Mass Production

This topic has 20 replies, 13 voices, and was last updated 5 September 2018 at 08:53 by Bob Rodgerson.

Viewing 21 posts - 1 through 21 (of 21 total)

Author

Posts
3 September 2018 at 08:41 #370149
Bob Rodgerson
Participant
@bobrodgerson97362
I am trying to find out what type of machine would be used to manufacture several thousand simple components from round bar of say 18mm dia with a 15mm Dia X 17mm deep blind bore in one end and an M6 internal blind thread *.5mm deep on the other end, the whole job being no more than 26mm long.

Pre-CNC days, how would this have been done? What modern CNC type machine would be used today?

Obviously the job could be done by programming a simple single spindle CNC machine to carry out the operations on one end of the bar then part off but the components would have to be re-loaded the right way round to carry out the operation of drilling and tapping the hole in the other end. This would be extremely time consuming and would probably take longer than the drilling and tapping operation itself.
Advert

3 September 2018 at 08:41 #26169
Bob Rodgerson
Participant
@bobrodgerson97362
Manufacture of multiple thousand components
3 September 2018 at 08:48 #370150
roy entwistle
Participant
@royentwistle24699
An M6 internal blind thread .5mm deep ?

Roy
3 September 2018 at 08:57 #370153
Phil P
Participant
@philp
Probably 8.5 deep if you look at your keyboard.

Phil
3 September 2018 at 08:58 #370154
Nick Taylor 2
Participant
@nicktaylor2
I'm sure he means 8.5mm deep.

To answer your question;
3 September 2018 at 09:09 #370156
Anonymous
Bob: Not enough information! What material? What tolerances are needed? If the component is 26mm long with a 17mm recess one end that only leaves 9mm for the M6 thread. If you really want 8.5mm of thread that only leaves a 0.5mm wall thickness. no tap is going to do that. You'll either need to screwcut or thread mill.

In theory any capstan or repetition lathe could do the job, athough the M6 thread is tricky. But I think all would need a second op. And I'm not offering to make them!

Personally I'd change the design to make it easier to manufacture.

Andrew
3 September 2018 at 09:18 #370160
Alan Waddington 2
Participant
@alanwaddington2
**LINK**
3 September 2018 at 09:38 #370165
Mick B1
Participant
@mickb1
My experience in this sort of production stems from mechanical controls in the late '70s. They were mostly cable controls for boat steering and engine systems, and remote valve controls for mechanical diggers. There were lots of mass-produced cable-end components of various shapes along with 'hubs', which were specially-shaped tubular and often screw-adjustable outer sleeve ends. There were thousands of varieties.

We used mostly cam autos for the big batches – they tended to be profitable for annual quantities of more than 20,000. They were essentially small capstans with a slow-running circular cam driving the slides. To buy a set of cams – often with circular form tools for component shaping – was quite expensive, and setup was lengthy, but they'd kick out several parts per minute.

There's a video here:-

https://www.youtube.com/watch?v=Ec8zKfZ7M7M

…showing one running. You can see the cam controller circulating about 14 seconds in.

Smaller batches might use modified standard capstans with plugboard automation, and larger batches still would go onto multispindle autos like the Wickman, which had six revolving spindles like a Gatling gun, each doing a separate movement of the operation.

In the dial gauge industry where I was working in the late '80s, Swiss autos originally designed for the mechanical watch industry made many of the small turned piece parts.

Tooling up and setting both these and the cam autos was very much a specialist skilled job with corresponding pay rates.

Edited By Mick B1 on 03/09/2018 09:52:51
3 September 2018 at 10:27 #370175
Neil Wyatt
Moderator
@neilwyatt
If the M6 hole can be made right through so all the machining is done from one end, it would be a one-setting job.
3 September 2018 at 11:11 #370185
Hopper
Participant
@hopper
Posted by Bob Rodgerson on 03/09/2018 08:41:54:

Pre-CNC days, how would this have been done?

Capstan lathe. Or any common lathe, manned by an apprentice.
3 September 2018 at 12:20 #370194
Neil Lickfold
Participant
@neillickfold44316
I once saw an old WW2 American cam auto machine that was making the 1st part of a .303 shell casing. It was just as it was last used in 1945 when production stopped. It was the last one, that the owners Grand father did not sell off or scrap or break down the set up of. It was as I was told, his personal piece of history. It had carbide tooling that was top secret in those days. Anyway, it drilled, did the hole for the primer, turned the out side, did the inside , the ring groove and parted off, all in 6 seconds. Makes on heck of a lot of noise and fluid and stuff goes ever where. It ran cutting oil, and they had what looked like an old washing machine, that spun the chips to reclaim the oil from the swarf. I was really impressed and they ran it that day for us to see. This was back in 07. Similar to the video, had a super rapid turret indexing, on the inline turret, and the back turret. It had a similar vertical part off , and a front tool that did not index, but profiled. This did the retaining grove.

The shells were not necked at this stage, that was done latter, along with the former for the primer hole final sizing.
3 September 2018 at 12:36 #370198
Neil Lickfold
Participant
@neillickfold44316
Back to the OP, quite a lot of high volume work was done on multi spindle lathes, with 6 to 7 stations. Each station did a particular operation, often with form tools , or gang tools or other tooling that was made specifically for that part being produced. These were either capable of hand loaded and unloaded parts, or bar feed with parts coming off.

Then the other end detail would be done as a second operation, hand loaded into a basic 2nd op machine, or into a 2nd op semi auto machine. The 2nd op machines, don't have the bar feeders on them, and require the operator to activate the start sequence. Most of the USA machines, needed 2 hand to simultaneously button start.

So in your example, without seeing it, the threaded end would be done 1st, then the end with the hole would be done in a dead length stop collet, for the hole and other detail and the final length as well.

Neil
3 September 2018 at 13:57 #370214
Jeff Dayman
Participant
@jeffdayman43397
Back what seems many years ago in the early 1980's when I was just starting in industry I worked for a large US based controls firm. They had a room full of Brown and Sharpe screw machines and multi slide capstan machines by various makers including K&T and Giddings and Lewis. One of my tasks was to design, coordinate manufacture of, and qualify custom cams and capstan tools for machines like the one in Mick's video. These machines were very versatile, some had been in continuous use since the 1930's. I think the parts described by the OP could be easily made on such a machine in two steps, and would have been, possibly from 1920's to 1980's, if qty were high enough. First step would be the threaded end, then part would be manually loaded to a second machine to do the blind hole 15 dia x 17. This approach assumes the OD remains largely cylindrical to allow normal material tube type feed and grip. Shallow blind threads were done both by multiple short modified taps and by screw cutting with a threader attachment on one of the capstan stations at the firm I worked for. I was told this threader station design was pioneered by a tool designer at the firm during ww2 to increase capability to make huge qty's of fuse parts and aircraft instrumentation parts. A thru- thread would of course be faster and easier to make in one step, but short blind threads are not a big deal on these machines.
3 September 2018 at 21:52 #370295
Bob Rodgerson
Participant
@bobrodgerson97362
Posted by Andrew Johnston on 03/09/2018 09:09:07:

Bob: Not enough information! What material? What tolerances are needed? If the component is 26mm long with a 17mm recess one end that only leaves 9mm for the M6 thread. If you really want 8.5mm of thread that only leaves a 0.5mm wall thickness. no tap is going to do that. You'll either need to screwcut or thread mill.

In theory any capstan or repetition lathe could do the job, athough the M6 thread is tricky. But I think all would need a second op. And I'm not offering to make them!

Personally I'd change the design to make it easier to manufacture.

Andrew

Hi Andrew, Material is 316 Stainless, tapped hole is tapping drilled 9.5mm deep and tapped as deep as possible, not sure what you mean by 1mm wall thickness because at this end of the work piece it is 18mm dia. The other end is 18mm O.D X 15mm bore X 16mm or so deep.

I have made the prototype on my manual later and am sure I could do it on my Tormach with the Rapid Turn set up using gang tooling and the lever operated chuck, however I have no desire to stand at the machine manually loading it and then turning the part around to carry out the work on the opposite end.
3 September 2018 at 21:53 #370296
Bob Rodgerson
Participant
@bobrodgerson97362
Posted by Neil Wyatt on 03/09/2018 10:27:02:

If the M6 hole can be made right through so all the machining is done from one end, it would be a one-setting job.

Neil,

M^ hole must be blind so no easy fix.
3 September 2018 at 22:06 #370297
Bob Rodgerson
Participant
@bobrodgerson97362
Thanks for all the replies, it looks like a repetition lathe or Cam auto could be the way to go.
3 September 2018 at 22:15 #370300
Neil Wyatt
Moderator
@neilwyatt
Posted by Bob Rodgerson on 03/09/2018 21:52:57:

Hi Andrew, Material is 316 Stainless, tapped hole is tapping drilled 9.5mm deep and tapped as deep as possible, not sure what you mean by 1mm wall thickness because at this end of the work piece it is 18mm dia. The other end is 18mm O.D X 15mm bore X 16mm or so deep.

9.5mm deep + 16mm is 25.5mm.

In a 'no more than 26mm 'long part, that only leaves 0.5mm wall between both holes. Assuming the M6 hole is drilled, care will be needed so the tip of the drill doesn't break through.

Seems a bit tight for a mass produced part to me.

Neil
3 September 2018 at 23:00 #370310
Martin Connelly
Participant
@martinconnelly55370
Plunge milling cutter will give flat bottom holes. Thread milling will thread to the bottom of the hole.

Martin C
3 September 2018 at 23:17 #370312
Anonymous
Hmmmm, we seem to have a fluid specification. Not so good for a production part.

In the OP it states the overall length is no more than 26mm long with a 17mm deep blind hole in one end and an 8.5mm deep thread in the other end. In my mathematical world the following is true:

26-17-8.5=0.5

If that's not the case it would appear that Godel has been at work.

As an aside plunge milling will not result in a flat bottom hole, as endmills and slotdrills are slightly hollow ground.

Andrew
4 September 2018 at 22:37 #370497
Jon
Participant
@jon
How did you get on tapping Grade 316 Bob.
5 September 2018 at 08:53 #370516
Bob Rodgerson
Participant
@bobrodgerson97362
BobHi Jon,

no problem tapping but I've only done one prototype. I have a batch of 70 or so to make which I will do on the Tormach with the Rapid Turn set up and this will be a test to see how well it goes. I think, because the holes are shallow it makes it easier. The bore size of the other end is not critical so I will drill this with a flat nosed carbide drill.

Beyond the first batch I think that thousands of these things will be required, hence the questions about which is the best way to mass produce them.
Author

Posts