Design for manufacture (DFM) by process, with rules of thumb

Design for manufacture, usually shortened to DFM, is the practice of shaping a part around the process that will make it, so it can be produced reliably, with little scrap and at the cost the product needs. A design that ignores the process can usually still be made, but it pays for that in extra operations, special tooling, slow cycle times or rejected parts. Most of a part’s cost is fixed by decisions taken in the CAD model, long before a supplier sees it.

The rules differ by process because each process has its own physics and its own tools. A milling cutter is round, so it cannot leave a sharp internal corner. Molten plastic shrinks as it cools, so thick sections sink. A press brake bends sheet around a punch of finite radius, and welding heat distorts whatever it touches. Once you know what the tool is doing, most DFM rules follow from it, and you can judge when one can safely be bent.

Choose the process first

DFM starts with the process, and the process depends mostly on volume, material and geometry. A housing needed in tens is usually machined or printed. As volumes rise into the thousands, injection moulding or die casting starts to pay back its tooling. A bracket may be laser cut and folded at almost any volume. Changing process once the design is detailed is expensive, so settle the choice at concept stage, even provisionally.

CNC machining

Machining removes material with rotating cutters, so its rules are mostly about tool access and rigidity.

• Internal corners. An end mill leaves a radius equal to its own. Specify internal radii slightly larger than a standard cutter radius, so the tool can move round the corner without dwelling, and larger still in deep pockets, where a stiff cutter has to be a thick one. Where a square-cornered mating part has to sit in the corner, a dog-bone relief does the job. Sharp corners also raise stress, as our guide to stress concentration factors explains.
• Pocket and slot depth. Depths up to about three or four times the cutter diameter machine without fuss. Deeper features need long-reach tooling and lighter cuts.
• Thin walls and webs. Walls below about 1 mm in metal, or about 1.5 mm in plastics, deflect under the cutter and can move once released from the fixture, especially where machining unbalances residual stress in the stock.
• Holes. Use standard drill sizes and keep drilled depths to a few diameters where possible. A blind hole with a drill-point bottom is cheaper than a flat-bottomed one, so accept the cone if the function allows it.
• Threads. Thread engagement beyond about 1.5 times the diameter in steel adds little strength. In aluminium, around twice the diameter is a common allowance.
• Set-ups. Each re-clamping adds cost and loosens the relationship between features on different faces. Put features on as few faces as possible, and give the machinist a flat face and a clear datum to clamp from.

The thin aluminium disc case study shows what happens at the edge of these rules: a disc with a 1.2 mm web that warped after machining and anodising, most likely from residual stress released unevenly plus heat from sealing. The remedies lay in the material, machining, fixturing and finishing together.

Injection moulding

A moulded part is formed by filling a steel or aluminium cavity with molten polymer under pressure, holding it while it cools and pushing it out. Most moulding rules come from the cooling and the ejection.

• Wall thickness. Keep it as uniform as possible. Most thermoplastic parts sit between about 1 mm and 3 mm, depending on the material and how far the melt has to flow. Where thickness has to change, taper it over a length of around three times the difference.
• Draft. Faces parallel to the direction the tool opens need a taper so the part releases. One to two degrees is a common default, with half a degree as a practical minimum on smooth faces. Textured faces need more, often about an extra degree for every 0.025 mm of texture depth.
• Ribs. Stiffen with ribs in preference to thicker walls. A rib about 50 to 60% of the adjoining wall thickness avoids sink on the opposite face. Keep rib height to about three times the wall, space ribs at least twice the wall apart, and give them a small root radius.
• Bosses. Make screw bosses about twice the screw diameter outside, keep the boss wall thinner than the main wall, and tie tall bosses to nearby walls with ribs.
• Corners. Sharp internal corners concentrate stress and hinder flow. An inside radius of at least half the wall thickness, with the outside radius equal to the inside radius plus the wall, keeps the wall uniform round the bend.
• Sink and voids. Thick sections cool last and pull material away from the surface as they shrink, leaving a shallow depression on the visible face or a void inside. Coring out thick areas is the reliable cure; higher hold pressure helps only so far.
• Injection point and weld lines. Where the melt enters the cavity governs how it fills and where flow fronts meet. Meeting fronts form weld lines, which are weaker and often visible, so position the injection point to keep them off load paths and cosmetic faces, and fill from thick sections towards thin ones.
• Undercuts. Any feature that stops the part being pulled straight out of the tool needs a side action, a lifter or a collapsing core, each adding cost and maintenance. A shut-off through the part, or a window in the wall below a clip, often removes the undercut.

Material choice moves these values. Amorphous polymers such as ABS and polycarbonate shrink less and more evenly than semi-crystalline ones such as polypropylene, acetal and nylon, and glass-filled grades shrink differently along and across the flow.

Sheet metal

Sheet parts are cut by laser, punch or waterjet and then bent, usually on a press brake. The rules follow from the way metal stretches on the outside of a bend and compresses on the inside.

• Bend radius. An inside radius equal to the sheet thickness suits mild steel, stainless steel and the softer aluminium alloys. Harder tempers such as 6082-T6 crack at tight radii and need a larger radius, or a more formable grade such as 5251 or 5083. Use one radius throughout the part where you can, so one tool set makes every bend.
• Flange length. A flange needs enough length to bridge the die. Around four times the thickness is a common minimum.
• Bend relief. Where a bend stops short of an edge, cut a relief so the material does not tear. Make it at least as wide as the thickness, and run it past the bend line by about the thickness plus the bend radius.
• Holes near edges and bends. Keep holes at least 1.5 to 2 times the thickness from an edge. Near a bend, holes distort unless they sit about 2.5 times the thickness plus the bend radius away from it. Holes smaller in diameter than the thickness are hard to punch cleanly.
• Flat pattern. The developed length depends on the bend allowance, usually set through a K-factor between about 0.3 and 0.5. Agree it with the fabricator, or let them develop the flat pattern from your 3D model.

Fabrication and welding

Welded frames and structures are built from plate and standard sections. Distortion and access cause most of the trouble, with fatigue a concern wherever loads cycle.

• Use standard section sizes and plate thicknesses, and as few different ones as the design allows.
• Size welds to the load. Over-welding adds heat and distortion. For an equal-leg fillet weld the throat, which carries the load, is about 0.7 times the leg length.
• Leave room for the torch. A joint the welder cannot see or reach at a sensible angle will be a poor one.
• Balance welds about the neutral axis of a member where possible, and expect a long weld on one side to bow it.
• Machine critical faces and bores after welding. Welding heat moves everything, so features that must hold tenths of a millimetre should be cut once the frame has been welded and, where necessary, stress relieved.
• Keep welds away from the most highly stressed regions of cyclically loaded parts. Weld toes are the usual starting point of fatigue cracks, as our fatigue analysis guide describes.
• Add vent and drain holes to hollow sections that will be hot-dip galvanised.

Additive manufacturing

Building layer by layer removes most tooling constraints and introduces a few new ones.

• Overhangs. In FDM and metal powder bed fusion, surfaces inclined more than about 45° from vertical need support, which adds time and leaves marks. SLS builds in a bed of powder that supports the part, so it needs none.
• Walls and holes. Minimum practical walls are around 0.8 to 1 mm for most polymer processes. Small holes tend to print undersize and are often drilled or reamed afterwards.
• Anisotropy. FDM parts are much weaker across their layers than along them, so orient the part with the main load running along the layers.
• Powder and resin removal. Hollow SLS, SLA and metal parts need escape holes so unfused powder or uncured resin can be cleared out.
• Post-machining. Metal printed parts usually need stress relief and machining on the faces that locate, seal or carry bearings, so leave stock on those faces.

Typical rules of thumb

These are commonly used starting points. Material grade, part size and the supplier’s equipment all move them, and a supplier’s own guidance takes precedence.

Tolerances, finishes and the cost of asking

DFM also covers what the drawing asks for. Each tight tolerance, fine surface finish or special treatment adds an operation or an inspection, and sometimes scrap. Apply them where the function depends on them, at bearing seats and sealing faces for example, and let everything else fall under a general tolerance. Our guide to manufacturing drawings and tolerances covers how to set them.

How SixGate™ can help

In SixGate™’s Detail & Simulation stage, the chosen concept becomes a detailed 3D model in Autodesk Inventor, designed for manufacture by the process that will make it, with FEA, CFD or DEM wherever the product needs it. You receive parts whose geometry already reflects how they will be made, which keeps the drawing pack and the supplier quotes that follow free of avoidable surprises. If you have an existing design that is proving expensive or awkward to make, the same work can start from your current model.