DFM Guide and Pre-submission Checklist
Design rules for CNC machining, 5-axis, sheet metal, 3D printing, injection molding and finishing, and what to send with your files. Every design still gets an engineer review.
Pre-submission Checklist
Send these with your files and the quote comes back faster, with fewer questions. An engineer reviews every order either way.
| Send | What to include | Why it matters |
|---|---|---|
| 3D model | STEP or IGES for machined parts. STEP, STL or 3MF for printed parts, with STEP preferred for metal. DXF or DWG also works for sheet metal | The model sets the geometry that is quoted and made |
| 2D drawing | Tolerances, GD&T callouts, threads and inserts, and critical dimensions | Fine threads, custom pitches and inserts are only made when the drawing calls them out |
| Quantity | The prototype quantity, and expected production volumes if known | Setup and tooling costs are spread across the batch, so unit price depends on quantity |
| Material | The alloy or grade, for example 6061-T6 or 316L | Alloys finish differently. 2024 varies, and cast alloys typically cannot be hard anodized to a cosmetic standard |
| Finish | The finish spec, and the post-treatment dimensions for tight features | Anodize and plating add thickness, so dimensions are worked back from your post-treatment sizes |
| Masking | Threads, precision bores and sealing faces that must stay as machined | Without a note, coating can land on features that need to stay bare |
| Sheet metal details | Thickness, hardware, weld locations, and an assembly drawing for assemblies | The weld sequence affects final dimensions |
| 3D print details | Main load direction and which faces are cosmetic | Prints are weaker in the layer direction, so orientation follows the load |
NDAs are available on request, before you share files.
CNC Machining
These four rules keep cost and lead time down. Parts that break them can usually still be made, and the design review will say how.
Internal Corners
Use a radius of at least 0.5 mm. A third of the pocket depth is a safe start.
Sharp inside corners. They need EDM or grinding and add lead time.
Wall Thickness
Keep walls at 1.5 mm or more. They stay stable during cutting in most materials. Aluminium walls can go down to 0.8 mm.
Thinner walls without flagging them. They flex under the cutter, and thin titanium walls need special fixturing.
Pocket Depth
Keep pockets no deeper than four times their width.
Deep narrow pockets cut from one side. Long tools deflect, so tight tolerances get harder to hold. Cut them from several sides or in stages.
Threads
Use standard coarse metric (M) or UNC threads. They are the fastest and cheapest.
Leaving fine threads, custom pitches or Heli-Coil inserts off the drawing. All of them are available when the drawing calls them out.
Specifications, materials and finishes are on the CNC machining page
5-Axis Machining
Treat these as guidance. If your geometry does not fit them, send it anyway and an engineer will advise.
Undercuts and Angled Features
Annotate undercut depths, angled bore directions and compound angles on the drawing, so the toolpath is planned before the quote.
Leaving them unmarked, so geometry constraints turn up mid-job instead of at quoting.
Tolerances Across Faces
State tight positional relationships between faces explicitly on the drawing. Callouts of ±0.02 mm or tighter across faces rely on the single setup.
Leaving cross-face relationships off the drawing, with each face dimensioned on its own.
Freeform Surfaces
Send the STEP model, because for compound-curved and freeform geometry it is the drawing. Add Ra callouts and any curvature tolerances for those faces.
Relying on 2D section views. They do not capture enough of the surface.
Fixturing Access
Give the part a secure clamping face that leaves every machined surface reachable on the rotary table.
Very large flat parts, or parts with no good clamping face, sent without a flag. They may need a custom fixture.
Specifications, materials and finishes are on the 5-axis machining page
Sheet Metal Fabrication
Treat these as guidance. Every design gets an engineer review whether or not it meets them.
Bend Radius and Flange Length
Use an inside bend radius of at least 1 × material thickness, and make flanges at least 4 × thickness long so the press brake can grip them.
Radii under 1 × thickness, which risk cracking, and short flanges. Some alloys take tighter radii after DFM review.
Holes Near Edges and Bends
Keep holes at least 2 × thickness from an edge, and 3 × thickness plus the bend radius from a bend.
Holes closer than that, because they deform during forming. Mark critical dimensions on the drawing so problems are flagged before cutting.
Grain Direction
Bend across the rolling grain, especially for tight-radius bends in aluminium and high-strength steel.
Tight bends along the grain, where cracking is more likely. For bends in several directions, blank orientation is confirmed during DFM.
Hardware and Weld Placement
Keep PEM fasteners and weld nuts clear of bends and edges, typically by 3 × their outer diameter. Mark weld locations and access needs on the drawing.
Fasteners crowded against a bend, or weld locations left off the drawing. The weld sequence affects final dimensions.
Specifications, materials and finishes are on the Sheet metal fabrication page
3D Printing
Guidance rather than fixed limits. If you are not sure a lattice, overhang or other feature will print, send the file and an engineer will advise.
Wall Thickness
Keep walls at or above the process minimum: 0.4 mm for DMLS, 0.5 mm for SLA, 0.7 mm for SLS and MJF, and 1.2 mm for FDM.
Thinner walls without flagging them in your brief. They are sometimes possible but risk failing or warping.
Build Orientation
Tell us the main load direction and which faces are cosmetic, and the part will be oriented to suit.
Assuming a print is equally strong in every direction. All additive processes are anisotropic, and parts are weaker in Z, the layer direction, than in X and Y.
Tight Tolerances
Add 0.3 to 0.5 mm of stock to interface bores, sealing faces and threads that need tighter than ±0.1 mm, so they can be CNC machined after printing.
Modelling those surfaces at final size, which leaves no stock to machine. Print the geometry and machine the interfaces.
Overhangs on Metal Prints
DMLS and SLM need supports on overhangs more than 45° from vertical. Design those supports to be removable, with access ports to reach them.
Supports that cannot be reached after printing. Expect a rougher finish where supports attach on interior surfaces.
Specifications, materials and finishes are on the 3D printing page
Injection Molding
Guidance rather than fixed rules. Send the design either way: the DFM review checks every part, including multiple undercuts, tight tolerances and unusual materials.
Draft Angles
Add 1 to 3° of draft to faces parallel to the pull direction so the part releases cleanly. Textured surfaces typically need 3 to 5°.
Zero-draft faces. They are possible with side-pulls, but add tooling cost.
Uniform Wall Thickness
Keep walls uniform, between 1.0 and 4.0 mm. Where a thick section is unavoidable, core it out to cut mass without losing stiffness.
Thick sections. They cool unevenly and cause sink marks or warpage.
Gates and Parting Line
Place gates on non-cosmetic surfaces where possible, and confirm the parting line location early.
Gates on cosmetic faces, or a parting line left until late. Gate marks are visible, and the parting line sets where the seam sits and where flash can form.
Undercuts and Side Features
Where possible, redesign undercuts to form through or to be reachable from the parting line.
Undercuts that block straight ejection. They need side-pulls, lifters or collapsible cores, which add tooling cost.
Specifications, materials and finishes are on the Injection molding page
Surface Finishing
Check these four points before you finalise the drawing. The DFM review covers them too.
Masking
Mark threads, precision bores and sealing faces that must stay as machined, for example "mask M5 holes".
Leaving masking off the drawing. The DFM review flags features that likely need it, but a note up front saves time.
Surface Finish
Machine to Ra 0.8 µm or better before decorative anodize or bright plating, and put the finish on the drawing.
Relying on the coating to hide machining marks. It follows the surface underneath.
Coating Buildup
Machine tight-tolerance features to pre-treatment size and give post-treatment dimensions on the drawing. We work back from those.
Ignoring buildup. Type II anodize adds about 2.5 to 12.5 µm per surface, Type III up to 38 µm and electroless nickel up to 50 µm.
Alloy Choice
Call out the alloy on the drawing. 6061 and 7075 anodize well, and we will flag any process limits.
Expecting every alloy to finish the same. 2024 varies, and cast alloys typically cannot be hard anodized to a cosmetic standard.
Specifications, materials and finishes are on the Surface finishing page
Send a Part for Review
Factorem has made parts for 300+ engineering teams, with 98% of orders delivered on time and 98%+ of parts accepted.
