DFM checklist: design rules for moulded, sheet metal and machined parts
43 checks to run before you release a drawing, each with the number behind it and the guide it comes from. Tick them off as you review a part (your ticks stay in this browser), size features with the three calculators, and get the printable PDF for design reviews.
Rules from Protolabs, Hubs, Xometry, Stratasys Direct and Fathom design guides and Boothroyd-Dewhurst DFA · compiled by Skill-Lync · updated 16 Nov 2026
What is DFM, and why use a checklist?
Design for manufacturing (DFM) means shaping a part so the chosen process makes it cheaply, quickly and without defects. Most of a part's cost is fixed by its design: the process, the material, the number of features, the tolerances. A checklist catches the routine mistakes (a flange too short to bend, a sharp inside corner no cutter can mill, a thick boss that leaves a sink mark) before they reach the toolmaker.
The numbers below are starting points that manufacturers publish, not laws. Where guides disagree, we give the range and name the source. Your supplier's own limits always win: send them the model for a DFM review before freezing the drawing.
1. Every part, before the drawing is released
Checks that apply whatever the process. Most cost is locked in by these decisions, long before anyone cuts metal.
A mould or die is a large one-time cost that only pays back when it is spread over many parts.
Every tight tolerance adds inspection and often an extra operation. Most features never needed it.
Shops publish their own limits; theirs beat any generic rule, including the ones on this page.
2. Injection-moulded plastic parts
Most moulding defects (sink marks, warp, short shots, parts stuck in the tool) trace back to wall thickness, draft and thick spots.
Stress concentration rises steeply below an inside radius of half the wall; the matching outside radius keeps the wall constant round the corner.
3. Sheet metal parts
Sheet metal goes wrong at the bends: flanges too short for the press brake, holes that stretch into ovals, corners that tear.
4. CNC machined parts
Machining cost is driven by the number of setups, the number of tools, and how long and thin those tools have to be.
5. Assembly (DFA)
Design for assembly cuts parts, fasteners and handling time. Boothroyd and Dewhurst's three questions are the core of it.
How long should a flange be, how thick a rib, how big a corner radius?
Three DFM calculators. Enter your numbers; the rules above are applied to them. Results are guide values to start a design, then confirm with your supplier.
Sheet metal: flange, holes, notches and hems
- Minimum flange length
- 7.29 mm (2.5 × T + R)
- Features from a bend
- 7.29 mm or more
- Smallest hole or slot width
- 2 mm
- Hole to edge
- 3.18 mm or more
- Notch / tab width
- 2 / 4 mm min, length ≤ 5× width
- Hem
- inside Ø 2 mm, return 12 mm
Protolabs band 1.52–2.29 mm. Flange and feature distances: Protolabs toolkit table; holes, edges, notches, tabs and hems: Protolabs design guidelines.
Injection moulding: ribs, bosses, corners and draft
- Wall range for this resin
- 1.14–3.56 mm (in range)
- Rib thickness / max height
- 1.5 / 4.5 mm
- Rib spacing
- 6.25–7.5 mm or more
- Boss outside Ø / wall
- 6–7.2 mm / ≤ 1.5–1.75 mm
- Corner radii (inside / outside)
- 1.25 / 3.75 mm (2.5 mm inside if loaded)
- Draft on textured faces
- 2.97° or more
Wall ranges: Protolabs. Ribs: Xometry, Stratasys Direct. Boss: Fathom, Protolabs. Corners: Stratasys Direct, Fathom. Texture draft: Fathom (1° + 1° per 0.025 mm).
CNC machining: corners, pockets, holes and threads
- Inside corner radius
- 4 mm or more
- Pocket depth for this width
- ≤ 24 mm (OK)
- Hole depth
- 20 mm recommended, 50 mm typical
- Thread length
- 6–12 mm (M4: below M6, check tooling)
- Thinnest wall
- 0.8 mm metal, 1.5 mm plastic
- Standard tolerance
- ±0.1 mm (±0.02 mm possible)
All values: Hubs CNC machining design guide.
How do you check a part against a DFM checklist? Two worked examples
The bracket. 2 mm aluminium, bent on 2.29 mm (0.09 in) radius tooling. Protolabs' toolkit puts 2 mm aluminium in its 0.06–0.09 in band with a multiplier of 2.5, so the shortest flange the press brake can form is 2.5 × 2 + 2.29 = 7.29 mm. Say the first draft has a 6 mm return flange: too short. Either lengthen it to 7.5 mm or more, or drop to a smaller radius. The same 7.29 mm applies to clearance holes next to the bend: a hole drawn 5 mm from it would stretch. Holes need at least 2 mm diameter and 3.18 mm from an edge, both fine.
The cover. ABS, 2.5 mm wall, M3 heat-set inserts, light texture 0.05 mm deep. Ribs should be 1.5 mm thick at most and 4.5 mm tall at most; a stiffening rib drawn 2.5 mm thick and 10 mm tall would break both rules, so it becomes two ribs, 1.5 mm thick, 6.25 mm or more apart. Insert bosses get an outside diameter of 6–7.2 mm, tied to the side wall with a rib. The texture needs about 2.97° of draft, so side walls drafted at 1° should go to 3°. A 100 mm overall length should carry ±0.28 mm, not the ±0.1 mm copied from a machined part.
Skill-Lync's courses teach design for manufacturing and assembly on real products, in SOLIDWORKS, CATIA and NX.
- Design for Manufacturability (DFM): 5 weeks online, DFA, die casting, sheet metal, additive; 2 projects
- Post Graduate Program in Manufacturing Design
- Automotive Plastic Design using CATIA V5
- Advanced Sheet Metal Design using NX CAD
Frequently asked questions
What is a DFM checklist?
A DFM (design for manufacturing) checklist is a list of rules a design engineer checks before releasing a part, so it can be made cheaply and reliably by the chosen process: wall thickness and draft for moulding, bend radius and flange length for sheet metal, corner radii and hole depth for machining. This one has 43 checks across 5 groups.
What is the difference between DFM and DFA?
DFM (design for manufacturing) makes each part easy to make by its process. DFA (design for assembly) makes the product easy to put together: fewer parts, fewer fasteners, parts that cannot go in the wrong way. Together they are called DFMA. DFA usually saves more, because every part it removes also removes its manufacturing cost.
What is the minimum flange length for sheet metal?
It depends on material and thickness. Protolabs' toolkit gives 2.5× to 4× the sheet thickness plus the inside bend radius; its simpler guideline is at least 4× the thickness. For 2 mm aluminium with a 2.29 mm bend radius that is 7.29 mm. Below the minimum, the press brake cannot grip the flange.
How thick should ribs be in injection moulding?
Ribs should be no thicker than about 60% of the wall they stand on, and around 40% on glossy show surfaces, or the thick base shows as a sink mark on the other side. Keep them under 3× their own thickness in height and space them at least 2.5–3× the wall apart.
How much draft angle does an injection-moulded part need?
Use at least 0.5° on faces parallel to the mould opening; 2° works for most parts. Textured faces need more: a common rule is 1° plus 1° for every 0.025 mm (0.001 in) of texture depth, so a 0.05 mm texture needs about 3°. Shut-off faces need 3° or more.
What is the minimum inside corner radius for CNC machining?
An end mill is round, so inside vertical corners always have a radius. Hubs recommends at least one-third of the pocket depth: a 12 mm deep pocket gets a 4 mm radius or more. Larger radii let the shop use a bigger, stiffer tool, which machines faster and more accurately.
Which jobs use DFM?
Design engineers, product design engineers and manufacturing engineers in automotive, consumer products, appliances and medical devices apply DFM daily, and interviews for these roles test it with questions like the ones on this page. Skill-Lync's Design for Manufacturability course and design programs teach it on industry projects.
Related on Skill-Lync
- FMEA RPN and Action Priority calculator
- Tolerance stack-up calculator: worst case, RSS and Monte Carlo
- GD&T symbols explained: chart, datums and MMC
- Understanding design for manufacturing and assembly (DFMA)
- DFMA for snap fits in plastics
- Plastics joining methods
- Mould design: the DFM checklist for tooling
- Springback in sheet metal
- All Skill-Lync CATIA courses
Sources
- Protolabs, Design Guidelines for Sheet Metal Fabrication
- Protolabs, Design for Sheet Metal Fabrication Toolkit (flange and feature-to-bend tables)
- Protolabs, Injection Molding Design Guidelines
- Protolabs, Design Better Screw Bosses on Molded Parts
- Stratasys Direct, Injection Molding Design Guidelines (2017)
- Fathom, Design Guidelines for Injection Molding (rev. 05152025)
- Xometry, Plastic Ribs for Injection Molding Design
- Hubs, How to design parts for CNC machining
- Fabcon, Sheet Metal DFM Guide: Rules, Failure Modes and Review
- Boothroyd, Dewhurst and Knight, Product Design for Manufacture and Assembly (3rd ed., CRC Press, 2011)
Figures in square brackets after a check point to these sources. All guides checked on 16 Nov 2026. Where two guides differ (for example, the inside corner radius for moulded parts: 0.5× wall in general, 1× where the corner is loaded), both values are given.