Single point acme threads?

[Laverda]

I need to make an acme threaded rod for an old machine tool as parts are not available. Although I have done single point threading may times, never acme. Will be grinding the tool from HSS. Anything different about cutting an acme thread or is it the same as a regular thread? Still 29.5 degrees on the compound or ?????

 

[Technical Ted]

Set your compound to just shy of half the degree of the thread profile. Acme is 29 degrees so set it to maybe ~14 degrees since 14.5 degrees is half. Don't use 29.5 degrees.

Also, you'll have to grind your tool using an Acme thread gauge. Use the tip width notch on the gauge for the correct thread per inch. The tip width is critical as well as the angles. If you don't have a gauge you'll need to get one or rely on measuring very accurately which would be much harder than using a gauge.

Good luck,
Ted

 

[tommy1010]

What size acme thread are you trying to make. I have a variety of acme rods from older machines that may fit you needs. You could have for the price of shipping.

 

[Bobw]

The PART may not be available, but Acme rod is..

If you can get the right size acme rod, do that.. And then do whatever you have to
do to the ends. Machine, Braze, Pin etc...

Acme threads are no fun, especially on a rod.. Not so bad on a short fat part,
but long and skinny, with a lot of tool contact area is a recipe for not much fun.

 

[rons]

What about getting a brazed carbide threading bit and grind the sides for your Acme thread. Or modifying the sides of a square bit.

I modified a brazed carbide bit to make some air fittings. The profile of the bit looked like a Acme profile.

 

[YorkCNC]

As stated above, you want to get the right tool grinding gage before even starting. You can set the compound at 14 degrees or less to get modified flank infeed like you do with 29.5 degrees for a regular thread. Another option is to set the compound parallel with the spindle and use straight radial infeed, and then use the compound to clean up the flanks and get your fit right after you hit your minor diameter. This is a typical method for square threads (as far as those can be called typical these days) but I've found success using it for acme.

Then there is the issue of support. I'm assuming this is for a leadscrew or similar where it's quite long relative to the diameter. In that case the part will not be nearly stiff enough to resist cutting pressure and will need to be supported by a follower rest. Be advised that this is pretty fiddly and tedious to do.

 

[lazz]

Having cut a few Acme threads Im completely surprised no one mentioned a follow rest.
If you cut an acme thread with out a follow rest think spring pass.... followed by a second spring pass... and another and another....

A few of the local young guys have been using these folks to buy acme screws.... and at their prices I could sell my follow rest and have enough money to buy all the Acme screws I may need for the rest of my life.

 

[PDW]

Having cut a few Acme threads Im completely surprised no one mentioned a follow rest.
If you cut an acme thread with out a follow rest think spring pass.... followed by a second spring pass... and another and another....

A few of the local young guys have been using these folks to buy acme screws.... and at their prices I could sell my follow rest and have enough money to buy all the Acme screws I may need for the rest of my life.

...... wot he said. I've made *one* Acme thread lead screw in my life and I plan on never exceeding that number. Clear case of when it's better to buy than build. Let someone else have the headache.

PDW

 

[JST]

In some cases, there are features that cannot be added to a purchased screw.

I made a crossfeed screw for a Rivett 608, it had a gear integral with the screw, in such a location that one could not shrink it on or the like. It had to be cut in place, or the part made of two pieces plus the gear, which I was not willing to do, Naturally the gear was substantially larger diameter than the threaded portion.

In a case like that, one makes the part. Used Stressproof, and it worked out well. Yes, you essentially HAVE TO use a follow rest. I do not even want to think about trying to do it without.

 

[Bobw]

In some cases, there are features that cannot be added to a purchased screw.

Said the machinist, as the welder laughed.

 

[James H Clark]

Having cut a few Acme threads Im completely surprised no one mentioned a follow rest.
If you cut an acme thread with out a follow rest think spring pass.... followed by a second spring pass... and another and another....

A few of the local young guys have been using these folks to buy acme screws.... and at their prices I could sell my follow rest and have enough money to buy all the Acme screws I may need for the rest of my life.

Hey Lazz: The reason no one mentioned the follower rest is because the O.P. never said how long is the thread. That makes a big diff.

JH

 

[farmersamm]

said the machinist, as the welder laughed.

:d






Find a decent Acme threaded rod, then salvage what's on the other end of the rod, and glue 'em up. When finished you can tweak all of the runout out of the thing by careful heat shrinking (flame straightening).

Actual welding can be a no-go if'n the steel ain't weldable. Also...…….welding creates a ton of heat, which can really ruin stuff. And welding is destructive. Braze welding doesn't substantially alter the part.

My theory...………… If it's made of unobtanium, you do the best you can to make it right. Can't get too much "broker" than it was.

Btw...….a good braze weld has up to 65K tensile strength.

 

[thermite]

posted by JST:
In some cases, there are features that cannot be added to a purchased screw.

Said the machinist, as the welder laughed.

Said the "Mama San", as the girls just giggled....

 

[Laverda]

The shaft is indeed a lead screw (still in machine so no exact measurements yet) and is 1/2" X 10TPI and about 3' long. About 4" on each end is not threaded and then at the very end about 1/2" has threads for the hand wheel. Entire length has a 1/8 wide key way. So again I know how to single point but never have done acme. I looked at McMaster and they have precision threaded rod but will still need to make the correct ends and weld or pin to the threaded part. So I think I am better off just making it from scratch. After that I need to make the acme nuts but that is easy with a tap.

 

[thermite]

The shaft is indeed a lead screw (still in machine so no exact measurements yet) and is 1/2" X 10TPI and about 3' long. About 4" on each end is not threaded and then at the very end about 1/2" has threads for the hand wheel. Entire length has a 1/8 wide key way. So again I know how to single point but never have done acme. I looked at McMaster and they have precision threaded rod but will still need to make the correct ends and weld or pin to the threaded part. So I think I am better off just making it from scratch. After that I need to make the acme nuts but that is easy with a tap.

Three feet of skinny 1/2" steel, an Acme formed, high-drag Carbide insert, not even a skinny HSS shearing-action nibble-luncheon to gradually "generate" the shape, and your first, ever, go at single-pointing this thread-form, on a 1970's vintage Taiwanese Victor 1640G that two years ago was giving you grief as to surface-finish on SHORT 5/8" conventional threads??

"Better off" just how?

The Acme is more likely to make YOU nuts than the other way 'round!



No extra pay for demonstrating you can stand a beating. Perhaps after wasting more than one go at it, yah?

Have somone running a video so you have a record of just how long, skinney s**t goes pear-shaped right about 18 inches in as the de facto if not also de jure noodle climbs right up over the top of the cutting tool and starts to squirm atop it like an Earthworm in a puddle of gasoline. DAMHIKT, either.

I'd buy it, then modify it.

Needs a keyway? I'd ORDER it that way as well. Three-foot run, half-inch stock, dead-nuts aligned, is a lot to ask off an old BirdPort mill and wotever you have for workholding.

My Quartet's 48" overall, 42" "working" inside the cutting-oil gutters table only HAS 30" of traverse, can put EITHER of a horizontal or vertical head over it. I get a wild hare, I can line-up FIVE 6" Gerardi modulars on it, too. Drawerful of Vee-blocks, clamps, etc.

Still not good enough for 36" in one go.

A BirdPort may have a 42" table. But does it have 36" of travel? With no table sag or deviation along it? One of those is not there.

Do only the bits one CANNOT "just buy". Challenging enough as it is, those are.

 

[muckalee]

I like your approach. If I was doing this. I would use a box guide instead of a follower rest. I would use an insert for the correct Acme thread. I would practice on a same size, same material scrap. Practice cutting the thread to size, certify and log dimensions. Practice cutting the keyway. I would cut the keyway in the lathe, so the box guide must allow for this. I missed what material you were going to use.

 

[eKretz]

Hey Lazz: The reason no one mentioned the follower rest is because the O.P. never said how long is the thread. That makes a big diff.

JH

If'n I had to lay a wager I'd say it's more likely that none who replied before Lazz have cut a long acme thread. With the updated info, this would be an absolute nightmare without a follower rest. I've cut a considerable pile of Acme threads; the short ones are pretty easy. The long ones at a hefty enough diameter are pretty easy. The long small diameter ones are a whole different ballgame. At this L : D and without a follower rest this shouldn't be attempted IMO. This particular example will be like a wet noodle in terms of stiffness/rigidity.

Purchase the ready made screw and add your features. And be prepared to straighten it afterward if you're going to cut a keyway all the way down one side.

 

[HuFlungDung]

Your best bet for machining an Acme thread is to begin with a grooving tool that is as narrow as the root width of the thread. It only cuts on the front, and you proceed to grind it with proper side clearance so it doesn't drag on the leading edge. After you have the groove cut to depth, then you can use your Acme form tool. I'd start with a tool narrower than the gage says, and again, cut only one flank or the other, not both at the same time.

Never cut all three sides of the thread at the same time. You can use a full form tool as a gauge to tell when your thread is complete, but it really isn't much good to cut the thread with unless you are machining bronze or brass or cast iron. You want a good finish on the flanks of a lead screw, and you need a custom finishing tool for each side of the thread because the top rake should be different for each flank to help with chip flow. A plain flat top tool will make a nasty finish.

Yeah, you'll have to fool around a lot with a follower rest. The technique I outlined tends to not raise a heavy burr on the outside of the bar as much as 3 sided cutting will. That burr formation will fuck up your follower's following action, as the burr will push the bar away from the rest and into your tool, followed by unpleasantness.

Cutting a full length keyway may warp the bar, too. So be prepared to straighten it.

Use a nice free machining steel like stressproof or equivalent.

Acme threads are not that bad to cut, considering that they are relatively shallow for their pitch. Like a 4tpi V thread is a monster to cut compared to a 4tpi Acme, especially when it comes to making the nut.

 

[Technical Ted]

I would suggest making the nut first so you can use it for a gauge when threading the screw. If you make the screw first and the tapped nut doesn't fit, you'll have to put the screw back in, align your threading tool and take a little more off... not the best way to go. Or, maybe the screw will be too sloppy...

Do the nut first.

Ted

 

[farmersamm]

It's just flat crazy to mess with threading the rod. Geez!!

1/2 x 10tpi is available on Fleabay for almost a pittance, and it's quite accurate.

Bronze is available for a bit more, actually a LOT more. You can also score your tap on the same site for a reasonable price.

Why make it harder than it is. It's gonna take a bit of skill to make your part with off the shelf parts.

All's ya want is a serviceable lead screw, and nut.




Started with this.....





Harris low fuming bronze rod is the filler metal of choice. Relatively low melting point with a good buildup.

Flux your bare steel, then butter it up. Let the butter coat cool, then use a small tip to add subsequent layers. You do not need to flux after you've bonded your first pass, you'll simply be adding layers to bronze. Just get it hot enough to wet in.