Turned spherical parts- help

[James Green 2Participant @jamesgreen2]

Looking to have a small batch of parts turned for project.

[James Green 2Participant @jamesgreen2]

HI All, Im looking for a small batch of parts to be turned for a project i am currently working on. Qtyx8-16 the big CNC and prototyping firms are turning me away due to volume. Any advice on people or places that could help me. the parts are small (for spectacles) ideally stainless but would be happy with brass.

Thanks in advance!

James

[John HinkleyParticipant @johnhinkley26699]

If you only want the spheres made, have you considered ball bearings? A picture of the part would probably elicit more useful suggestions.

John

[James Green 2Participant @jamesgreen2]

Hi John, thanks for the response. please see image below. im open to simplification suggestions particularly as this is a prototype.

Many thanks , James

 

[Nick HulmeParticipant @nickhulme30114]

Are all the threads full profile right up to the shoulders?

[James Green 2Participant @jamesgreen2]

Hi Nick,

Thats not necessary if it simplifies manufacture.

All the best,

James

[JohnFParticipant @johnf59703]

James, looking at the drawing there is no dimension for the sphere but it looks to be around 5-6 mm ?

For the small quantity you require I would make this with a form tool dependant on the accuracy you require, no tolerance's are given. You can make a form tool that's suitable for brass from carbon steel, gauge plate works well, first drill, ream, bore ? a hole in the tool the size needed with the hole angled to give the required cutting clearance then cut off half the hole, harden and temper. Sharpen with a slip stone on the top surface, prior to hardening you can increase the clearance with a small stone or burr in a Dremel type tool or even by hand. I have used this method many times for small batches of items.

Making the parts I would turn and thread one end then form the sphere, next plunge in with a parting tool to rough the second thread then part off. Now make a split holding fixture to locate on the 1st thread and the sphere, turn and thread the second thread. Another jig will be required to D & T the centre hole in the sphere.

Hope this helps John

[James Green 2Participant @jamesgreen2]

THanks John,

This is great detail and if i decide to go down the road of making it from scratch myself this is certainly the approach I will take. I will be sure to let you know how this goes if this is the best option.

All the best,

James

[Anonymous]

Posted by JohnF on 09/10/2017 23:06:07:

James, looking at the drawing there is no dimension for the sphere but it looks to be around 5-6 mm

Odd, the drawing I'm looking at has a dimension giving the radius of the sphere as 2.5mm?

Andrew

[James Green 2Participant @jamesgreen2]

2.5 radius is what I'm hoping for but would consider changing that slightly if it made manufacture easier to achieve

[Chris Evans 6Participant @chrisevans6]

They are doable but a real faff to make. A fair bit of time involved making things up to hold them for secondary operations. More of an instrument makers work than a CNC jobbing shop. I did once come across a CNC turner in Walsall West Midlands that did really small items for the "Body Piercing" trade. They where next door to a bearing supplier I used, not been that way for 15 years or more though.

[JohnFParticipant @johnf59703]

 

Posted by Andrew Johnston on 09/10/2017 23:26:30:

Posted by JohnF on 09/10/2017 23:06:07:

James, looking at the drawing there is no dimension for the sphere but it looks to be around 5-6 mm

Odd, the drawing I'm looking at has a dimension giving the radius of the sphere as 2.5mm?

Andrew

Hi Andrew, yes you are quite correct — it was late and missed that ! Cheers John

James — what tolerance do you need on the 5mm diameter? If its the sphere you need it makes no difference to production regardless of size [within reason !] 

Edited By JohnF on 10/10/2017 09:35:36

[JasonBModerator @jasonb]

Don't know if it really needs any jigs for a second op.

-Face stock and form one of the 1.6mm spigots and thread

Form tool 4mm wide to shape shere

Remove from lathe and holding by rest of the stock drill and tap M2 hole

Back into lathe, cut other 1.6mm spigot with parting tool then part off

Thread the remaining spigot M1.6 by hand, easier to hole diestock still and rotate the part by hand, M1.6 onto brass does not need much effort. Or could put a M2 screw into the cross hole to give a bit more to get hold of.

Edited By JasonB on 10/10/2017 09:41:49

[opochkaParticipant @opochka]

Will be a real struggle trying to form that ball.

Easier to buy brass balls ready-made.

https://simplybearings.co.uk/shop/Loose-Balls-&-Rollers-Brass-Ball-Bearings/c23_5014/index.html?page=1

The real struggle will be to get the holes perpendicular.

[Nick HulmeParticipant @nickhulme30114]

It's not a dificult job, even for a beginner, provided the requisite care and enthusiasm are available

I'd turn and thread the spigot on the front of the stock first.

Second I'd form the ball and turn the rear spigot section, slightly over length and 4mm OD, then part off over length.

Repeat first and second steps for a few more parts than required .

Third I'd use a custom machined split "collet" holder with a single slit to hold and align the part concentric for turning and threading the other spigot, aligning on the thread OD but gripping the spherical surface.

Repeat third step for all parts.

If a cross slot is machined in the front of the holder to accommodate the spigots to slightly more than half their diameter it will grip the sphere for boring and threading the hole in the sphere on all parts.

This way there is no fiddly setup, everything is automatically concentric, you aren't locating and fixing with a small thread and you can work in steel almost as easily as brass

 

– Nick

Edited By Nick Hulme on 10/10/2017 12:18:57

[JasonBModerator @jasonb]

The ball will be easy to do with a form tool, just like this bigger one.

Put the M2 hole in while still on the parent stock and it will be easy to hold so Hole will be perpendicular

J

[James Green 2Participant @jamesgreen2]

THanks, everyone

The photos are great Jason, thats great advice. I dont currently have a lathe. but if I go down this route I'm sure i can find access to one for a few days. Currently I am hoping to find someone who is set up to make these, instrument makers seems like the best option following this conversation

[EmgeeParticipant @emgee]

Jason

Did you use centre support when plunging the ball cutting tool ?
I am not sure the 1.60mm finish diameter required will stand the force if using the same method.

Emgee

[JasonBModerator @jasonb]

Emgee, If you look at my post @9.40 I suggested doing the ball before cutting the 1.6mm dia nearer the chuck. This woul dleave the ball supported on a 3mm dia shaft which I think would be OK. If not simple female ctr on the 1.6mm dia would help.

I did not use end support when I did the 9/16" dia ones in the photos as I did not want a hole where the valve spout was going.

James, it was mentioned above about making the form tool by drilling a hole in some gauge plate, this pic shows such a hole and my marking out for the rest of the shape, may make it clearer for you to see how the tool is knocked up.

[Howard LewisParticipant @howardlewis46836]

The intriguing bits are thread diameters, 1.6mm diameter of the right and left hand threads, and a 2.5mm internal.

Seems like neither fish nor fowl to me, not being 1.5mm or 1/16 inch diameter.

Have not looked to see if anyone offers taps for 2.5mm, and if available, should be interesting making a thread to the bottom of a blind hole. The taps, would need the point grinding off; completely for the bottoming (plug) tap.

The threading would cause me more concern than turning a sphere.

Are the thread sizes sacrosanct?

Howard

[Anonymous]

If we assume metric threads then M1.6 is a standard size; 1.5mm isn't. Likewise I assume that the hole specified as 2mm really requires an internal M2 thread. However finding taps for 2.5mm shouldn't be a problem, M2.5 is also a standard size.

For what I assume is intended to be a production item the drawing is lacking a huge amount of information, some of which Howard has pointed out.

I note that the OP prefers stainless steel, but everyone has concentrated on brass. The form tool may work on brass, but stainless steel would be rather more interesting.

Andrew

[James Green 2Participant @jamesgreen2]

Thank you everyone for your time and help with this. Your comments and advice are proving incredibly useful. My intention is to produce this part in stainless but even to prototype and test in brass at this stage would be perfectly reasonable. I'm going to revise my drawing following your feedback. None of the details are finalised and if small adjustments to thread sizes or ball diameter increased production ease then I would of course take this on board. Thanks again everyone. This is a wonderful platform for the exact help and support I was after!

[JasonBModerator @jasonb]

I don't think there is anything wrong with your choice of thread sizes, M1.6, M2 and M2.5 are both standard sizes, Don't let the comment by someone who can't have used metric put you off. What you also need to think about is the pitch of the threads as you may be better off with metric fine rather than the standard metric coarse threads, this will give you a few more turns of thread on the spigots.

The drawing should have M1.6 shown for the spigots and M2  the hole and the pitch. You could go the whole hog and add tolerances if needed.

Agree with Andrew the for tool won't be as easy on stainless but may work, if not could be done with a ball turner

Edited By JasonB on 11/10/2017 08:03:24

[JasonBModerator @jasonb]

As Wednesday is shed night and curiosity had got the better of me I thought I would see if the machining sequence I posted earlier would work, nothing too exact but enough to prove the method also as Andrew had got me thinking about how a form tool would work on stainless decided to use that rather than easy brass.

Took a 4mm Sq HSS tool blank and tickled the end with a Dremel chain saw grinding bit and offered up the shank of a 5mm drill to eyeball the profile, not top rake.

Put a bit of 5mm 303 stainless in the 3-jaw as that was on the lathe, turned the 1.6mm dia spigot and then went straight in with the form tool, dry, about 300rpm, mounted at a slight angle means no side clearance needed and the profile was a bit wonky anyway so best not mounted at right angles.

Threaded the end and then over to the mill to drill and tap M2, should have spent a bit more time centering up and spotted deeper as drill wandered a bit but it will do for this purpose.

back in the lathe and used a parting tool to form the other 1.6mm dia and then parted off, took a bit off the side of the ball but hay ho.

held in an ER block to thread the other side

Job done but I did resort to R/H threads both sides as I don't have a L/H M1.6 die. Easy to thread and tap, easy to form the ball. If it were a paying job a bit more time getting the form tool right, drilling centrally and using correct threads and they could be made quite easily.

J

[Howard LewisParticipant @howardlewis46836]

Well done Jason.

Anything below M3 is watchmaking for me, really prefer to use M5 and above, although above M10 the pitch gets a bit coarse, for anything needing fine adjustment. (In which case it is likely to be 1/2 UNF).

Hopefully, the Forum has provided, as usual, advice on sorting the problem!

Howard

[Author]

Posts