like a boring bar style tool?
> - on the lead screw threading, when you said you went to either side a bit for a smaller progressive bite, does that mean the threading tool advances straight in, or the compound still has some angle?
> - what type of insert holder/tool did you use for both ID & OD operations
> - what do you recommend for an anti-backlash arrangement on the nut, do you have a pic of that


I'll post a picture of the threading tools I used.
And no, I don't use any kind of anti-back lash mechanism on the nut.  I always lived with slop in the screws and nuts over the years.  It don't bother me unless it's really bad.


----------



## 4GSR (Dec 14, 2017)

RandyM said:


> So Ken, do you use a thread gage? And if so, what kind? I see there are the individual blades and the plate style. Any pros or cons to either?


No gages.  I make the screw first, getting it correct to measurement over wires.  Next, I thread nut and use the freshly made cross feed screw as a gage for a snug fit to the nut.  I single point the thread in the nut.  No tap used to finish the thread.
Ken


----------



## gi_984 (Dec 14, 2017)

http://www.greenbaymfgco.com/ACME-nuts.php
Anybody use Greenbay manufacturing for ACME nuts?


----------



## 4GSR (Dec 14, 2017)

gi_984 said:


> http://www.greenbaymfgco.com/ACME-nuts.php
> Anybody use Greenbay manufacturing for ACME nuts?


Nope.  I find it easier to make your own.  Most of the ones they list don't even come close to working out for the ones I've ever replaced over the years.  Plus, an 3/4"-10 Acme is not a standard size anyone carries.  Now, I may have to eat my words.
Ken

Edit:  Green Bay does carry 3/4-10 Acme left hand.  But you got to remember, it is a class 2G fit thread.  That means it could have as little as .0069" to as much as .0363" of pitch diameter slop in the two threads.  In my book, that is too much slop in a cross feed screw to have.  GB will only offer closer fit threads upon special order.  And you know what special order means, $$$$ to get something made to much tighter tolerances.  In the home shop, a good snug fitting screw and nut can be achieved easily by careful planning.  (I forgot to take pictures of the threading tools I use and post.)
Ken


----------



## gi_984 (Dec 15, 2017)

Hi Ken,
Thanks for the update.  I expected the tolerances to be a bit on the loose side.  Please post any pictures of the milling set up, etc for the nut.


----------



## markba633csi (Dec 15, 2017)

Roton also carries acme rod and nuts, prices look reasonable but I haven't bought any.
Mark


----------



## 4GSR (Dec 15, 2017)

gi_984 said:


> Hi Ken,
> Thanks for the update.  I expected the tolerances to be a bit on the loose side.  Please post any pictures of the milling set up, etc for the nut.


Will do.  Probably be after Christmas, maybe even New Years.  I've got a full plate right now. Ken


----------



## 4GSR (Dec 18, 2017)

Here's a picture of the threading tools I used as requested.


----------



## Sblack (Apr 13, 2018)

I found the carbide threading inserts had to be run at a higher speed than you would usually thread at with HSS to get a decent finish. It certainly sharpened the reflexes! One could run upside down and backwards like Joe Pie (youtube - advanced innovations) advocates. You cut from left to right so you don't have to rush to disengage before you crash. Nice work here. I will refer back to it if I ever decide to make a lead screw. Any idea what metal alloy the original ones are?


----------



## 4GSR (Apr 13, 2018)

Sblack said:


> I........................ Any idea what metal alloy the original ones are?


12L14 and or 1213.  That's why it wore out.  Just finished up the compound screw and nut using a tap I got from one of the members. Expressline99 Paul.  He has a ebay store where he sells Acme taps and bronze, too.


----------

