Threading right up to a shoulder - ideas?

[SRT Mike]

If you see the file I attached, it helps explain

The cylinder has a recess that is 6mm deep and it's made from aluminum. There is a part that goes into the bottom of that recess and is 2mm high, leaving 4mm space above.

That plug that's sort of mushroom shaped - the top part is the same OD as the cylinder and the bottom smaller OD part will screw in.

I don't have a ton of room to work with (4mm of thread area). I can use any thread I want, but i want to get the thread as close to the shoulder in the plug part as possible. The cylinder recess is 6mm deep, and I can overshoot the thread to ensure the entire first 4mm is threaded completely... but I can't do that on the top.

If I use my generic 60-degree laydown threading bit on the plug, and cut a fine thread, I am not really going to be able to get all that close to the shoulder.. I am not at work right now but I bet I can only get within maybe 2mm of the shoulder with an AG60 threading bit.

I thought I had seen some full form threading inserts that let you go right up to the shoulder - they extended out slightly beyond the end of the toolholder.

Or, if I got a full profile insert made for a fine pitch thread, wouldn't the actual cutting tip triangle be a lot narrower, allowing me to get right up to the shoulder?

Or does anyone have any suggestions on how to do this? I know more threaded area would be ideal, but I am very constrained on the length and dimensions of this part so what I have here is all I got to work with. Any suggestions are welcome

[Geof]

Originally Posted by SRT Mike ......Or, if I got a full profile insert made for a fine pitch thread, wouldn't the actual cutting tip triangle be a lot narrower, allowing me to get right up to the shoulder?...

Right up to the shoulder may be optimistic but within half a pitch may be possible.

I think the full profile insert is the way to go, I have had similar parts and that is what I have used.

[One of Many]

I've often used a thread relief in the cap or a counter bored thread relief in the barrel, one thread pitch wide, but 1/2 thread pitch relief in each side can work. The finer the thread the better of course.

DC

[neilw20]

It is a manual gadget called snap tap or something like that.
The label has long since worn off.
It works like this:
There is a tool holder that can slide away on another track.
The toolholder is held in position in the track by a spring loaded ball that reacts the cutting force.
The track is at 30 degrees on the topslide.
It is attached via a pin and a link to a sliding stop mounted on the bed near the tailstock.
As the tool is threading towards the face (really fast is OK too !) just when the tool gets to the face the link pulls the tool away from the job, in effect instantly stopping Z movement of the tool which then translates to a +X move parallel to the face of the job.
Now the tool is clear of the job the carriage moves back towards the tailstock and the link hits a spring stop and restores the tool back into the spring loaded ball position ready for the next cut.

When used on internal threads it is mounted at -30 degrees and retracts in a -X direction.

I am sure this could be adapted to CNC, but I think you can do it with a CNC now as long as the spindle speed is slow enough.

Naturally the tool must be such that it can go right up to the face.

You could always thread mill it instead.

Another way is to start at the face and cut the thread towards the tailstock running in reverse with the tool upside down.
This is how I do internal threads from a blind face.
Just use low enough RPM so that the Z axis can accelerate instantly to the required pitch.

[SRT Mike]

Thanks for the info gents.... 1/2 a thread pitch would be close enough.

I have also often used a groove at the top of the thread for relief, and I'll maybe put a relief groove in the cylinder base part, because putting it there I can do with a boring bar and very precisely control how deep the relief is (whereas if I do it on the plug, I would use a grooving bit and they are fixed widths).

That spring loaded threading tool sounds neat too!

I'll give the full profile insert a shot and see how I make out - hopefully will succeed!

[neilw20]

Running in reverse from a groove is trivial once you mount the tool upside down and remember to run the spindle in reverse.
You don't have to worry about making the groove. It will just happen as you feed in X pass by pass.

[g-codeguy]

AG60 = .059 distance from side of insert to centerline of point.
A60 = .035 for same dimension
32UN = .020 for same dimension.

One thing to realize is that a slower RPM will allow the insert to get closer to the shoulder before starting to pull out. Unless you use 00 in the 2nd pair (for G76 2-block call) which will leave a ring next to the shoulder. Use 01 to pullout over the shortest distance.

[msomerville]

If you needed the two pieces to shut off against each other I might consider a short bore that is just bigger than your thread diameter.

[juergenwt]

Mike - you are not giving us enough info. How many parts? What dia is the thread? It looks like a small thread.
First - since the part is metric I would stay with a standard metric fine thread.
Second - for the inside thread I would make an undercut and than cut from the inside out - or - I would try to find a metric standard fine tap. Buy two and grind one of them flat bottom going. Start with the first one and finish with the second one to the undercut. Don't forget to put a nice chamfer in front.
For the plug - you can cut as close as possible with a tool bit having a small tip.
You take a regular tool bit like a 5/16 x 5/16 and on the left side grind a 30 deg angle almost to the front. Than tilt another 30 deg. and grind to a small tip ( you can make a tip just slightly larger than the depth of your thread). You will than end up with a 60 deg. tip. Grind your clearance by hand.
Set compound to 29 1/2 deg and align the left ( first ground) angle with the face of your spindle or 90 deg to the thread. Cut to an undercut. The chamfer on the internal thread will help you - or - buy a die, cut with one (the chamfered side) and follow up with the other side of the die that is almost a sharp full thread. Check the die and make sure it has one side with a chamfered start and the other side starts with a thread that has a very short chamfer.
If you can not find one - grind one side. Juergenwt

[SRT Mike]

Originally Posted by juergenwt Mike - you are not giving us enough info. How many parts? What dia is the thread? It looks like a small thread. First - since the part is metric I would stay with a standard metric fine thread. Second - for the inside thread I would make an undercut and than cut from the inside out - or - I would try to find a metric standard fine tap. Buy two and grind one of them flat bottom going. Start with the first one and finish with the second one to the undercut. Don't forget to put a nice chamfer in front. For the plug - you can cut as close as possible with a tool bit having a small tip. You take a regular tool bit like a 5/16 x 5/16 and on the left side grind a 30 deg angle almost to the front. Than tilt another 30 deg. and grind to a small tip ( you can make a tip just slightly larger than the depth of your thread). You will than end up with a 60 deg. tip. Grind your clearance by hand. Set compound to 29 1/2 deg and align the left ( first ground) angle with the face of your spindle or 90 deg to the thread. Cut to an undercut. The chamfer on the internal thread will help you - or - buy a die, cut with one (the chamfered side) and follow up with the other side of the die that is almost a sharp full thread. Check the die and make sure it has one side with a chamfered start and the other side starts with a thread that has a very short chamfer. If you can not find one - grind one side. Juergenwt

Thanks for the info!

How many parts - well it's a new product we are doing, so I will be running these in batches of 200-400pcs at a time.

Compound? Cross slide? What are those? I'm making them on a CNC lathe... but a few folks and you have suggested threading from the inside and moving out... may I ask why? I've never done that, will I get a better finish or something? Or is that relevant on a manual machine to ensure you get right up to the shoulder?

The thread can be anything I want, I was thinking to use a very fine pitch thread to give as many threads to contact as possible, maybe a 48 pitch or something.

I have a laydown threading toolholder (ID and OD) so I was thinking to get an insert that will fit on that, like a full profile UN-48tpi and see how it works... if it doesn't, I can go from there. I will be sure to put a chamfer on the front lip - thanks for the tip!

[Geof]

Originally Posted by SRT Mike .....The thread can be anything I want, I was thinking to use a very fine pitch thread to give as many threads to contact as possible, maybe a 48 pitch or something.....

There is a bit of a play off here; if you use a fine thread you need to keep tighter tolerances simply because you do not have as much thread depth to play with.

If the plug has to screw tight against the end of the tube you either have to slightly counterbore the tube by about 1-1/2 threads or put an undercut the same width on the plug.

I will be contrary to the suggestions to thread from the inside out. On a right hand thread I don't think there is any particular advantage but there may be a disadvantage. Depending on your machine you may need a bit of free travel to all full synchronization between the rpm and feed; you can get this by starting a few pitches ahead of the part threading in but if you thread out you don't have an free travel.

[SRT Mike]

Originally Posted by Geof There is a bit of a play off here; if you use a fine thread you need to keep tighter tolerances simply because you do not have as much thread depth to play with. If the plug has to screw tight against the end of the tube you either have to slightly counterbore the tube by about 1-1/2 threads or put an undercut the same width on the plug. I will be contrary to the suggestions to thread from the inside out. On a right hand thread I don't think there is any particular advantage but there may be a disadvantage. Depending on your machine you may need a bit of free travel to all full synchronization between the rpm and feed; you can get this by starting a few pitches ahead of the part threading in but if you thread out you don't have an free travel.

Good thinking on the thread starting on the outside to let it sync right with the spindle, I hadn't thought of that but it makes perfect sense.

I was planning to put as short a counterbore at the top of the cylinder as possible, so I can maximize the # of threads in contact. I've had good luck with an AG60 partial profile threading insert for threads up to 32TPI - I'll try the 48tpi and see how it comes out. My main concern with the fine threads was getting a nice V profile on the threads so they mate nicely. I'll give it a shot and see how I make out.

Thanks!