Coining/Die operation manufacture process advice...

[JohnFox]

Hi Guys,
I hope someone can help me with this query. I need to manufacture the attached part (material:2mm thick
316l stainless steel, tolerance +/- 0.2mm).

At the moment during the design and testing phase I laser cut the part and add the internal and
external edge radiuses with a profile tool on the milling machine. Those processes are not very cost effective
and take to long for production. Could I make this part via a combined stamping/coining operation?

This would be much more cost effective with the objective to add the required internal and external radius edges in the same hit if possible.
I have had no experience with metal forming processes so would be looking to sub this out.

Is this a reasonable approach to take in this instance or can anyone suggest something better?

many thanks,
JohnFox

 

[MikeHalloran]

As dimensioned, I don't see a way to make it as you describe.

... or at all. The slot location is not dimensioned.



Mike Halloran
Pembroke Pines, FL, USA

 

[JohnFox]

Hi Mike,
sorry I missed a dimension, the drawing was more to show what I was doing not specifically to send off for production. I don't think that will effect whether on not a 0.5mm radius can be produced via a coining/die operation inside the slot or whether the part can be made at all...

I hope that is ok.

many thanks,
JohnFox

 

[MikeHalloran]

Understood.
To answer your actual question, you could coin the edge down, but the material has to go somewhere. You can get a radius that's tangent to the faces, but the edges will be messy, with the former edge corner sort of extruded down over the edge proper. You will have a lot of trouble with slivers of material falling off and fouling the tool.

You can probably do the part with no or very little secondary processing as an investment casting.

Mike Halloran
Pembroke Pines, FL, USA

 

[JohnFox]

Hi Mike,
excellent, that is exactly what I needed to know. I understand. I will investigate making the part as an investment casting and see what the costs come back like.

Many thanks for your help and advice.

best regards,
JohnFox

 

[ajack1]

You could certainly coin the areas you are talking about with a press tool, however as Mike says you will get a small amount of excess material on the vertical faces however you will not get slivers or bits of material falling off if it is done properly.

Most of the “flashing” can be removed with vibratory finishing any good press shop will offer this service. Another option is to have a progression fine blank tool made, do a search for fine blanking; this however will not be a cheap option unless you have high volume requirements.

 

[ornerynorsk]

It may be more cost effective to have "slugs" turned and parted off from barstock. That would leave only the slot to machine, which could be done quite efficiently in a set of fixture jaws on the machining center. Investment casting should also get you within the .2mm tolerance, but your surface finish and some material props might be different between wrought stock and a casting. Could also look into MIM, if the volume warrants it.

 

[JohnFox]

Hi guys,
many thanks for all the helpful and useful advice. This has certainly got me thinking and reading about die/coining operations. I am starting to get the idea.

Today I investigated further making the part via more traditional methods as ornerynorsk has just suggested. I think I can indeed make the part economically from bar stock. I will let you know the outcome within the next couple of days or so. If the volume goes up I will look into MIM...

best regards,
JohnFox

 

[JohnFox]

Hi Guys,
upon further investigation I have decided to make this part via swiss style machining, it is just about cost effective. It takes around 3 minutes per piece off the bar stock and I use a radius tool for the internal edges. I intend to tumble the parts to put a small radius on the external edges.

many thanks,
JohnFox

 

[tripleZ]

JohnFox,

What is the flatness/parallelism requirement on the thickness? Next, what volume are we talking about? What are the corrosion requirements? And are you willing to budge at all on the radius corners? What about small chamfers with burr traps rather than full radii? I can mold most of that but would have to tumble deburr to round the outsides...I can't have much effect on the slot chamfers.

Conventional powdered metal pressing vs. MIM may work if we're talking EAU of 50,000 or more. It all depends on your strength & corrosion requirmements. That thickness & that diameter may be dicey w/ the c'sink...that may need secondary machining to avoid blowing up tooling. Low-temp sintered 316L shouldn't have problems with ±.2mm as long as you're willing to live with some chamfer modifications. High-temp sintered 316L will probably require some secondary grinding to flatten the part. We can sinter 316 to full density (called Ult-16 mat'l) but I'd probaby need to see double your stated tolerance on the slot as I'll see about 6% size change.

Check out

http://www.mpif.org

for a bit more info. They have links to some SS P/M houses on there as well if you want to pursue further.

 

[ornerynorsk]

You should be able to get the edge radii with either a form tool or interpolating before the slug is parted off. Tumble finishing should only be used for a final appearance or burnish to keep your cycle time down and to prevent surface mottling of your parts, unless that is desired. Good luck on the project.

 

[JohnFox]

Hi Guys,
thanks for the replies...

tripleZ: Parellism/flatness tolerances would not be tight. Volume would not be large, 1000 pieces per month. Non marine environment, general use. Edge radius and thickness flexible. Your reply is very interesting - many thanks. It gives me an insight and information for future jobs.

ornerynorsk: Yes, exactly, that is what I am doing, internal edge radii with a form tool and tumbling to finish the external edges and keep the cycle time down and hence cost. I increased the part thickness slightly and internal radius value to make things slightly more comfortable..

many thanks,
JohnFox

 

[williedawg]

Hi Guys,
upon further investigation I have decided to make this part via swiss style machining, it is just about cost effective. It takes around 3 minutes per piece off the bar stock and I use a radius tool for the internal edges. I intend to tumble the parts to put a small radius on the external edges.

many thanks,
JohnFox


Maybe I'm missing something....but where did you find bar stock with this outside contour ?