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 ≥0.8mm; plastic ≥1.2mm ±0.05mm (normal); more stringent evaluation is required Internal angle R≥0.5mm (as large as possible) Deep cavities, thin walls, sharp angles, deep threads, tight tolerances
Injection molding 0.8–3.0mm (as uniform as possible) Subject to mold and material Rounded corner transition; draft angle ≥1° (texture/deep cavity ≥2°) Sudden changes in wall thickness, sink marks, warping, insufficient draft, and excessive rib thickness
Sheet metal fabrication Commonly used: 0.5–6mm (selected according to material) Cutting + bending requires comprehensive evaluation Inner bending radius ≥ plate thickness t (recommended) Insufficient hole spacing, bending interference, cracking, springback, assembly deviation
Vacuum casting 1.5–4mm (recommended) Depends on master mold and material Avoid sharp corners and add rounded corners and transitions Bubbles, trapped air, thin wall deformation, and unreasonable parting

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 the internal angle cannot be directly processed into an acute angle; it is recommended R ≥ 0.5mm, the key non-assembly angle should be enlarged as much as possible.
  • 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: Unable to process/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.
  • It is recommended to add fillets, undercuts or openings at the bottom of deep cavities to reduce root cleaning, poor chip removal and surface chatter marks.
  • For functionally insensitive areas, the difficulty of deep cavity processing can be reduced through split design, enlarged openings or multi-piece assembly.
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.
  • For large areas of thin wall, reinforcement ribs, arch structures or temporary process supports can be added to reduce processing deformation and clamping deformation.
  • Try to avoid strong cutting, deep grooves and clamping points in thin-walled areas to reduce vibration marks, warpage and dimensional instability.
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.
  • It is recommended to reserve chamfers, counterbore holes or lead-in surfaces for key assembly holes to reduce assembly scratches, poor meshing and on-site repairs.
Cost Impact: Medium Risk: Broken Knife/Broken Tap

5. Tighten Tolerances Only Where Needed

  • Tight tolerances across full dimensions will significantly increase CNC machining, process control and CMM inspection costs without necessarily improving product functionality.
  • It is recommended that tight tolerances be concentrated on key mating surfaces, locating holes, sealing surfaces and assembly datums, and conventional tolerances be used in the remaining areas.
  • The reference A/B/C, critical dimension chain and inspection method are clearly specified in the drawings, which can reduce quotation confirmation and production disputes.
Cost impact: high Risk: Longer lead time

6. Define Chamfers and Edge Requirements

  • It is recommended to chamfer openings, edges and assembly entry openings (e.g. C0.2–0.5) to improve assembly smoothness and reduce the risk of scratches.
  • For cosmetic parts, define the A-side, grain direction, machining-mark limits and finish requirements.
  • For functional parts, priority is given to ensuring the quality of mating surfaces, coaxiality of key hole shafts and deburring requirements to avoid assembly interference.
Cost Impact: Low-Medium Risk: assembly scratches

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.
  • In thick areas, it is preferable to use hollow, hollow, reinforced ribs or component structures instead of solid thick blocks to reduce sink marks and cooling time.
  • Long strips, sheets and large flat structures need to be evaluated 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: strain/yield loss

3. Size Ribs to Avoid Sink Marks

  • Recommended rib thickness ≤ 60% of main wall thickness, while ensuring strength while reducing backside shrinkage.
  • The tendon roots should be rounded to reduce stress concentration, cracking and assembly stress failure.
  • The rib height, rib spacing and gate location need to be combined with the material flow assessment to avoid insufficient filling or trapped air.
Cost Impact: Low-Medium Risk: Sink marks/insufficient filling

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.
  • Critical studs recommend the addition of guide chamfers, error-proofing structures, and assembly torque boundaries.
Cost Impact: Medium Risk: Cracked/slipped teeth

5. Define Cosmetic Surfaces and Defect Limits

  • Define the A-side, non-visible surfaces and acceptable defect areas for cosmetic parts.
  • The parting line, ejector pin mark, and gate position will affect flow marks, weld lines, silver wires, and appearance consistency. It is recommended to confirm the plan before opening the mold.
  • 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: Poor appearance/repair

6. Reduce Undercuts and Side Actions

  • Undercuts, side holes, deep grooves and complex buckles usually introduce sliders, inclined tops or side extraction mechanisms, which significantly increase mold costs and cycle times.
  • Priority is given to reducing complex core pulling through component division, assembly structure, buckle direction adjustment or local modification.
  • When undercuts must be retained, the quantity, core pulling stroke and maintenance accessibility should be controlled to avoid poor stability during the mass production stage.
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.
  • For stainless steel, high-strength steel and hard aluminum, it is recommended to increase R appropriately to reduce the risk of cracking, indentation 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.
  • The assembly holes close to the bend can be changed to oblong holes, process slots or post-bending processing solutions.
Cost Impact: Low-Medium Risk: Hole deformation/assembly deviation

3. Size Holes and Cut Features for the Process

  • Recommended minimum aperture for laser cutting ≥ t, too small holes will increase the risk of burrs, burnt edges and dimensional instability.
  • It is recommended to use rounded transitions for sharp corners, narrow grooves and dense cutting features to reduce stress concentration and thermal effects.
  • Large-area dense holes, slits or mesh structures need to be evaluated for warpage, and if necessary, additional process edges or shaping processes will be added.
Cost Impact: Medium Risk: Burrs/Deformation

4. Check Bend Access and Flat Patterns

  • For multi-bending structures, it is necessary to check the accessibility of bending tools and the bending sequence to avoid self-interference of parts.
  • Provide a flat pattern or clearly identify bend direction, datum edges and the dimensioning scheme.
  • Multi-bend assemblies need to clearly define positioning edges, positioning holes and critical dimension chains to reduce cumulative errors.
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.
  • It is recommended to reserve positioning points, process edges and post-weld shaping allowance in the welding area to reduce deformation and assembly deviation.
  • 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

  • It is recommended that the hole position be positioned based on the datum edge, datum hole or assembly datum to avoid cumulative errors after multiple bends.
  • Use a locating hole with a slot where the assembly needs both accurate positioning and practical fit-up tolerance.
  • Tolerances are tightened individually for key hole locations, while remaining hole locations remain regular, which can reduce inspection and rework costs.
Cost Impact: Medium Risk: Difficulty in assembly

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

  • Recommended wall thickness for vacuum casting 1.5–4mm; If it is too thin, it will easily deform; if it is too thick, it will easily trap air, shrink and solidify unevenly.
  • Large-area thin walls can add ribs, arch structures or local thickening to improve sample strength and batch-to-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 sudden cross-sectional changes. It is recommended to use rounded corner transitions to reduce trapped air and stress concentration.
  • Internal corners that are too small, deep grooves that are too narrow, and closed corners increase the probability of bubbles and repair costs.
  • 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

  • Reasonably select the parting surface and try to keep the parting line away from the main view surface, mating surface and key appearance surface.
  • Deep cavities, closed areas and complex corners require the design of exhaust paths to avoid trapped air, bubbles and material shortages.
  • For complex prototypes, the structure can be split, the pouring direction optimized, or the master mold scheme adjusted to improve appearance and dimensional consistency.
Cost Impact: Medium-High Risk: Decreased 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.
  • When the quantity increases, it is recommended to prepare molds or evaluate more suitable manufacturing paths such as injection molding, CNC machining, and sheet metal.
  • It is recommended to reserve secondary processing, drilling or trimming strategies for critical dimensions to improve 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 plating, silkscreen printing and spraying will amplify sharp edges, repair points and surface defects, so the process window needs to be confirmed in advance.
  • 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.
  • Secondary drilling, milling or insert solutions can be considered for key mating surfaces and hole locations to improve the consistency of small batches.
  • Soft rubber and rubber-like materials need to consider compression deformation, rebound and long-term creep to avoid over-tightening.
Cost Impact: Medium Risk: unstable assembly

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

  • It is recommended to define datum planes, datum holes and datum edges for assemblies to avoid tight tolerances without datums.
  • Key matching dimensions should form a closed-loop dimension chain to reduce cumulative errors and assembly uncertainty.
  • When coaxiality, position, flatness or CMM reports are required, the inspection methods and positioning standards should be clarified in advance.
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.
  • Clearly allowable parting lines, ejector pin marks, gate locations, repair areas and color difference standards.
  • When it comes to spraying, coating, silk-screening, brushing or polishing, gloss, texture, masking areas and packaging protection should be defined in advance.
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