Support Hours: 09:00–18:00 (GMT+8) · Messages and quote requests are accepted 24/7.

Find the DFM Answer You Need

Jump to process-specific design rules, cost drivers, inspection inputs or quote-preparation answers.

DFM Reference Values by Process

Use these starting values to compare process fit and identify design risks. Final capability depends on material, size, geometry, finish, quantity, inspection and assembly requirements; upload the model and identify critical dimensions, datums and acceptance criteria for confirmation.

Process Minimum wall thickness (recommended) General tolerances (reference) Recommended fillet/radius Typical risk points
CNC machining Metal ≥ 0.8 mm; plastic ≥ 1.2 mm ±0.05 mm starting point; tighter tolerances require review Inside corner radius R ≥ 0.5 mm; use larger radii where possible Deep cavities, thin walls, sharp internal corners, deep threads and tight tolerances
Injection molding 0.8–3.0 mm; keep walls as uniform as possible Subject to mold and material Rounded transitions; draft ≥ 1° (≥ 2° for textured or deep surfaces) Abrupt wall changes, sink marks, warpage, insufficient draft and thick ribs
Sheet metal fabrication 0.5–6 mm is common; select by material and process Evaluate cutting and bending together Inside bend radius ≥ material thickness t as a starting point Insufficient hole spacing, bending interference, cracking, springback, assembly deviation
Vacuum casting 1.5–4 mm as a starting point Depends on master mold and material Use corner radii and gradual transitions Bubbles, trapped air, thin-wall deformation and poorly planned parting lines

CNC Machining Design Guidelines

Focus on tool access, wall stability, datums and functional tolerances. These choices reduce special tooling, extra setups, deformation and coordinate measuring machine (CMM) inspection cost.

1. Add Fillets to Internal Corners

  • CNC milling tools have a radius and cannot cut a perfectly sharp internal corner. Use R ≥ 0.5 mm as a starting point, and enlarge non-critical fillets wherever the design allows.
  • Larger rounded corners are recommended for deep cavities, deep grooves and pocket structures to facilitate chip evacuation and reduce the risk of vibration, tool marks and tool breakage.
  • If square corners must be retained, electrical discharge machining (EDM), wire cutting or a split assembly should be evaluated before quoting.
Cost Impact: Medium-High Risk: Unmachinable geometry / tool marks

2. Limit Deep Cavities and Grooves

  • Keep cavity depth within about 4× the tool diameter where practical; deeper features usually require long-reach tools and slower machining.
  • Add fillets, reliefs or openings at the bottom of deep cavities to improve tool access, chip evacuation and surface finish.
  • For non-critical areas, consider a split design, larger opening or multi-piece assembly to reduce machining difficulty.
Cost impact: high Risk: vibration/dimensional drift

3. Control Thin-Wall Deformation

  • As a starting point, use at least 0.8mm for metal walls and 1.2mm for plastic walls; confirm large or extensive thin-wall features separately.
  • Use ribs, curved geometry or temporary process supports to reduce machining and clamping distortion across large thin-wall areas.
  • Avoid aggressive cuts, deep grooves and direct clamping on thin walls where possible; each can increase chatter, warpage and dimensional drift.
Cost Impact: Medium-High Risk: Deformation/Scrap

4. Keep Holes and Threads Accessible

  • Keep blind-hole depth within about 3× the hole diameter where practical; deeper holes increase deflection and chip-removal risk.
  • Keep thread depth within about 3× the diameter where practical; deeper threads increase tapping and inspection risk.
  • Add chamfers, counterbores or lead-in surfaces to critical assembly holes to reduce scratching, cross-threading and rework.
Cost Impact: Medium Risk: Tool or tap breakage

5. Tighten Tolerances Only Where Needed

  • Applying tight tolerances to every dimension increases machining, process-control and CMM inspection cost without necessarily improving function.
  • Reserve tight tolerances for critical mating surfaces, locating holes, sealing surfaces and assembly datums; use general tolerances elsewhere.
  • Define datum references A, B and C, the critical dimension chain and the inspection method on the drawing to reduce quote assumptions and acceptance disputes.
Cost impact: high Risk: Longer lead time

6. Define Chamfers and Edge Requirements

  • Add chamfers to openings, edges and assembly leads (for example, C0.2–0.5) to improve fit-up and reduce scratching.
  • For cosmetic parts, define the A-side, grain direction, machining-mark limits and finish requirements.
  • For functional parts, define mating-surface quality, coaxiality for critical bores and shafts, and deburring requirements to prevent assembly interference.
Cost Impact: Low-Medium Risk: Assembly damage

Injection Molding Design Guidelines

Confirm wall thickness, draft, ribs, undercuts, parting, ejection, gate position and cosmetic surfaces before tooling. Early decisions reduce sink marks, warpage, mold changes and inconsistent acceptance.

1. Keep Wall Thickness Uniform

  • Avoid abrupt thickness changes; where practical, keep wall-thickness variation within 20% to reduce uneven shrinkage.
  • Core out thick areas or use ribs and assembled structures instead of solid blocks to reduce sink marks and cooling time.
  • Evaluate long, thin and large flat features for flow direction, cooling shrinkage and warpage risk.
Cost Impact: Medium Risk: Sink/Warp

2. Add Adequate Draft

  • Use at least 1° draft as a starting point; deep, textured or high-gloss surfaces commonly need at least 2°.
  • Insufficient draft can increase demolding resistance, scuffing, whitening, ejection deformation or mold wear.
  • Align texture with the pull direction where possible, and confirm texture depth and cosmetic-surface location before tooling.
Cost Impact: Medium Risk: Scuffing / poor release

3. Size Ribs to Avoid Sink Marks

  • Use rib thickness ≤ 60% of the main wall thickness as a starting point to balance stiffness and sink-mark risk.
  • Add radii at rib roots to reduce stress concentration, cracking and assembly failure.
  • Review rib height, spacing and gate location together with material flow to reduce short shots and trapped air.
Cost Impact: Low-Medium Risk: Sink marks / short shots

4. Plan Inserts and Threads Early

  • For higher assembly loads, consider heat-set, press-fit or molded-in metal inserts instead of threads cut directly into plastic.
  • Sufficient thickness, ribs and rounded transitions are required around the insert to prevent cracking when pressed in or pulling out during use.
  • Add lead-in chamfers and mistake-proofing features to critical bosses, and define assembly-torque limits.
Cost Impact: Medium Risk: Cracking / stripped threads

5. Define Cosmetic Surfaces and Defect Limits

  • Define the A-side, non-visible surfaces and acceptable defect areas for cosmetic parts.
  • Parting lines, ejector-pin marks and gate position affect flow marks, weld lines, splay and appearance consistency. Confirm their locations before tooling.
  • Transparent parts, high-gloss parts and spray-coated parts are more sensitive to materials, mold temperatures, gates and post-processing and need to be evaluated individually.
Cost Impact: Medium-High Risk: Cosmetic defects / rework

6. Reduce Undercuts and Side Actions

  • Undercuts, side holes, deep grooves and complex snap features can require sliders, lifters or side actions, increasing tooling cost and cycle time.
  • Reduce complex side actions by splitting the part, changing the assembly, redirecting the snap or revising local geometry.
  • When undercuts are necessary, limit their number and stroke and preserve maintenance access for stable production.
Cost impact: high Risk: Long cycle / high maintenance

Sheet Metal Design Guidelines

Review bend access, hole spacing, springback, welding, finishes and assembly datums together. For assemblies, identify the datum edge, locating hole and critical hole positions before quoting.

1. Choose a Practical Bend Radius

  • Use an inside bend radius of R ≥ t as a starting point, where t is material thickness; confirm material-specific limits.
  • Use a larger radius for stainless steel, high-strength steel and hard aluminum when needed to reduce cracking, marking and springback.
  • For cosmetic parts, define grain direction, bend-mark limits and finish requirements.
Cost Impact: Medium Risk: Cracking/Springback

2. Keep Holes Clear of Edges and Bend Lines

  • Keep the hole edge at least 1.5×t from the bend line; use 2×t where additional margin is practical.
  • Keep the hole edge at least t from the outer edge to reduce tearing during cutting, bending and assembly.
  • Where an assembly hole must sit close to a bend, consider a slot or machine the feature after bending.
Cost Impact: Low-Medium Risk: Hole deformation/assembly deviation

3. Size Holes and Cut Features for the Process

  • Use a laser-cut hole diameter ≥ t as a starting point; smaller holes increase burr, burn and dimensional-variation risk.
  • Use rounded transitions around sharp corners, narrow grooves and dense cut features to reduce stress concentration and heat effects.
  • Evaluate dense hole patterns, slots and mesh structures for warpage; temporary process edges or a forming operation may be required.
Cost Impact: Medium Risk: Burrs/Deformation

4. Check Bend Access and Flat Patterns

  • For parts with multiple bends, verify tool access and bend sequence to prevent the part from interfering with the press brake.
  • Provide a flat pattern or clearly identify bend direction, datum edges and the dimensioning scheme.
  • Define locating edges, locating holes and critical dimension chains for multi-bend assemblies to control stack-up error.
Cost Impact: Medium Risk: Interference/Rework

5. Plan Welding and Finishes Together

  • Powder coating, painting, electroplating and anodizing change assembly gaps; allow for coating thickness at critical joints.
  • Provide locating features, temporary process edges and post-weld straightening allowance where needed to control distortion and assembly variation.
  • For cosmetic parts, define weld quality, grinding limits, visible surfaces and finish-masking areas.
Cost Impact: Medium Risk: Coating interference/deformation

6. Use Datums and Practical Hole Tolerances

  • Dimension hole positions from a datum edge, datum hole or assembly datum to avoid cumulative error after multiple bends.
  • Use a locating hole with a slot where the assembly needs both accurate positioning and practical fit-up tolerance.
  • Tighten tolerances only for critical hole locations and use general tolerances elsewhere to reduce inspection and rework cost.
Cost Impact: Medium Risk: Assembly misalignment

Vacuum Casting Design Guidelines

Use vacuum casting for cosmetic or functional samples and low-volume builds. Review wall thickness, parting, venting, finish and acceptance criteria early to reduce bubbles, distortion, repairs and batch variation.

1. Use Stable Wall Thickness

  • Use 1.5–4 mm wall thickness as a starting point. Thin walls can deform; thick sections can trap air, shrink and cure unevenly.
  • Add ribs, curved geometry or local thickening to large thin-wall areas to improve part strength and batch consistency.
  • For long cantilevers, thin edges or large openings, review demolding strength, sagging and handling risk.
Cost Impact: Medium Risk: Deformation/Bubbling

2. Add Rounded Transitions

  • Avoid sharp corners, sharp edges and abrupt section changes. Use rounded transitions to reduce trapped air and stress concentration.
  • Very small internal radii, narrow deep grooves and closed corners increase bubble risk and repair cost.
  • For cosmetic parts, define the A-side, acceptable repair areas and finish requirements.
Cost Impact: Low-Medium Risk: Bubbles/Tearing

3. Plan Parting and Venting

  • Choose the parting surface carefully and keep the parting line away from primary cosmetic and mating surfaces where possible.
  • Deep cavities, closed regions and complex corners require vent paths to reduce trapped air, bubbles and incomplete fill.
  • For complex prototypes, consider splitting the design, changing the pour direction or revising the master pattern to improve appearance and dimensional consistency.
Cost Impact: Medium-High Risk: Low yield

4. Match the Mold Strategy to Quantity

  • A silicone mold may produce about 15–25 parts, depending on geometry, material, demolding difficulty and finish.
  • As quantity grows, compare the tooling economics and repeatability of injection molding, CNC machining or sheet metal fabrication.
  • Plan secondary drilling, machining or trimming for critical dimensions where it improves assembly consistency.
Cost Impact: Medium Risk: Batch-to-batch variation

5. Define Finish and Cosmetic Acceptance

  • For cosmetic parts, specify finish grade, gloss, color, texture, masking and acceptable color variation.
  • Vacuum metallizing, screen printing and spray finishing can reveal sharp edges, repair areas and surface defects, so confirm the finish standard before production.
  • Define the A-side so parting lines, repair areas and pour marks can be kept away from customer-visible surfaces.
Cost Impact: Medium Risk: Inconsistent appearance

6. Plan Fits and Secondary Machining

  • Allow practical clearance in vacuum-cast assembly holes, or use slots where additional fit-up tolerance is needed.
  • Consider secondary drilling, milling or inserts for critical mating surfaces and holes to improve small-batch consistency.
  • Allow for compression, rebound and long-term creep in soft or rubber-like materials to avoid over-tightening.
Cost Impact: Medium Risk: Inconsistent fit

Design Features That Increase Cost

Reserve complex geometry, tight tolerances and premium finishes for features that affect function or customer-visible quality. Simplifying non-critical features can reduce tooling, inspection, rework and lead time.

Recommended approach
Apply tight tolerances, premium finishes and special inspection only where function or customer-visible quality requires them. Define the A-side, functional surfaces, datums and acceptance criteria, and use standard requirements elsewhere.

Deep Cavities and Grooves

Deep cavities increase tool overhang, vibration, chip-removal difficulty and machining time.

Consider: splitting the part, enlarging the opening, adding fillets or using an assembly.

Small or Deep Holes and Threads

Small or deep features increase tool-breakage, chip-removal and inspection risk.

Consider: a larger diameter, lower aspect ratio, insert, through-hole or separate fastener.

Thin Walls and Large Flat Areas

Thin walls and large flat areas can deform during manufacturing, transport or assembly.

Consider: ribs, curved geometry, local thickening or a reinforced assembly.

Tight Tolerances on Non-Critical Dimensions

Unnecessary tight tolerances add machining, inspection and scrap risk.

Consider: tightening only critical fits, defining datums and using standard tolerances elsewhere.

Complex Undercuts and Side Actions

Undercuts can require sliders, lifters or side actions that increase tooling and maintenance cost.

Consider: a separate assembly, revised snap direction or fewer and shorter side actions.

High Cosmetic Standards and Multiple Finishes

Multiple polishing, painting, printing or plating steps increase cost, lead time and variation.

Consider: limiting premium finish to the A-side and defining defect limits before quoting.

Common DFM Mistakes and How to Avoid Them

Check these recurring issues before submitting a model. Each correction can reduce clarification, quote changes, sample rework and production delay.

1. Sharp Internal CNC Corners

Add machinable fillets, split the part, or confirm whether EDM or wire cutting is justified.

2. Tight Tolerances on Every Dimension

Tighten only critical fits and functional surfaces; use standard tolerances elsewhere and define the datum scheme.

3. Abrupt Injection-Molding Wall Changes

Core out thick areas or use ribs to keep walls uniform and reduce sink marks, warpage and mold rework.

4. Insufficient Draft

Start with at least 1° draft, or 2° for textured or deep surfaces, then confirm material, texture and pull direction.

5. Sheet-Metal Holes Too Close to Bends or Edges

Keep holes at least 1.5×t from bend lines and at least t from edges; use slots or post-bend machining where needed.

6. Sharp Vacuum-Casting Corners Without Venting

Add fillets and plan the parting surface, pour direction and vent path; split complex deep cavities where practical.

Define Inspection Requirements Before Quoting

Identify datums, critical dimensions, cosmetic surfaces, inspection records, material documentation and acceptance criteria in the drawing or project requirements. This makes quote assumptions and delivered results easier to verify.

If a 2D drawing is not ready
Upload the 3D model and describe critical fits, tolerances, assembly, A-side, material, finish and inspection requirements in the project notes. We will identify assumptions that need confirmation during the DFM review.

1. Define Datums and Critical Dimensions

  • Define datum planes, holes and edges for assemblies so that tight tolerances have an unambiguous reference.
  • Build critical mating dimensions into a closed dimension chain to control cumulative error and assembly uncertainty.
  • When coaxiality, position, flatness or CMM reports are required, define the inspection method and setup before quoting.
Benefit: Reduced rework Benefit: Faster confirmation

2. Define Cosmetic Surfaces and Acceptance Limits

  • Define the A-side, non-visible surfaces and acceptable defect areas for cosmetic parts.
  • State the allowable parting lines, ejector-pin marks, gate locations, repair areas and color variation.
  • For painting, coating, screen printing, brushing or polishing, define gloss, texture, masking and packaging protection before quoting.
Benefit: Improved cosmetic yield Benefit: Clear acceptance

DFM FAQs

Review common questions about geometry, tolerances, finishes, inspection and the information needed for an accurate quote.

Already Have Drawings? Request a Custom Parts Quote

Upload your CAD files and add material, quantity, tolerance, finish and delivery requirements. We will review manufacturability and recommend the next step.

Start Project Now