Making a new Cross Slide Acme Screw

[Tex-VA]

Fellow lathe operators - I plan to photo and document my remake of a South Bend 9" / 10k cross slide acme screw. I have made these successfully in the past. I know there may be better methods to make this part but bear with me and we try to get a usable one finished. I will start with grinding the acme bit and finish with it on a lathe if all goes well. I hope anyone that knows of better methods for doing this project will ad in their advise and we all can learn something new.

I ground an acme bit today and I will start here.
First, a quick word about bench grinders. They can be very dangerous tools. If the wheels get a crack in them, can break up due to there high speed and I have heard of users being injured badly or even killed. A grinding wheel can have a flaw from the manufacturer. The way I have been taught to test for this is to hold the by one finger into the mounting hole and light raping around the circumference. You are suppose to listen for dead sounds that would signifies a crack or void. The other things that can go wrong are dropping the grinder or hitting the wheel while the wheel is mounted on the grinder. The other thing one needs to avoid is grinding soft material like aluminum, brass, bronze, and etc. What happens is the soft material melts a bit and gets into the wheel and then the grinding heats up metal, it expands and cracks the wheel. Under the worst circumstances the wheel explodes with a lot of force. I have used as a rule of thumb, never grind any non-ferrous metals. Also use salty glasses and do not ware gloves.


The first photos are the set up of the miter gauge on the table of my grinder. I used a rectangle of aluminum that I held up to the miter so I could get the bit at 14.5 degrees.
The grinder is a 8" Ryobi that I bought at Home Depot for under $60.00. The table is a “Grind-R-Table” made by the Glendo Company. http://www.accu-finish.com/
I have the rig set up on a board so I can move it around the shop.
I set the table at about 4 degrees using the gauge on the side of the table angle gauge on the side of the table bracket. The blank bit is .250 HSS Cobalt and I ground it free hand on the table till I got it close then used the miter gauge to bring it to the 14.5 angle.

The 2nd photos are of grinding the bit with the fine wheel and testing the angle with the acme thread gauge. I should mention, I could not photograph the work while I was grinding and I don’t show it but I have a tuna can with rust-lick to use as a dip pot to keep the bit cool. You can ruin the bit if you get it too hot and burn it.

I'll post more soon.
Tex

 

[Tex-VA]

The 3rd set are grinding the flat on the tip and using the acme thread gauge to get the size right go 10 threads per inch.

 

[Tex-VA]

More grinding acme bit

The last photos are of the bit and gauge and the diamond hone for stoning the final edge.

About 20 years ago, my shop teacher in the Fairfax County Adult Education machinists class, Harry Harps, showed us how to grind bits with out the miter table. He just rested the blank on his finger and got great results. He said you get a much better bit that way because all of the vibration is absorbed by your finger. I don’t have the skills to use that method yet.

I hope this helps and inspires some of you, please let me what you think.

The next posting will be cutting the acme thread on the lathe.
Tex

 

[enginebuilder]

WHere did you get the "grinder table" ?
I like it.
Jim

 

[Tex-VA]

"grinder table" ?

Hey Jim - It came fro the Glendo Co. They advertise in "The Home Shop Machinist". They ran a promotional sale many years ago and bought one. I have seen plans for making one but I can't remember where. I have included a link below. Tex

http://www.accu-finish.com/

 

[abarnsley]

Looks good but I don't see Relief for helix of thread

I don't see the different angles needed on sides..

Tool should be ground either Left or Right handed, so bottom of tool does not rub on thread.

I made one 15 years ago, turned out nice, follower rest use mandatory

Super smooth and sharp bit (that dimond hone should do it )

 

[Jerald MI.]

Good info, thanks Tex-Jerald

 

[Tex-VA]

Re: Looks good but I don't see Relief for helix of thread

I don't see the different angles needed on sides..

Tool should be ground either Left or Right handed, so bottom of tool does not rub on thread.

Hello - I plan on using tool holder that holds to bit parallel to the cross slide. This makes grinding the bit much easier than with the lantern or rocker tool post with bit holders. The sides of the cutting end of the bit are 29 degrees / 14.5 degrees each side to match the acme thread (////////////////). The angle of the .4375 10tpi acme thread is 4.161 degrees. So by my calculations then, anything over that should work and not drag on the thread. I approximated 4.5 to 5 degrees. I just drew this out in my cad system, to make sure, and it looks like it will work. This bit should cut both right and left handed 10tpi acme threads. I did grind a bit, a while back, for the old lantern / tool holder type and that use complicated angles. This is much easier to do. This method of grinding the bits has worked for me before but may be I was just lucky. I'll try cutting the thread as soon as I can get the blank shaft turned. We'll see then. - Tex

 

[jim rozen]

You could also consider purchasing the precision
leadscrew stock from a board member, swells.

It's nice stuff.

Jim

 

[Greg White]

Please ,go on with your story!!!
A sailor from the Viet Nam war usta cut acmes like there was no tommorow,he helped fix alot of our machines,yep.Doug McIntosh was his name.
De Vlieg jig mills usta have a odd lead screw,he spotted (fit)the tool bit to the shaft,made new nuts,what a blessing.
J.R.could you post a link or something to this Swells fellow???
Respect
GW

 

[Jerald MI.]

http://www.wswells.com/index.html



Watching this post with great interest.-Jerald

 

[mendoje1]

Also watching with great interest. Finally learned how to use that ACME thread guage which has been sitting in my toolbox

Jeff

 

[mwhat]

cant wait to see the next step

 

[Tex-VA]

Re: Cross Slide Acme Screw

I finished up the threading today. It's taking much longer that expected, taking notes and photos slowed me way down. I will try to get the work that I have written up and up here tomorrow. I'm about half way done with the lead screw. I plan to make the lead screw with a larger mic dial and I will show all of that. The only things I'm not going to make is the thrust bearings (I can buy them) and the ball handle (we work on that later).
Also, I find, I'm not happy with my camera. It's a Nikon CoolPix 4300, and has good resolution but I can't control the point of focus the way I would like. I used a Nikon FTN in my youth, years ago, and I still have one but I 'spose chemical photography is dead and I no longer have a darkroom. I was looking the small Nikon single lens reflex D-40. Do any of you all have any suggestions? Of course, it's nerve racking to shoot photos the bit cutting the threads being you have to take you hand and attention off the lathe. There is no camera the can help me do that. I'll try to get back Sunday. Tex

 

[Tex-VA]

Making the Cross Slide Acme Screw

Yesterday I completed the .4375 10tpi LH Acme threads for the SB 10k / 9" cross slide screw. The first thing I did was cut a piece of .875, what was supposed to be 12L14, a little over 15" long. The finished lead screws over all length is a little under 13.625" and I will need an inch or so to sacrifice on the threaded end so I can use the follow / traveling rest. That will be shown latter. The length of the screw doesn't have to be exact, there is a good bit of tolerance here. The other side, with the handle, will have to be "spot on" in a few places because of the use of thrust bearings and the a dowel pin to load them. I deal with that in a few days.
I put the blank into the 3 jaw chuck on my South Bend 10L lathe, faced and center drilled both ends. I took photos of just about all of the procedures but I'm am only going to concentrate on the high lights so I'm leaving out the basic things like facing and center drilling. One thing I would like to mention is to use a small center drill.
The first long cut is on the handle end. The measurement from the start of the drive gear and the handle shaft is approximately 7", so I needed to have about 8" of blank coming out of the chuck. The cross slide gear is 12 tooth 20DP which has a diameter of .700. I will finish that later so I cut the shaft down to .750 at a length about 7.750 inches. After I finished that cut I measured loosely 4.125 from the tail stock end and set my saddle stop to make that cut. The diameter do the handle end is .375 but for now I will cut it to .550. I need to make it so it will fit into my small Bison 3.250 chuck. You will see the need for that when I cut the gear. Neither of these need to be precise as they will be finished later.

The first 2 photos are the cutting of the handle end and the small chuck with the 5C adapter I made. Also you can see the problem I had getting a good finish on the steel I don't know what it is but it's not 12L14 (bad ebay purchase). To get a good finish I had to hone my bits and take a light cut. That leaves smooth but dull finish. Scotch bright pads bring it right back. By the way, I all ways cover the lathe bed when I use any abrasives on the lathe.

I have now attached the small chuck on the lathe and put the blank in the chuck with at least .500 between the end of the gear and the chuck jaws. The gear blank will have to be cut later. There is no need to cut it now, I will concentrate on the threads. The shaft needs to be .4375 so I cut that first. Then I cut down to a diameter .300 about an inch long at the tail stock end for the travel rest.

The next 2 photos attempt to show that.

I need to start another post to ad more photos.

If anyone would like the cad / dfx drawings of the screw, please email me at altex "at" cox "dot" net and I will send it to you.

 

[Tex-VA]

Set Up for cutting the Threads for Cross Slide Acme Screw

The last cut before setting up the acme bit is to cut a grove for starting the threads. I just hogged out a little with a cut-off tool. I cleaned it up later.

The second photo here is of the tool post and the bit I ground earlier. The tool holder I used is one that I made about 20 years ago in adult ed shop class. I was a required project but has turned out to be quite useful. I added the wedges under the bit for adjusting the hight of the bit to the plans, they called for using shims. I like to add my own touch to what I make. Many of my shop friends also do this, I guess it's like fixing up a hot rod, a motor cycle, or even your guitar. Making guitar parts is how I got into machining.

http://i260.photobucket.com/albums/ii1/Tex-VA/8Acme.jpg[/IM

The next 2 photos are using the acme thread gauge to get the bit square to the stock. The bit needed to have the top on the center line of the lathe and the compound rest set to 14.5 degrees before I did this. You can also see how I set up the travel rest and the tool tool holder set close to it. Note the live center, I used the one from my SB cnc lathe. I has a longer nose.

[IMG]http://i260.photobucket.com/albums/ii1/Tex-VA/10Acme.jpg

More to come:

 

[Tex-VA]

More on making the Cross Slide Screw

Next photo is of the South Bend threading stop. I set both of the micrometer dials to 0 with the bit touching the stock. Then I adjusted the thread stop to stop the cross slide screw to 0 by backing the compound out about 1/2 a turn. Once the stop is set then I retested to compound dial by touching the stock and resetting the micrometer to 0 if needed. I always check the dial before making the cut because the stop can be a few thousands off. It saves a lot of time and mistakes by getting you close.

The next 2 photos are of beginning to cut the thread. I installed the travel rest, I don't think I mentioned it before, but I found I needed it to get an even thread depth in the middle of the screw. The two fingers on the travel rest need to be snug, but not too tight, on the work. I set the gear box at 10 threads per inch and have the lead screw going backwards or in reverse. The spindle was put in back gear, set to the slowest speed. The saddle will travel from the head stock to the tail stock with the spindle going forward or counter clockwise. I set the carriage stop where the bit will start in the grove I had cut earlier. I advanced the compound .010 for the first cut. I covered the bit and the stock liberally with thread cutting oil using a small brush. I turned on the motor and using the thread dial indicator I engaged the half nuts when a line on the thread dial indicator comes around and matches the witness line. You can use any line when cutting even number of threads. I disengaged the half nuts when the bit comes to the end of the cut. The travel rest ends up over the "nub" that I cut at the end of the shaft. You have to stay on the ball here, even at the slowest rpm, it seems to speed up when it gets close to crashing.

I disengaged the half nuts after the first cut. I then backed off the cross slide so I could bring the saddle back to the beginning of the cut at the carriage stop. I found I had to use a chip brush to remove the chips from the screw to allow the travel rest to smoothly return. This unfortunately removed most of the cutting oil which I had to re-coat for every cut. I repeated this process, advancing the compound incrementally before each cut.

Next I will list the cuts I made and the amount of advance of the compound:
The depth of cut on the micrometer dial with the compound set at 14.5 degrees for the .4375 10tpi acme thread is, by my calculations, .062. The below list is how I got there.

1st cut .0100
2nd cut .0100
Now I started to lighten up the depth
3rd cut .0075
4th cut .0075
Here I will take a couple of passes with no compound advance to get the thread cleaned up.
5th cut .0000
6th cut .0000
I started advancing the compound again.
7th cut .0050
8th cut .0050
9th cut .0035
10th cut .0035
Another clean up cut
11th cut .0000
12th cut .0025
13th cut .0025
Another clean up cut
14th cut .0000
Now I gently filed the edge off the threads then move the tail stock back so I could test the thread. That will be shown in the next post. I had to careful not to change the set up. The nut started but it was a little tight so I brought the tail stock back and took another cut.
15th cut .0025
16th cut .0000
17th cut .0000
Clean up again and test.

 

[jim rozen]

Wow. I think you qualify for an honorary 'diamond' rating here.

Cold rolled steel

Home-ground acme threading tool

Left hand threads

Follower rest

Yep this is hall of fame stuff.

Jim

 

[Tex-VA]

Finishing up the threads

This is a photo my first test of the threads.

The cross feed nut felt a little too tight so I needed to take a few more small cuts, file, and test again

The nut went on smoothly so now I can brake down the threading set up. I still need to leave the work in the chuck because I need to get the gear to the proper diameter.

I will try to get the gear made tomorrow and I will show how I do that.

I would like to thank all who stayed with me so far in doing this. A good friend, Charles Keeney who bought my 9" SB lathe, stopped by this afternoon to have me look at a tool he was having a problem with. I ask him to proof read the post before this one. He found many, hopefully small, mistakes that I corrected. I would like to ask that if anybody has been confused or felt I've left out something with my postings on making the cross feed screw to please reply here and I will try to make it clearer. I'm a fair machinist, I can get things done, but not such a good writer. I'm working on that.

 

[Jerald MI.]

Tex-I think most of us can understand w/o difficulty the information you are sharing. No need to worry.

This is a great thread-Jerald