Two engineers can draw the same metal bracket, functionally identical, and get quotes that differ by a factor of four. The difference is never material cost. It is a set of geometric decisions — a bend radius that forces a special tool, a sharp internal corner, a wall thinner than the casting can fill, a weld a torch cannot reach — each quietly adding an operation, a setup, or a scrap rate.
These rules are not secret, just rarely collected in one place. Here they are, organized by process, with the reasoning behind each so you can apply them to cases this article does not cover.
Sheet metal rules
Bend radius
A bend has a minimum inside radius below which the outer fiber cracks. The working rule is an inside radius at least equal to material thickness for mild steel and most aluminum, and one and a half to two times thickness for harder tempers like 6061-T6. More important than the exact number: use the same inside radius on every bend in the part, because each distinct radius means a different punch and another setup on the press brake.
Flange length and hole spacing
A flange must be long enough for the brake tooling to grip — roughly four times thickness plus the bend radius. Holes too close to a bend distort into ovals; keep hole edges at least two and a half times thickness plus the radius from the bend line, or pierce them after forming at the cost of a second operation.
Bend relief
Where a bend ends partway across a face, the material tears at the transition unless you cut a relief notch — at minimum as deep as the bend radius plus thickness and as wide as the material thickness. Omitting reliefs is the single most common sheet metal drawing error.
K-factor and flat patterns
Bending stretches the outside and compresses the inside, so the flat blank is not the sum of the leg lengths. Let the fabricator generate the flat pattern from your 3D model using their own K-factor. The rest of the rule set is in the sheet metal design guide.
Machined part rules
Internal corners must have a radius
A milling cutter is round, so an internal vertical corner always has a radius. Specify one at least a third of the pocket depth — larger radii let the shop use a bigger, stiffer cutter that removes material faster, and going from 0.032 in to 0.125 in can cut cycle time substantially on a deep pocket.
Depth-to-diameter limits
Tools deflect and chatter as they get longer. Keep pocket depth under about four times the cutter diameter, and drilled hole depth under about five times hole diameter, unless you are prepared to pay for gun drilling. Deep, narrow features are the most reliable way to make a machined part expensive.
Minimum wall thickness
Thin walls chatter and deflect under cutting force. Hold at least 0.030 in in aluminum and 0.040 in in steel, more if the wall is tall.
Setups are the real cost driver
Every time the part is unclamped and reoriented, you pay for fixturing, alignment, and lost accuracy between faces. Features on two opposite faces are cheap; features on five faces need either a five-axis machine or four setups. This is where 3-axis vs 5-axis machining economics bite, and where designing parts to cut CNC cost pays back within the first order.
Choose the alloy for machinability
Machinability varies enormously. Free-machining brass and 6061 aluminum cut fast; 304 stainless work-hardens and cuts slowly; titanium is slower still and eats tooling. Do not specify stainless reflexively — the tradeoff is covered in aluminum vs steel.
Casting rules
Draft
Every surface parallel to the direction the part leaves the mold needs draft, or it will not release. Typical values run 1 to 2 degrees for die casting, 1 to 3 for investment casting, and 2 to 5 for sand casting. Interior surfaces need more than exterior ones because the casting shrinks onto the core.
Uniform wall thickness
Thick sections cool last and shrink into voids and porosity. Keep walls as uniform as you can, and where a thick section is unavoidable, core it out. Die casting typically runs 0.06 to 0.12 in walls in aluminum; sand casting needs much more.
Fillets and ribs
Every internal corner gets a generous fillet — sharp corners are stress risers and they cause hot tearing during solidification. Stiffness comes from ribs, not from thick walls, and ribs should be thinner than the wall they support to avoid sink and porosity at the junction.
Machining allowance and parting lines
Add stock to any surface that must be accurate, and put the parting line on an edge — across a cosmetic face it leaves a visible flash line that has to be dressed off.
Weld design
Welding is where designs that look fine in CAD become impossible in a shop.
- Access. A torch and the welder's hand need physical room. If a joint sits at the bottom of a box that is closed on five sides, nobody can weld it. Check access in the model before you release it.
- Distortion. Heat shrinks the joint as it cools and pulls the assembly out of square. Symmetric welds on both sides of a neutral axis cancel each other; a single long weld on one side will bow the part.
- Don't over-weld. A continuous bead is rarely needed. Stitch welds carry most loads fine, cost less, and distort far less.
- Tolerance after welding. Do not specify tight dimensions across a welded joint; machine the assembly afterward or move the tolerance to a feature the heat did not reach.
- Dissimilar metals. Aluminum to steel cannot be conventionally welded. Use fasteners, transition joints, or redesign.
Fasteners and threads
Threading directly into thin sheet does not work — you need at least one and a half thread diameters of engagement. In sheet metal, use self-clinching nuts or studs, far stronger than an extruded and tapped hole. In machined parts, thread depth of one and a half diameters in steel and two in aluminum is plenty; deeper threads add cost and carry no extra load.
Prefer coarse threads unless you need fine adjustment, and keep distinct fastener sizes to two or three — every extra size is another bin and another chance for the wrong screw. Anything that vibrates needs a deliberate anti-loosening strategy.
Finish allowance and corrosion
Every coating has thickness, and it lands on your tolerances. Typical values worth designing around:
| Finish | Thickness added per surface | Design consequence |
|---|---|---|
| Type II anodize | 0.0002–0.0008 in | Mask threads and press-fit bores |
| Type III hard anodize | 0.001–0.003 in | Roughly half grows outward; adjust nominal size |
| Electroplating | 0.0002–0.001 in | Builds up on edges and corners |
| Powder coat | 0.002–0.004 in | Mask mating faces and ground points |
| Paint | 0.001–0.003 in | Will not hide machining marks |
Anodizing is not conductive, so grounding and bonding surfaces must be masked. Mixed metals in contact create galvanic corrosion, particularly aluminum against stainless in a wet environment. The full picture is in corrosion protection for metal parts.
Put it on the drawing
None of these rules helps if the shop cannot see your intent. A metal part drawing needs material and temper, critical dimensions with tolerances, surface finish callouts, thread specs, masking notes, weld symbols, and the datum surfaces it is inspected from. What belongs on the sheet is spelled out in what a manufacturing drawing must include, and the general discipline in design for manufacturing.
Projects House does metal part design and DFM review as a standard part of product development. If you have drawings that came back with surprising quotes, send them through our contact form and we will tell you which rules the design is breaking.