DFM Made Simple: A Practical Checklist for Engineers

Quick answer: Design for manufacture (DFM) means designing a part so it can be made and assembled easily, at the right cost, the first time. Most DFM problems come from a small number of habits: tolerances tighter than needed, features too close to bends or edges, too many different parts and fasteners, and a process that does not suit the quantity. Check those four things before you release a drawing and you will avoid most rework.

This guide is written for engineers and product designers who want a simple checklist they can use on their own designs. It is based on what we see every week in our workshop in Smithfield, NSW, and on established DFM references.

What is DFM?

DFM is the practice of checking a design against how it will actually be made. A part that works in CAD can still be slow, expensive or impossible to make. DFM finds those issues while they are still cheap to fix, on the screen rather than on the shop floor.

DFM vs DFA: DFM looks at each part and how it is made. Design for assembly (DFA) looks at how the parts go together. You need both. A cheap part that is hard to assemble is not a cheap part.

When should you do a DFM review?

Do it before you release drawings for quoting or manufacture, and again before any production run. The later a problem is found, the more it costs. A change in CAD costs minutes. The same change after tooling or a batch is made can cost weeks.

Step 1: Match the process to the quantity

The right process depends on how many you are making.

• 1 to 10 parts: 3D printing, laser cutting and folding, or CNC machining. No tooling.
• 10 to a few thousand: laser cutting and folding, CNC machining, simple fixtures.
• Thousands and more: stamping, casting or injection moulding start to pay for their tooling.

Ask yourself: is this design suited to the quantity I actually need? A part designed for injection moulding is often a poor choice if you only need 50.

Step 2: Sheet metal rules of thumb

These are general rules. Always confirm with your manufacturer, because tooling varies. T means material thickness.

• Bend radius: inside radius at least 1 x T for mild steel. Hard aluminium such as 6061-T6 needs a much larger radius or it may crack.
• Holes near bends: keep the edge of a hole at least 1.5 x T plus the bend radius away from the bend. Closer than that and the hole will distort.
• Holes near edges: at least 1 x T from the edge, and 1.5 to 2 x T is better.
• Hole size: hole diameter at least equal to the material thickness.
• Flange length: a bent flange should be at least 3 x T wide, and long enough for the press brake tooling.
• Bend relief: add relief cuts where a bend meets an edge, so the material does not tear.
• One thickness and one bend radius per part where possible. Every change means a tooling change.
• Countersinks in thin sheet: a machined countersink can leave almost no material in thin sheet. Use a thicker sheet, a formed (dimpled) countersink or flush hardware instead.
• Self clinching nuts and studs: every size has a minimum sheet thickness and a minimum distance to the edge. Check the manufacturer's data sheet before you pick one.
• Tolerances across bends: a dimension that runs across several bends builds up error. Dimension critical features from one face, or use slots so they can be adjusted.

Step 3: CNC machining rules of thumb

• Internal corners: cutters are round, so internal corners will have a radius. Allow a radius rather than a sharp corner. Larger radii cut faster.
• Hole depth: drilled holes up to about 3 x diameter deep are easy. Much deeper holes need special tools and cost more.
• Standard sizes: use standard drill and thread sizes.
• Thread depth: tapped threads deeper than about 2 x diameter add cost but almost no strength.
• Through holes are cheaper and easier to check than blind holes.
• Setups: design so features can be reached from as few sides as possible. Every extra setup adds time and error.
• Thin walls vibrate and distort when cut. Keep walls stiff enough to machine.
• Edges: do not write "remove all burrs". Say what edge break you need, for example 0.4 mm x 45 degrees.

Step 4: Tolerances, only where they matter

Tight tolerances are one of the biggest hidden costs in any design.

• Use a general tolerance block (for example ISO 2768-m) for everything that is not critical.
• Put tight tolerances only on fits, locations and features that affect function.
• Know what the process can hold. A laser cut part, a folded part and a ground shaft are very different.
• Use clear datums so the part is measured the same way it is made.
• State the result you need, not the process to get there.

Step 5: Assembly (DFA)

The cheapest part is the one you do not need. For every part, ask three questions:

1. Does it move relative to the parts around it?
2. Does it need to be a different material?
3. Does it need to be separate so the product can be assembled or serviced?

If the answer to all three is no, try to combine it with another part.

Then:

• Use one fastener size and type wherever you can.
• Assemble from one direction, ideally from the top down.
• Add locating features so parts find their own position.
• Make it hard to assemble wrong. Make the part clearly symmetrical, or clearly not.
• Leave room for tools to reach every fastener.

Step 6: Finishing and coating

• Powder coat adds thickness, typically 60 to 100 microns a side. Allow for it on fits and mask threads and mating faces.
• Earthing points need bare metal. If the enclosure is the earth path, plan where the coating is masked.
• Welded parts distort. Design for access to the weld and say which faces need machining after welding.
• Specify the finish you need, not more. A cosmetic finish on a hidden part is wasted money.

Step 7: 3D printed parts

3D printing is excellent for prototypes and one-offs. Know its limits:

• SLS nylon typically holds around ±0.3 mm. That is not good enough for bearing fits or precise locations.
• For a prototype, ream holes or use inserts where you need accuracy.
• For production, consider moving critical parts to machining or moulding, and redesign them for that process.

The DFM checklist (print this)

1. Does the process suit the quantity?
2. Are tolerances tight only where function needs them?
3. Is there a general tolerance block on the drawing?
4. Are datums clear and practical to measure?
5. Are holes far enough from bends and edges?
6. Are bend radii suitable for the material?
7. Is there one material thickness and one bend radius per sheet part?
8. Are bend reliefs included?
9. Do countersinks and clinch hardware suit the sheet thickness?
10. Do internal machined corners have a radius?
11. Are holes and threads standard sizes and sensible depths?
12. Can the part be machined in as few setups as possible?
13. Can any parts be combined?
14. Are fasteners standardised?
15. Does everything assemble from one direction?
16. Can every fastener be reached with a tool?
17. Is it hard to assemble the wrong way?
18. Have coating thickness, masking and earthing been allowed for?
19. Are weld access and distortion considered?
20. Has someone who will make the part looked at it?

Number 20 matters most. The quickest DFM check is to show the design to the person who will make it.

Need a second set of eyes?

McIver Engineering designs and manufactures in Smithfield, NSW. We review designs as the people who will make them, and we tell you plainly what will cause problems and what it will cost to fix. If you would like a DFM review of your design, contact us.