Another challenge.. acme thread 3" x 20"long

Xjenderfloip · Jan 30, 2012

The request of this year so far, if i could make 3" acme nuts 20"long....in duplex.
I dont like to say no, so i said yes

, but to be honoust, with this one i have some doubt.
I made some long and small nuts before, however not this length dia ratio, it also made me wonder what the application would be, since the shafts are duplex aswell...with an effective thread length of 27"... seems like a rather strange design.

But anyway, with a thread dept of around .25 i tought about using a silent bar with extention, one that in my experience will be just a bit too long for using a profile insert.
But i might give that a shot first anyway, second option is cutting it parametric with a grooving tool, a very small one that is.

Third option might be the HSS aproach, but thinking about the very slow cuts and lots of grinding ....

At this stage we only quoted, but since this customer comes only when others said no, the chance that we get this is pretty high, even when we quoted high(ish) (12 hours a piece)

Im between hoping we get it, and hoping we dont.

Theres no special tap for this right?

Limy Sami · Jan 30, 2012

Right out of my league, but I'd like to see the answers.

little.one.der · Jan 30, 2012

The problem I've always had when trying to use damped bars to thread, is that you always have to take TONS of spring cuts. Like LOTS. At different depths of the thread so you don't encourage more deflection.

Just thinking out loud, but I've always wondered if you could get just a finishing tap. Rough out the threads on the lathe. If it chatters, so what. Then run the finishing tap through...

SND · Jan 30, 2012

All I can figure right now in 2 minutes is to support a boring bar on both ends and run the piece along, adjust the tool bit stick out. Kinda like line boring, not sure if you can set that up in a boring mill maybe. Actually, in that case if you could set it up to thread mill it in a line bore set up it would be done in less passes and no screwing around with the tool. Too tired right now to look it up. At least duplex ain't too bad, chips fairly ok.

Everything can be done, so long as you either have the right machine, or that you and the customer have a load of money to spend on it.
When it seems complicated, I think some guy was probably doing it by candle light 100yrs ago.

stumpwater · Jan 30, 2012

By duplex do you mean double lead? .25" thread height would mean a 2 thread per inch. You might be able to rip out to diameter with a grooving tool and then come back with an Acme tool infeeding on a 14.5 deg. angle. Trying to cut both OD and flank will be too much. I could do this in cast iron but it would be a pain in steel. Tighten up what ever holds the backside of your carriage down and test cut your tools on a short piece for clearance.
You're about to teach some engineer why we don't use 7:1 nut lenghts.
Good luck
Mike

Bobw · Jan 30, 2012

In my experience, custome Acme nuts cost $$$$$$$$$$$.

I didn't see a Qty, maybe I have AssBurgers. but 12 hours each, who cares about the hours. What is some other poor bastard going to quote them for?

20 inches through, not a chance in hell I'd touch that, buy me a six pack and I'll hep you bid it up.

My Acme experience's have always been "nobody wants to touch it". I've mostly just got it close and drove a finishing tap through it. Been paid well for it.........

BUT.... 20 inches of ACME nut. F.. That. If I had the through bore, and the travel to do it. First, I'd add in the cost of a boring bar to go 20 inches deep. Then I'd add in the cost of the threading bar to go 20" deep. Then, even if it was one part, I would price in 2 ginormous taps. Then I would multiply my time times 6 if I could get tubing, X20 if I couldn't.

12 hours a pop, I think that's fair, if you have the machine that can do it.

Get a tap made, get it close and then chase it. It's cheating, but it will also probably save you money.

union 'chinist · Jan 30, 2012

Where I work we have to cut similar threads from time to time. What we use them for are stub acme 2,3,and 4 lead threads for valve stem operators such as Limitorques and Movats.
The types we cut are in Phosphor Bronze and as was mentioned earlier it takes a lot of spring cuts over and over again to get out all the material. This creates a bushing which actually spins the stem in and out of a valve.

Many of the threads we cut have started showing up on a more than routine basis. For these we have picked up some custom made taps. Trust me, it is the only way to fly. Usually they come as sets, a rougher, mid cut and final cut.

Trying to bore that with any tighter tolerance is a real chore. What you have described sounds exactly what we have to deal with. It can be done, it just takes some serious time factored in. Add to it the extra leads and things can get hard to remember where you left off at and what to pick back up on. An indexer set up is nice, but you can cut off both sides of your tool and leave the indexing to the tool compound, but you probably know all that really.

You might want to make sure what you have been quoted isn't also stub length, because they have considerably different diameters than a standard acme thread. Best of luck to you.

Gerrythewelshman · Jan 31, 2012

nut

Hi Xjenderfloip ,
I cant remember if I told you I worked in Venlo and Deurne lovely country.
How many.
What material.

SND · Jan 31, 2012

I think I just thought of a way to do this on a manual lathe with the piece chucked up, so long as the spindle bore runs good, not that its the greatest way but would get it done. so we're at what... 5 ways so far.

SND · Jan 31, 2012

He said material is DUPLEX, probably 2205. Pretty much a slightly fancy stainless that chips closer to 17-4. I find it machines pretty good. Quantity would of course help in deciding what's worth setting up and how much you wanna throw at tooling.

GarlicDude · Jan 31, 2012

Gordon B. Clarke said:
Any chance your customer would accept a design change?

I'm thinking of something along the lines if making at least two shorter nuts, screwing then onto the ACME spindle and then inserting them into a special bush (which you also make to the correct length) to hold them in position for a correct full pitch. Before removing the threaded spindle each "nut" could be fastened (nut to bush) with for example one or two set screws.

It'd probably be both easier and faster That translates as cheaper

Gordon

I was thinking similar. Make two relatively short nuts, screw them onto an appropriate shaft with a tube in between the two and weld.

HuFlungDung · Jan 31, 2012

I'd not be too excited about doing this with an overhung boring bar with no outboard support.

Has this been invented yet: a hollow boring bar such as you'd use on a boring mill with the outboard bearing support. And an adjustable tool that is actuated by an internal cone ended mandrel (think: ramp wedge) kind of like a 3 point internal hole micrometer mechanism.

You'd probably want some sort of short stroke (pneumatic?) piston driving this cone mandrel back and forth between the cutting and retract positions. I suppose you'd have to stop between passes to change the stop length for the cone when it pushes the tool bit into position, to advance slightly for the new DOC.

CalG · Jan 31, 2012

Thinking out loud,

But a piloted boring bar with a bushing in the spindle bore would be mighty stiff.

The cutting tool would be fitted midway along the bar. Hmm.. that would be 1250 mm long bar at minimum. A hefty chunk in it's self.
THe tool could be clamped directly to the cross slide, with packing for center height.

The depth of cut would be made by adjustment of the tool bit with an indicator . Just like setting any boring tool.

The proof of the pudding would be in the tasting.

gorrilla · Jan 31, 2012

CalG said:
Thinking out loud,

But a piloted boring bar with a bushing in the spindle bore would be mighty stiff.

The cutting tool would be fitted midway along the bar. Hmm.. that would be 1250 mm long bar at minimum. A hefty chunk in it's self.
THe tool could be clamped directly to the cross slide, with packing for center height.

The depth of cut would be made by adjustment of the tool bit with an indicator . Just like setting any boring tool.

The proof of the pudding would be in the tasting.

This is sorta the same problem I ran across a few years ago. Food service company had a freezer door opener that used a two thread per inch pitch stub acme nut. I assume stub acme because it was quite shallow and 29 1/2 included angle. The actuator used a cut thread on the shaft and actually poured babbitt into the nut body to make the nut fit. Worked sweet till some nimrod failed to keep it greased. Then they came to us inquiring about a bronze nut. Now comes the tricky part. This thing was only about 3/4" id, and roughly 6 inches long. I ended up cutting it with a .125" wide grooving tool and sidestepping it to get the right thread width. Just kept stepping it over till the parts screwed together. Get to the depth number, make a bunch of spring passes, then sidestep with the compound on an old Cardiff manual lathe, in the compound set parallel with the Z axis. Of course the groove tool had to be custom ground to get the side angles and relief right. Fortunately, the customer just wanted it to actuate that door, a little slop in the threads made no difference. But cutting it was hairy, still. But twenty inches? Even with a 3" bore, no thanks, help yourself.

Xjenderfloip · Jan 31, 2012

Thanks for all the replies and great ideas guys, the material is indeed Duplex 2202 / 1.4462, and it was 10 or 15 pieces (i forgot the exact number, was too focussed on the part itself)

I think next week we know if we got the order, our salesman did fully understand that its a crazy design, nonetheless he quoted, but built an extra few days for experimenting/addional tooling cost, so theres some space... if they accept that is.

First step for me would be to find out why the designer made it like that on paper, ask if he realises what a challenge he created (on paper) and if possible give him the chance to discretely change his design.
Then the material choice, this long nut, without addional play between spindle and nut for special grease, being both of the same material and hardness, its begging for cold welding.

If they cant or wont change anything, i will start with a short test piece and an extended silent tool, trying out different sized grooving inserts to get an impression of the harmonics.
Theres no way im even gonna try a profile insert (maybe if it was bronze and 1/3 shorter).

Depending on the chatter and the result, i tend to think about making 1 finish tap to get to the final size.
I think thats doable for less then $2000,- turn/mill a long tap head with a hole and keyway, then send out to the grinder, and stick on a bar.
Will require huge torque tough.

If chatter is so bad that it wrecks inserts instantly, building a toolpost and trough the spindle guidance sounds like a great idea, but expensive, and adjusting a toolbit every cut is not something im waiting for when i have to make 15 of these things.

I will keep you updated!

Xjenderfloip · Jan 31, 2012

Yeah, we have a bunch of small letters in every quote

Gerrythewelshman · Feb 1, 2012

Thread

Hi Xjenderfloip,
You have a toughy.Heres my 6 pence worth.
I have produced a thread like this but like everyone 3times shorter.
donot even try it on a small machine.
The lathe must have a good spindle /bearings + the hp and more important
the drive belts must not slip(had this on a big Hitachi)
long jaws made to suit hold 1/2 way a 12" chuck +
2" dia st.st. borebar with a round carbide tool 12deg top rake (NOT FULL FORM)
with a swarf deflection radius at back as to keep the flow from the bar
a flat for grub screws (from front) to hold it at correct helix.

You will have another option with this borebar/tool you could thread mill.

in my view tapping is not an option.

RC99 · Feb 1, 2012

SND said:
All I can figure right now in 2 minutes is to support a boring bar on both ends and run the piece along, adjust the tool bit stick out. Kinda like line boring, not sure if you can set that up in a boring mill maybe.

Or mount the work on the saddle of a lathe and put the cutter between centres on a bar a bit smaller then the ID of the thread to allow for chip clearance...

Then a couple of travelling steadies if needed on the bar to reduce chatter. Or some supports like you see portable line borers use... Supports do not have to be that flash... Look at the supports used in this video... Just some generic bearings and a couple of pieces of aluminium... http://www.youtube.com/watch?v=cl_kXgxS6Fk

gorrilla · Feb 1, 2012

Xjenderfloip said:
Thanks for all the replies and great ideas guys, the material is indeed Duplex 2202 / 1.4462, and it was 10 or 15 pieces (i forgot the exact number, was too focussed on the part itself)

I think next week we know if we got the order, our salesman did fully understand that its a crazy design, nonetheless he quoted, but built an extra few days for experimenting/addional tooling cost, so theres some space... if they accept that is.

First step for me would be to find out why the designer made it like that on paper, ask if he realises what a challenge he created (on paper) and if possible give him the chance to discretely change his design.
Then the material choice, this long nut, without addional play between spindle and nut for special grease, being both of the same material and hardness, its begging for cold welding.

If they cant or wont change anything, i will start with a short test piece and an extended silent tool, trying out different sized grooving inserts to get an impression of the harmonics.
Theres no way im even gonna try a profile insert (maybe if it was bronze and 1/3 shorter).

Depending on the chatter and the result, i tend to think about making 1 finish tap to get to the final size.
I think thats doable for less then $2000,- turn/mill a long tap head with a hole and keyway, then send out to the grinder, and stick on a bar.
Will require huge torque tough.

If chatter is so bad that it wrecks inserts instantly, building a toolpost and trough the spindle guidance sounds like a great idea, but expensive, and adjusting a toolbit every cut is not something im waiting for when i have to make 15 of these things.

I will keep you updated!

Good point about the material and the likelyhood of it galling and coldwelding itself. A long tube with nuts at each end, with plenty of grease in the gap in between, would go a long way towards making this a much more doable job, and I think would help the design as far as strength and longevity as well. Some sort of bronze in place of that stainless would help SOOO much, but the overall strength might suffer a tad. Depends on exactly what they're trying to do with those screws. With a 3" screw, they're obviously trying to do a LOT!
Getting the two nuts into the ends of that tube while maintaining the lead might require a bit of thought, but it doesn't look as difficult as that 20" long id thread would be.
Good luck.

Mydrrin · Feb 1, 2012

Hmm, my thoughts would be to use like a 10 acme top notch insert on a divibe bar, 2.5" bar. Cut up half way, flank to size. Cut to full depth, flank to size. Chase with special tap if there is chatter problems that can't be dealt with.

Another challenge.. acme thread 3" x 20"long

Stainless

Diamond

Cast Iron

Diamond

Aluminum

Diamond

Plastic

Cast Iron

Diamond

Diamond

Cast Iron

Diamond

Diamond

Stainless

Stainless

Stainless

Cast Iron

Diamond

Stainless

Hot Rolled

Similar threads