PDA

View Full Version : Best method to produce this little widget



rooze
15th Apr 2021, 12:47 AM
Hello Y'all

Can anyone advise me on the best way to have these aluminum discs made, please -

391556

The diameter will be 2.25 inches and the height 0.75" The holes need to be bored to a depth of 0.5"
The bores need to be drilled to a tight tolerance as the springs you see inserted are a push-fit.

I'd be starting out with having some prototypes made, probably a dozen then larger production later once any kinks are ironed out. A low grade/ low cost alloy material is fine, there's nothing fancy about what these are doing, though they do need a fairly polished finish that's non-corrosive.

I think ideally I'd like to make these myself initially. And I'd be OK investing in some type of desktop CNC machine if I knew what to look for and could find something under $1000

But where would I source the aluminium/aluminum/alloy blanks cheaply enough?

What type of machine (specifically, please) would I need to buy to do the holes? On the sample I have, the hole bottoms are flush/flat and are not tapered as they might be if drilled using a conventional drill bit, though this isn't an essential part of the spec if it inflates the cost.

Can anyone help or even do this project?

I'd also like to interchange the materials at some point and use either wood or acrylic blanks, so the machine purchased needs to be able to handle various materials.

I've looked around for aluminum blanks but all I could find in this size were some super-fine tolerance discs that were fifty bucks a piece! I need to get these made for a couple bucks each.
Thoughts, please!
Cheers

BaronJ
15th Apr 2021, 02:05 AM
Hi Rooze,

Welcome to the forum.

Do you have the machines that could make these parts ? If so then whilst CNC could do them it would probably be easier and cheaper to make them yourself, particularly if you want to use different materials at some point.

This is how I would make them. Using a lathe part slices of material off to width from round alloy bar. Make a simple jig that can hold your round and be rotated and indexed to provide positioning for the holes. The centre hole can be done on the lathe before parting off. If there is only the spring in the hole, do you really need a flat bottom in it.

Hope this helps:

BobL
15th Apr 2021, 08:54 AM
To start with I doubt this is a task for a small desktop CNC.

2.25" is a stock size for Al bar so you just need something to cut it to length.
You would need a very large (ie 10's of thousands of $$) to hold longer lengths of this bar in a lathe
OR
You could use a small lathe and a small bandsaw to cut down short lengths of bar to hold it in the lathe chuck.

The cheapest and quickest way to cut this material would be using a table saw with a negative raked blade. The stock has to be held firmly or it will spin as well as producing a poor finish.
You could get away with a bench top saw to do this. The finish may not be to your satisfaction and then may need to be faced off using a lathe.
The same table saw and blade combo will also easily cut acrylic and wood (albeit slowly)

How many do you need to make, if its only a few the $50 a piece for the blanks is cheap especially if you have to buy machinery and get up to speed with use of machinery.

You don't mention the diameter of the holes but a quick way to get a flat bottomed hole in Al is using a Forstner bit. However they only come in fixed sizes so the closet size might be too tight or too big. While Forstner bits can be used in a hand held portable drill, drilling large holes in Al is problematic as the pressure neede is very high so you will need a drill press

old1955
15th Apr 2021, 01:11 PM
Welcome to the forum.

caskwarrior
15th Apr 2021, 01:16 PM
There is definitely no $1000 machine manual or cnc that is going to do this job for you really. Unless you get very lucky. Manual mill with a divider and a good horizontal bandsaw that cuts straight is probably your cheapest option.

Anything CNC even an old fadal or hass you may as well just light 10k on fire now.

Id say produce them manually for now or outsource them.

Sent from my SM-G973F using Tapatalk

Jekyll and Hyde
15th Apr 2021, 05:59 PM
There is definitely no $1000 machine manual or cnc that is going to do this job for you really. Unless you get very lucky. Manual mill with a divider and a good horizontal bandsaw that cuts straight is probably your cheapest option.


Might be. Poster is in the US, as you know it's a whole different world of machine tool availability over there depending on where exactly they are.

But producing them in aluminium for a 'couple of bucks each'? That might be a tall ask even in USD, without outsourcing to China, unless you get a massive run done by a CNC company. Looks like online (probably close to off the street price) for 2.25" 6061 bar is about $35USD per foot, which works out to about $2 USD per 3/4" before you even start machining. 2000 series aluminium might be cheaper, but looks like it also might be a less common stock item from the brief look I had.

For prototyping in aluminium, pick one of the many hobby machinist boards with a far higher US population than here (Probably 95% of active members on here are in Australia, not much good to you), and ask for someone to do it there. Someone with a lathe and a mill can knock them out FAIRLY quickly, but it's still going to cost you. I figure an absolute bare minimum of 15mins each for me to make them here once in the rhythm, that's bandsawing solid stock to rough length, face both sides on the lathe and centre drill, then punch the hole pattern out on the rotary table on the mill using a centre cutting endmill to give the flat bottomed hole. Add a bit of time if the outside diameter needs to be cleaned up too, and add more time for every tight tolerance. And given things often take longer than I think they're going to anyway....

If I had a big enough spindle bore to pass it, could skip the bandsaw step and turning the OD would add a lot less time - if you're lucky enough, someone local to you will have a big old Monarch or Pacemaker (or one of the various other big old American iron) with a big enough spindle bore to pass it through. Although, thinking about it, the Graziano has a 2" spindle bore with some form of taper in it, could probably jam about 12" of 2.25 stock through the chuck before the taper got too small, and with a 2.25 OD could probably get away with at least another 6"-8" hanging out the front, so might be able to bypass most of the bandsawing for the dozen desired with a 2" spindle bore, which is going to be a LITTLE easier to find.

Of course, given you mention you want to make them in wood or acrylic later anyway, 3d printing in plastic would probably be the far cheaper way of prototyping them, even if you buy yourself a 3d printer to do it...

rooze
16th Apr 2021, 03:51 PM
Hey, thanks y’all for some great feedback. I wonder if there’s some way to cast these as a cheaper option.
I’ll check that out next

Cheers

BaronJ
16th Apr 2021, 05:56 PM
Hi Rooze, Guys,

I rather suspect that casting would be a more expensive and time consuming method of production ! That is unless you are going to go for Die casting, producing millions, in which case Mazac would be the material of choice.

Some years ago I went through a not dissimilar process. I had to produce several thousand aluminium discs, 100 mm in diameter 12 mm thick. I found that the most cost effective way to produce them was to trepan them from squares of plate cut to just over 100 mm, actually 110 mm if I remember correctly. Trepaning was far faster than using a hole saw.

The following process saw 16 drilled and threaded holes around the edge of the disc. The was a countersunk hole in the centre of the disc as well.

Each disc took about three minutes to produce ! I wouldn't be surprised if producing your widget took about the same time.

Production is all about cost ! Time is money and labour isn't cheap !

grunto
18th Apr 2021, 08:40 AM
Try one of the online services - just upload a file and you will get back some indicative pricing straight away.

https://www.xometry.com/

elanjacobs
18th Apr 2021, 10:59 AM
Don't wanna be to be 'that guy', but it's time for a reality check. This is going to be blunt, sorry.


Starting from the end of your question.

I need to get these made for a couple bucks each.
Not gonna happen. End of story. The rough material cost ALONE is gonna be at least double that before you even think about machining it :no:


The bores need to be drilled to a tight tolerance as the springs you see inserted are a push-fit
You'd want to be holding a half thou tolerance on that, drill and ream would be the DIY method to get that.


And I'd be OK investing in some type of desktop CNC machine if I knew what to look for and could find something under $1000
Again, not gonna happen. Accuracy is expensive. Plus, you'll need to machine the blanks out of bandsawn bar stock first, so you'll need a lathe as well.


But where would I source the aluminium/aluminum/alloy blanks cheaply enough?
You can't.


I've looked around for aluminum blanks but all I could find in this size were some super-fine tolerance discs that were fifty bucks a piece!
Ya. Material + programming time + setup time + machining time + tooling + overheads + hourly rate of the guy running it = hand over the credit card.

nigelpearson
18th Apr 2021, 03:32 PM
Howdy Rooze.

Someone in China could churn them out for a couple of bucks a piece, but I suspect best USA prices would be $8 to $10 each?

Also,

A) Non-corrosive is a challenge. Is it used in something caustic? (which might require Anodising)
Or are you talking about the springs not rusting into place?

You could use really cheap Aluminum (e.g. commercial quality Aluminum stock), but it will look blotchy when anodised.


B) How well does the disc have to grab the spring? If it is a very close fit, assembly will be a challenge. A drop of Loctite in the pocket might be easier




Anyway, If the spring diameter is close to a standard size, I would try prototyping on a lathe (CNC or otherwise), with live tooling. 14 steps;

1) Face the bar.

2) Lock spindle. Load drill, or centre-cutting end mill, in live tooling. Turn on coolant.

3) Wind cross slide to back pocket radius. Plunge back spring pocket.

4) Wind cross slide to middle of bar. Plunge middle spring pocket.

5) Wind cross slide to front pocket radius. Plunge front spring pocket.

6) Unlock spindle. Rotate 60° and lock again.

7) Plunge spring pocket.

8) Unlock spindle. Rotate 60° and lock again.

9) Plunge spring pocket.

10) Unlock spindle. Rotate 120° and lock again.

11) Plunge spring pocket.

12) Unlock spindle. Rotate 60° and lock again.

13) Plunge spring pocket.

14) Load parting tool. Use it to skim outside of bar, and then part disk off at 0.75"

(and if you are using a CNC lathe, either trigger bar feeder to push through more stock, or trickily use the parting tool in two steps, and use a brass sheet in the slot to slide stock along before parting off)



I'm sure a better machinist could improve my steps, but I hope that will give you an idea?

BaronJ
18th Apr 2021, 05:26 PM
Hi Nigel, Guys,

I've done that with pocketed springs, the tolerance can be quite loose ! Twisting the spring like a screw as its placed in the pocket causes it to grip the wall in the pocket.

Actually similar devices are commonly found in clutch mechanisms !