The Complete Guide to Sheet Metal Design
What is sheet metal?
Sheet metal is metal, in sheets. It’s thinner than plate metal (.25 in and thicker) but thicker than foil (.006 in and thinner). It’s most commonly available in steel and aluminum, in various gauges (thicknesses). It’s available with various coatings for corrosion resistance or surface finish. Sheet metal is made by taking a large cast ingot and rolling it into a long ribbon of the desired thickness. This long, flat piece of metal is then rolled into a coil and sent directly or cut into sheets before being sent to a machine shop.
What is it good for?
Sheet metal is great for large, durable parts with relatively few features. They make good RF shields and ground planes, and thicker gauge parts are great for adding strength and weight to things.
What is it not good for?
Sheet metal isn’t so good for very small parts, complex or very precise geometry, highly cosmetic parts, or lightweight parts.
How is it made?
For lower volumes (1 part – 10,000 parts), your parts will be made using a blanking and forming process. A blank (the flat version of your part) will be cut from a sheet using a punching or laser cutting process, and then bent to the final shape using a brake press.
At a very high level, sheet metal punching is similar to using a hole punch on a piece of paper. A top tool traps the material against an appropriately-shaped bottom tool and pushes through, creating a hole (or other feature). In the case of sheet metal, though, your material is up to a quarter inch of steel, and your hole punch is a multimillion dollar, many ton, high precision piece of machinery. Modern industrial sheet metal punches are CNC operated, accurate to .005” or better,and are capable of hundreds or thousands of punches per minute. They can often hold hundreds of tools and auto-feed sheets of material.
Punching requires a different tool set (top and bottom die) for each unique feature – each diameter of hole, square or rectangular cutout, or special feature needs its own tool (or tools). The good news is that tools are relatively cheap ($100-$1000 for most tools), and most suppliers will have a tool library with a wide variety of standard holes and features to get you started. If you are working closely with a supplier, ask them for their punch list, and design your parts to use punches that they have in stock. It will save you a bunch of money, and it will save them the hassle (and lead time) of ordering new tools.
Punched parts are priced by the operation. Each operation is cheap – fractions of a penny per hit, but a large part can easily require hundreds of hits, and they add up. You also need to pay for any custom tools you need, and at several hundred dollars apiece, tooling cost can easily outstrip your part cost if you’re not careful.
Industrial laser cutters are the bigger, much more powerful (and expensive) cousins of our own Mindtribe Boss laser. Instead of a shop-friendly size and power, production lasers are multi-thousand watt behemoths capable of vaporizing half-inch steel plate with .005” precision. It’s awe-inspiring and frankly a bit terrifying. These machines also often sport auto-load capabilities and blazing fast cutting speeds.
Because of the nature of laser cutting, you can only cut straight-sided holes into parts. That means a lot of the cool 3D features available on punched parts (extruded holes, louvers, jog bends, bumps, etc) can’t be achieved on a laser. On the plus side, lasers require no tooling. Because there is no tooling to break, the minimum hole size is limited only by the size of your laser beam, not the thickness of your material. It should be noted that there are a variety of materials that are hazardous to cut on a laser – painted and galvanzied metals can produce gaseous cyanide or chlorine, which needs to be properly treated and vented. Lasering is also usually more expensive than punching, which makes it a good method for low-volume, highly detailed parts, but less good for higher volumes.
Lasered parts are priced by machine time – the more features you have and the thicker your material, the more expensive your part will be.
At low volumes, flat blanks from a punch or laser are bent using a press brake – a hydraulic press that squeezes two jaws together with dozens of tons of pressure. They can be fitted with a wide variety of tooling to produce different bends. For low volumes, several alignment fixtures will be set up along the length of a press, and an operator will manually align and form each bend in your part.
Because of the human attention needed, bends are by far the most expensive features to add to your part. For this method, each bend can cost $0.50-$1.00.
For higher volumes (10,000 parts and more), you start moving towards sheet metal stamping. While punching uses small tools to punch out one feature at a time, stamping uses a single, large tool to stamp out the whole part at once. Stamping tools are similar to injection molds, in that they’re expensive to produce and basically single-purpose. That being said, stamping tools can produce an entire part in one (or a few) hits, which drastically reduces time and cost to produce. Also, because they’re custom-made and run on higher-tonnage machines, stamping tools can produce a lot of features that aren’t possible with punch tools, like complex surfaces, punches on both sides of the material, and bends.
Progressive Die Stamping
Simple parts can be stamped in a single operation, but more complex parts require what’s known as progressive die tooling. A progressive tool is two large pieces of metal – a top half and a bottom half. Each half contains many punch tools, along with bending, shearing, and forming operations. These operations are organized into several stations that the part passes through before emerging fully-formed from the opposite side of the tool.
Large stamping and progressive die tools are operated by punch presses, which are multi-story tall machines capable of exerting hundreds of tons of pressure. They’re often fed directly from a coil, and produce thousands of parts per hour.
Stamped parts are costed by machine time and setup, and are 70%-90% cheaper than lower-volume parts. Part of this is the speed at which parts can be produced, and part of it is that stamping tools can produce bends, as well as punches. However, stamping tools are expensive. They’re priced by size, number of punches, complexity, and tonnage. Simple blanking-only tools start at several thousand dollars, and large, complex tools can easily run half a million dollars or more.
What can I do with it?
Now that we know how sheet metal parts are produced, let’s talk about some possible features and things to keep in mind when you’re designing.
Some General Notes
Everything starts with a blank – All sheet metal parts (well, almost all of them) start out as a blank. A blank is a pattern of holes and features cut into a flat sheet of metal, which will then be bent up into a sheet metal part. Sheet metal is much easier to work with and transport when it’s flat, so shops want to do the bends last, as much as possible.
Everything is dependent on thickness – The thickness of your sheet stock determines the strength and weight of your part, and your minimum bend radii, punch size, and flange length. We’ll dig into all of that in a bit, but for now let’s just note that it’s hard to make small things out of thick metal. On the other hand, if your part is large and you need more strength, just increasing your material thickness is an easy design change.
You can’t make a part bigger than your sheet – Sheet metal comes in sheets, which means you can’t make a part that’s bigger than the sheet that you start with. It seems obvious, but when you start designing and wrapping metal around corners, it’ easy to forget and run out of sheet. Luckily, you can usually just get a bigger one – most vendors can handle sheets up to 48”x96” or even larger, so unless you’re making something REALLY big, you’re probably fine. If your part is larger than 96” long, then you probably want to start looking towards something like extrusion, roll forming, or joining separate parts together.
There are a wide variety of features that can only be fabricated by punching. We’ll take a look at some of my favorites here, but first, some general notes about punched features.
Punched features are created by punches, and punches are constrained by physics. The rule of thumb is that a punch should be at least twice as thick as the material it’s penetrating, which means you can’t have holes in your material that are narrower than twice your material thickness.
Punch direction is important! Punching and stamping leave a rounded edge where the tool enters and a sharper or more ragged edge on the opposite side (like a bullet hole, but much less dramatic). If one side of your part is going to face towards live electrical wires, assembly workers, or puppies, the sharp edges should probably point the other way. If you’re going to polish or powder coat the edges of this part later, you don’t need to worry about punch direction, but you’ll have to pay for the finishing.
Any feature that isn’t a straight-sided hole will need to be punched from a certain direction (something like a countersink, extruded hole, louver, knockout, etc). Once these features are punched, they stick up out of the material, and can hit the head of the CNC punch machine. Machine shops, understandably, want to avoid this. There are some clever ways to get around this, like bending a flange 180° after it’s punched or ordering a custom, reverse-direction form tool, but they’re much harder than just punching all your features the same direction.
Now, some of my favorite punched features;
- Extruded holes are the sheet metal equivalent of a screw boss. They can be tapped later, and readily accept self-tapping screws.
Though they’re expensive, bends are what give strength and shape to your sheet metal parts, so they’re incredibly important. Here are some general guidelines for all bend features.
Sheet metal can’t be bent to a perfectly sharp corner, so your bends will always have a radius. The smallest bend radius you can achieve is usually about the thickness of your material. Smaller bend radii cause stress concentrations in your part, and also require sharper tooling, which is difficult to maintain.
The minimum flange length for a bend is three times your material thickness. This should intuitively make sense. If you try to bend a flange that’s the same width as your material thickness, there’s no way to grab the metal in order to bend it.
There are several different types of bend features, with tradeoffs in expense, usefulness, and precision.
- Standard bends are just that – a bend in a piece of sheet metal. I’m noting them here so I can compare other things to them.
- Jog bends are two standard bends right next to one another. They’re useful for changing the height of your parts, adding a locating feature, or adding strength to parts. Because they’re so close together, special jog bend tooling can be used to form both bends at the same time, effectively giving you two bends for the price of one.
- Hand bends are a way to cheat and get bends for free. By punching a row of slots in your part, you create a line where the part will bend, and an assembly technician later bends the parts to their final shape. This lowers the cost of your parts, though it will increase your cost of assembly labor, but usually results in an overall savings. The bends you get are imprecise and weaker than a standard bend, but they can be left flat or bent up, which is handy if you need multiple configurations out of a single part. This is also a great hack for prototyping, if you want 3D parts out of your router, laser, or waterjet cutter.
- Hems are created by bending a flange of your part back on itself. This increases the strength of the hemmed edge and also gets rid of any sharp edges, which your technicians (and possibly your future self) will thank you for. The downside of hems is that they’re expensive (they usually take three bend operations to form) and add weight to your part.
- Cross-breaks are shallow bends across a wide, flat face. They give the part slightly more height, which stiffens it and helps it resist buckling. If your parts are less than 12” to a side, you probably don’t need to worry about them, but for larger parts, they can make a big difference.
Chamfers and Fillets
Unfinished sheet metal parts are sharp. Like, real sharp. And often heavy. You can use the corners of unfinished sheet metal parts to cut open boxes, if you don’t have a box cutter laying around. In the time before Mindtribe, I literally sent one of my coworkers to the hospital by leaving a prototype on their desk. It may seem silly, but chamfering your parts is actually a big deal.
Chamfering the outside corners of your parts removes the sharpest parts – it doesn’t remove all the danger, but it mitigates the worst of it.
Why chamfers and not fillets? A few reasons – a chamfer can be punched with any square or rectangular tool, but a fillet requires a special tool with the right radius. Because toolpaths don’t always line up perfectly, sometimes your fillet tool punches out extra material, which leaves two tiny, sharp 90° corners instead of one large one. Hardly any improvement. A misaligned chamfer tool just gives a slightly larger or smaller chamfer.