Reply with QuoteLaser or waterjet cut I would think is the way to go.
Konrad
Shim Stock Machining/Forming Options
I'm looking for suggestions on how to form or machine shim stock for very small parts such as the click spring (dark blue part) shown in the attached jpg on a hobbyist budget. The thickness of the spring will be approximately 0.032" with the complex form shown. The tip will be bent 90 degrees where it contacts the click (shown in gray). The picture doesn't properly represent the end of the click and the 90 degree bend. The sizes are all to scale with the largest gear being 3.1" to give an idea of the spring size.
Is it possible to mill such material with solid carbide end mills that are coated in TiAIN and how would you hold the part while machining?
Or is it possible to cut this material such as with tin snips to get the rough shape and then file?
Also, when bending the tip 90 degrees would I need to heat it up red hot before bending to keep it from breaking?
Any feedback would be greatly appreciated.
Best Regards.
Carl
Similar Threads:
Laser or waterjet cut I would think is the way to go.
Konrad
How many do you have to make? I think that changes the plan depending. Are you sure shim stock is what you want? Not sure of the "springiness" there.
For a one off, lots of possibilities enter the mind. Take some hardened stock and grind to shape, possibly under CNC control. It's a pretty small part so you can protect your machine if CNC'ing.
Or, take the annealed (soft) stock and try machining. Use some really small cutters and take light cuts.
You could also try to punch the annealed stock to shape.
I would consider whether there are changes in the shape of the spring that will facilitate easier manufacture as well. For example, the bottom part need not flare out for the mounting screw, it could be simplified so it is the same width and eliminate a little bit of work there.
You can machine a piece much thicker and surface grind it down on a magnetic chuck if that helps too.
Cheers,
BW
Laser and/or waterjet sure would be a nice setup but I just got finished converting my mill to CNC and hope to get a little use out of it before looking into better techologies like these. Although I doubt that I could affort one that cuts metal.
For now I'm just looking for alternatives to making these parts using more traditional machining techniques even if it ultimately means I have to do it entirely by hand. The springs are used in 8 day long case clocks (grandfather clocks) and I would be making two of these springs per clock. So it's not likely that I would make more than a couple of hundred over the duration of this project. I would only make 2 to 4 at a time depending on how they are made.
I agree that the shape could be modified considerably to simplify machining but I would still be hand dress them, if you will, to get the final shape. While it is not functional it is a traditional looking design.
It was my understanding that shim stock is also referrred to as blue tempered spring steel which is really what I would be using.
My take away so far is that shim stock can not be machine with an end mill in it's hard state even with TiAIN coated carbide. But it can be ground. Since I don't have any way to grind, I will need to explore annealing the shim stock.
I did not realize that shim stock came in an annealed state. I suspect this is a 1095 alloy. So I guess I would need to buy the tempered version and anneal it myself before machining and then re-temper it after machining/forming process?
Best Regards.
Carl
For such a thin cross section part and its function as a spring, heat cutting would certainly be out. Waterjet has some issues with leaving fissures that lead to cracking on thinner brittle materials intended for stress strain cycles. Secondary metal finishing would be needed to remove the outer profiles sand blast surface finish.
Punching would be the most efficient and repeatable if you had the quantity to cover the tooling cost.
Left with machining them, I would approach it in a 2 setup fixture cutting 4-6 in a stack with heavier top cap hold down clamping. The fixture would have 2 stations. One for comleting the holes (and indexing pin holes for subsequent operation) and OD arc. The second would also have a heavy cap clamp and have indexing pins, Along with an OD arc nest to support the OD while cutting the ID profile. I would also simplify the inside profile around that larger hole if it is just cosmetic it will require a smaller cutter. Modified to basic angles could opt for a larger cutter that will last longer at a lower RPM for the material being cut.
At that point, you can decide if you can machine off the indexing pin tabs at each end of the spring or remove by hand later.
If you use spring steel or blue tempered shim stock. It only needs to be anealed in the bend area on sharp bends. Practice with a radius or local annealing for the best results. Not red hot.
DC
DC,
That's more doable with my current situation. I like the two step approach and will work on a jig to get this tested with my equipment.
Thanks for the feedback.
Best Regards.
Carl
Still,..laser cut is cheap and I don't think heat would be a issue in thin parts. It takes a few seconds to cut things like this.
At least, go to your local laser shop and see what they say.
Also waterjet, a stack of at least 10 or so would be easy enough.
Cutting it out conventionally can be done but putting the small holes in? what sizes are they? tolerance?
You have to be pretty skilled to drill them. Accurate holes, I sometimes have them water cut under size and ream after.
Konrad
Konrad,
I appreciate the recommendations as it may utlimately be where I end up with this. For now, I'm more interested in learning/seeing how harder materials like shim stock and gauge stock can be machined. I realize that this puts more stress on the mill and even the tooling and I will most likely see more tool breakage and failure but it's more a learning experience. While I would like to do this in-house, it may not be practical after this exercise.
The click spring has a mounting hole that is 0.089" for a screw and another hole which is 0.040" for a tapper pin. I was planning on using a hold down plate while drilling the two holes (through the plate too) with a carbide drill of the respective sizes. Here again I've never tried this but it appears that the solide carbide straight flute 140 degree drills are designed for hardened materials.
With any luck, I'll post the results and some pictures.
Best Regards.
Carl
In my experience as an OEM Field Service Tech, the laser cut edge heat effected zone was at about one material thickness. As a guestimate scale at the narrowest section, on an 1/8" wide piece at .03 thick, .03 around the periphery would be compromised.
Most of the spring steel I had seen laser cut were formed and post heat treated to restore the temper condition on parts where it mattered. Until it could be proven out, I'd think it unwise.
My experience with a water jet and stacking part was a real failure. The sheets would balloon with pressure on pierce and periodically at corners. Once it has garnet in between the layers, I think all bets are off. I've heard it is possible, but it may be for PSI in excess of 40K. Either that or avoid piercing and always enter from the side. I don't get that much time to play. I use ours when I just need R&D parts for design work, not production.
I have designed and CNC cut custom springs for my automation projects out of .06-08 blue tempered spring steel. Cutting 4 in a stack with a 1/2" 4 flute carbide endmill. I can get a couple dozen with the same cutter. My suggestions were what I know will work and where my experimentations didn't pay off and showing where a particular process has known negative impact for the application.
I have found quicker isn't always better if all it does is waste time finding out what doesn't work. Konrad is right though. A quote from those in the know won't hurt. Just be aware they will take the work in, but rarely guarantee the results will work. They just cut it, not many provide engineering guidance they cannot back up.
DC
Sure, it will be a good learning experience.
I'm thinking of another way without fancy fixtures,.. cut rectangles pieces to size, drill holes in vice, use screw, [ for .089" hole] and clamp about 10 or 20 pieces together, use pin for .040 hole, can use drill bit shank of a number drill for lining up other side, make pattern, [cad drawing] and glue on both sides, use your bench, hand or surface grinder to grind to pattern [keep cool]. Sometimes on heavy tool steel material, like 3" and up I scribe the outside contour with my home made spring loaded carbide scribe in the CNC, then I cut on vertical band saw within 1/16 or 1/8, then finish contour mill. This saves allot of time and cutter!
Konrad
If you are going to go through all that hand work, one might as well have them laser cut over size and mill the heat effected edge off. That would certainly be a good idea to save some time and cutter life, if lasering to net didn't work as planned. I'd think secondary milling would still require tabbed index pins and a fancy fixure to support it under the cutting pressures it may see. For what the spring is to be used for, consistancy in the finished spring attributes would seem a high priority?
I keep wanting to build one of them skeleton clocks. They sure are a marvel to look at, but I don't know how accurate they are or how much fussing they take to keep running. Changing a couple batteries once a year is tough enough for me to keep up with!
DC
There are many way's to skin a chicken!
I'm trying to find a way for Carl to do this in house as he doesn't consider any outsourcing.
Do you have a surface grinder, Carl?
A surface grinder can cut very cool with coolant creepfeeding down, stack of 20 or so.
I could dress the shape on wheel and grind down unattended, concave, convex. Two wheel would be required and minimal
clean up by hand.
OK...back to CNC. I have done thin sheets, [tool steel] glued down on mild ground steel plate and it worked great.
Perhaps your spring steel is large enough to make 50 or 100 pieces. Drill all holes firsrt, not sure what cutter would work better?
I would go as small as possible for minimal cutter pressure, but then not too small, otherwise you have flex.
Lets say about 1/8", then try go around the contour .010 deep with allot of coolant. Try full depth and see. You can also try a 1/8 ball nose or 1/8 ball burr cutter, when done, these will need a bit more hand clean up. Better yet, drill with carbide bit on contour line
so you have only about .020" meat between the holes, then come in with endmill and go around one cut.
Konrad
Unfortunately I do not have a surface grinder. Making the jigs and fixtures is part of my training/learning so that's a good thing for me. I like the idea of glueing the parts before clamping.
I've got most of the g-code done for a 3 part operation but will need to order some supplies in the next week or two. I think the 1/8" carbide end-mill TiAIN coated will be the best. I only have a small mist coolant setup but will try that. My first test will only cut 1 for obvious reasons. If it looks like it will work, I'll try stacking.
Thanks again for the replies gentlemen. This is a great forum.
Best Regards.
Carl
I don't think I have explained it well, this is what I would do....Originally Posted by cmnewcomer
Take one large sheet of spring steel to make 50 or 100 pieces.
This sheet glued with loctite to a flat, ground steel plate, [or cold rolled plate?]
In cheap cad cam [bobcad], draw one piece with tool path holes etc, then spread, pasted it all over the sheet, then machine.
Konrad
OK, now I see where you were going with that Konrad. That would be after I've confirmed all parts are properly sized, tested, etc.
For now, I will only make a few at a time and make small adjustments possibly to the dimensions of the click. Once I've got things where I want them I may consider making multiple pieces in one setup but even then it may be overkill for my requirements.
The jig I've made will be used to machine in two steps. I have a setup hole in the lower left of the aluminum block for getting the tool centered. The larger hold down plate at the top will be removed for the 1st operation and the spring steel will only be clamped by the lower hold down plate. I'll mill the outside profile of the click 1st in one pass. Then I'll install the larger hold down plate for the 2nd operation and mill the inside profile. The click spring will be entirely under the larger hold down plate so I believe it will be secure. I'll then perform the drilling operations and the hold down plate will prevent the drill from wandering.
Thanks again for the feedback everyone.
Best Regards.
Carl
Annealed Blued Spring Steel
Ok, I'm an idiot. I just found out that the C1095 blued spring steel can be purchased in the annealed state. However, all of the online places I can find are the big boys who don't sell to hobbyists. I'v looked into Admiral, Onlinemetals, and others but no luck.
Does anyone know an online supplier of annealed blued spring steel?
Best Regards.
Carl
This forum is great. Thanks DC!
There is a million ways to do it.
You can use the .089 hole to put in one screw and design in some tabs on the permitter to add more screws for hold down into a custom fixture block. Cut around the part and the tabs. Remove and cut the tabs off by hand and then blend in the rough spot. Kind of a pain but it works.
You could do the same sort of thing and build some moveable clamps into the fixture. Remove and replace the clamps as the cutter goes around. Kind of a pain in the arse.
If I only had to make a few I'd probably do them on double stick tape. Sounds crazy but it works. Run around with a 1/32 end mill at say, .010 depth of cut.
If you're in charge, redesign the part and add more screw holes. Drill or mill the holes in the shim stock and then screw it down to a custom fixture block, 10, 20, 100 parts at a time. Blast around with an end mill, remove the screws and there are your parts. That is production machining 101. Everything stays nice and flat, the part is held down well and you can cut as fast as possible. Flood coolant all the way.
Most of the shim stock I cut at work is 304 stainless. It's decently springy. Mcmaster has it. It's a pain to work with.
Re: Shim Stock Machining/Forming Options
I know this is a very old thread, but I was looking for a way to cut and bend .010" HARDENED shim stock to make spring clips. I can't locate the material in the unhardened state. I don't have access to a laser or waterjet, and also don't have a surface grinder. I do not have a heat treating oven, or access to one. I know from past experience, that it is very difficult to anneal thin metal like this with a propane torch. As soon as you withdraw the torch, it "quenches". I found that placing the part in sand, heating it to annealing temperature, and immediately dropping more warm sand on it, will sometimes stop the quench. The sand acts as an insulator to keep the steel from cooling off rapidly. I suppose if the part is flat enough, and I had a very powerful torch, I could stack it on a thicker piece of metal, and heat both at the same time. The thicker metal should keep the thinner piece from cooling too rapidly.
