Overview#
CAD will happily let you model parts nobody can make. Design for manufacture (DFM) is the habit of checking geometry against process limits before sending files out. The numbers below are common guidelines, not standards; your vendor's published capabilities and your resin's data sheet take priority. Where Fusion helps (rules, Design Advice, flat pattern), this page says so.
Where to find it#
- Sheet metal checks: the Flat Pattern (Sheet Metal > Create), Inspect > Measure, and sheet metal rule values.
- Plastic checks: Plastic rule Design Advice, Inspect > Draft Analysis, Inspect > Section Analysis.
- Vendor-specific DFM: most online shops provide an automatic DFM report when you upload a DXF or STEP.
Step by step#
Sheet metal DFM checklist#
- Choose a standard thickness available from the vendor.
- Set the rule to the vendor's bend radius and K-factor.
- Check minimum flange length (about 4 times thickness plus radius, or the vendor's chart).
- Keep holes at least 2 to 2.5 times thickness plus bend radius away from bends so they do not distort.
- Keep hole diameters at least equal to thickness (laser) and larger for punching.
- Add reliefs at the end of bends that meet a flat edge; add corner reliefs at box corners.
- Keep slots and tabs wider than the thickness, with a corner radius not sharp corners.
- Keep all bends in the same direction accessible; avoid bends that trap the tool (deep narrow U shapes).
- Make the flat pattern, check overall size against the sheet, and export DXF.
- Add notes: material, finish, thickness, deburr, tolerance.
Injection molding DFM checklist#
- Define the pull direction and parting line first.
- Keep walls uniform; transition thick to thin gradually (3:1 taper).
- Add draft of 1 to 2 degrees on all faces parallel to pull, more on textured faces.
- Use radii at all inside corners (at least half the wall) and outside (inside radius plus wall).
- Rib thickness 50 to 60 percent of the wall; height under 3 times the wall.
- Core out bosses; connect with ribs; avoid isolated thick sections.
- Avoid undercuts, or plan side actions and lifters (cost increases).
- Locate gate, ejector pins and sink-prone areas with the molder.
- Run Design Advice, draft analysis and section analysis.
- Ask the molder for a DFM review before cutting steel.
Options reference#
| Topic | Sheet metal | Injection molding |
|---|---|---|
| Thickness | Single uniform thickness (rule) | Nominal wall, uniform, within range |
| Radii | Bend radius at least equal to material limits | Inner radius at least half wall |
| Holes / features near edges | At least 2 to 2.5 x thickness from bends and edges | Keep bosses away from thin walls without ribs |
| Reliefs | Bend and corner reliefs | Fillets and gradual transitions |
| Draft | Not needed | Required on all pull-direction faces |
| Software aids | Sheet Metal Rules, Create Flat Pattern, DXF | Plastic rules, Design Advice, Draft analysis |
| Undercuts | Hems, returns limited by tooling | Side actions, lifters, collapsible cores |
Tips and pitfalls#
Tip: Ask the vendor for a design guide or "design for manufacturing" PDF; many publish bend radius, minimum flange and hole rules per material.
Tip: Standardise bend radius across the part to cut setup changes; every different radius is a different punch.
Warning: Tolerances. Bent features typically hold plus or minus 0.25 to 0.5 mm and about plus or minus 1 degree, laser-cut edges tighter. Do not dimension bends as if they were machined.
Warning: Sheet metal grain direction affects crack risk on tight bends. Orient critical bends across the grain.
Warning: Do not assume the plastic rule's advice is complete. Warpage, weld lines and gate position are not modelled by geometry rules; use mold flow analysis if the part is critical.
Tip: Prototype with 3D printing, but remember printed ribs and bosses behave differently than molded ones.
Turning guidelines into checks you can run in Fusion#
| Check | Where | How to read it |
|---|---|---|
| Minimum flange or bend leg | Measure on the flat pattern or the folded body | Compare with about 4 x thickness + radius |
| Hole-to-bend distance | Measure from the hole edge to the bend line on the flat pattern | At least about 2.5 x thickness + radius |
| Hole size | Measure the hole diameter | At least about the thickness for laser (more for punching) |
| Flat pattern size | Measure bounding box | Compare with the sheet or bed |
| Draft | Inspect > Draft Analysis | All pull-direction faces drafted |
| Wall thickness | Section Analysis or Design Advice | Within the rule range |
| Undercuts | Draft Analysis with the pull direction set | Faces showing as undercut need cores |
Worked sheet metal example#
A 2 mm stainless 304 bracket, 2 mm inside radius, laser-cut. Minimum flange = 4 x 2 + 2 = 10 mm. The part has a 12 mm flange, which passes. Holes must be at least 2 x 2 + 2 = 6 mm (using the lower end of the 2 to 2.5 guideline) from the bend: a hole 5 mm from the bend fails and should move 1 mm outward or become a slot. Hole diameter 3 mm is acceptable for laser cutting stainless (at least equal to the 2 mm thickness). A 1.2 mm wide slot would fail because it is narrower than the thickness. Corner relief: round, 4 mm. This takes minutes to check on the flat pattern and avoids a rejected quote.
Tolerances you can realistically hold#
| Feature | Typical achievable | Note |
|---|---|---|
| Laser-cut profile | plus or minus 0.1 to 0.2 mm | Better on thinner sheet |
| Hole position (laser) | plus or minus 0.1 to 0.2 mm | |
| Bend angle | plus or minus 1 degree | Springback varies by material |
| Bend-to-edge dimension | plus or minus 0.25 to 0.5 mm | Accumulates over several bends |
| Injection moulded linear | roughly plus or minus 0.1 to 0.3 percent plus a base value | Depends on resin, shrinkage and size |
| Draft angles | 0.5 to 3 degrees | Texture needs more |
These are generic figures to compare with a vendor's published capabilities. With three bends, a stack of plus or minus 0.3 mm per bend can give plus or minus 0.9 mm on the final position, so dimension from a common datum rather than chaining.
Moulding: the order of decisions#
- Pull direction and parting line. Everything else depends on these. Use Draft Analysis to find undercuts.
- Wall thickness. Choose it from resin and flow length. Flow length divided by wall ratios of about 100:1 to 200:1 are common for easy-flowing resins, so a 2.5 mm wall can fill 250 to 500 mm from the gate.
- Draft. 1 to 2 degrees general, more with texture.
- Ribs, bosses and snaps. Sized to the wall as covered on the previous two pages.
- Gate, ejector pins and cooling. Agree these with the molder.
Worked tolerance example#
A 100 mm moulded dimension in ABS with 0.5 percent shrinkage is designed 100.5 mm in the mould. If the shrinkage varies by plus or minus 0.1 percent, the part varies by plus or minus 0.1 mm. A press-fit that needs plus or minus 0.05 mm will not hold without secondary machining, so design features to be adjustable or tolerant (snap fits, slots) rather than precise.
Cost drivers: a quick comparison#
| Choice | Sheet metal effect | Moulding effect |
|---|---|---|
| More bend radii | Extra tooling changes | Not applicable |
| Tighter tolerance | More inspection, more scrap | More mould iterations |
| Thicker material or wall | Higher material cost | Longer cycle time (about squared) |
| Undercut or hem | Extra operations | Side actions or lifters, higher tooling cost |
| Small quantities | Laser and brake are cost-effective | Tooling cost dominates; consider printing or machining |
For quantities of a few hundred, 3D printing or CNC may beat tooling; for tens of thousands, moulding wins. Use the vendor's quote tool to find the crossover for your part.
Common failures and fixes#
| Symptom | Cause | Fix |
|---|---|---|
| Vendor rejects the DXF | Holes near bends, tiny slots | Move features, enlarge slots |
| Parts do not fit after bending | K-factor mismatch or tolerance stack | Match the vendor's K-factor; datum from one edge |
| Moulded part warps | Uneven wall or thick sections | Even out walls; core out pads |
| Sink marks on the cosmetic face | Ribs or bosses too thick | Thin the ribs to about 50 percent; use a textured finish |
| Ejection marks or drag | Insufficient draft | Add 1 to 2 degrees; increase on texture |
| Quote is far higher than expected | Undercuts, tight tolerances | Simplify, or loosen non-critical tolerances |
Practice exercise#
Audit two parts against the checklists and produce a measured change list.
- Take your L-bracket from the sheet metal pages (2 mm material, 2 mm radius). Open its flat pattern and measure: the minimum flange (compare with 10 mm), the distance from each hole edge to the bend line (compare with 6 to 7 mm), each hole diameter (at least 2 mm) and the bounding box.
- Write down every violation with the measured value and the limit. Fix at least two in the model, for example move a hole from 4 mm to 8 mm from the bend, and rebuild the flat pattern.
- Take the enclosure from the Lip and Snap Fit page. Run Inspect > Draft Analysis with the pull direction set to Z, and list faces without draft. Measure at least three wall thicknesses with Section Analysis.
- Check rib thickness (target 40 to 60 percent of the wall) and boss outer diameter (about 2 to 2.5 times the screw diameter), and fix any that fall outside.
- Compute the tolerance stack for a three-bend part with plus or minus 0.3 mm per bend, and decide whether any dimension should be re-datumed to a single edge.
Expected result: a written list of at least four measured violations with before and after values, for example a hole moved from 4 mm to 8 mm from a bend and a rib reduced from 2.5 mm to 1.4 mm, plus the computed stack of plus or minus 0.9 mm.