DFM Review Checklist for Injection Molded Parts

A DFM review is not a formality that delays the tool order. It is the last point at which a change costs hours instead of weeks, and the first point at which someone outside the design team looks at the part with the tool in mind.

Twelve-area DFM review checklist and review session workflow

Figure 1. Twelve-area DFM review checklist and review session workflow.

This checklist is organized the way a review actually runs: geometry first, then tooling, then process, then the commercial and quality questions. Use it as the agenda, not as a rubber stamp — a review where every box is ticked and nothing is questioned is a review that did not happen.

1. Wall thickness

[ ] Nominal wall thickness defined and stated on the drawing
[ ] Wall thickness consistent across the part
[ ] Maximum-to-minimum wall ratio within 2.5:1
[ ] Thick-to-thin transitions made gradually, over at least 3 × the difference
[ ] No isolated thick sections that will sink or void
[ ] Wall thickness appropriate to the resin (thin walls need high-flow grades)
[ ] Flow length to thickness ratio calculated for the worst-case flow path

Ask: which wall is the thickest, and what does it do? Thick sections are usually there to carry load or to accommodate a feature, and both have better answers than more material.

2. Draft angle

[ ] Draft specified on every vertical face, including inside faces and holes
[ ] Draft in the direction of pull, not against it
[ ] Extra draft on textured surfaces (1° minimum, plus 1° per 0.025 mm of texture depth)
[ ] Deep features, ribs and bosses drafted generously
[ ] Undercuts identified and either eliminated or assigned to a slide, lifter or stripping action

Ask: what is the texture, and does the draft account for it? Texture is the single most common cause of a part that will not release.

3. Radii and corners

[ ] External corners radiused
[ ] Internal corners radiused at ≥ 0.5 × wall thickness where possible
[ ] No sharp internal corners at any stress location
[ ] Fillet radius consistent with a standard cutter size the tool shop already owns
[ ] Weld line locations evaluated against the stress pattern

Ask: does the radius at the corner match the wall thickness, or just look nice? A small fillet at a thick corner concentrates stress exactly where the part will fail.

4. Ribs

[ ] Rib thickness 50–60% of the adjacent wall
[ ] Rib height within 3 × wall thickness unless flow analysis supports more
[ ] Rib spacing ≥ 2 × wall thickness
[ ] Ribs drafted on both sides
[ ] Root fillets specified
[ ] Ribs staggered so they do not create a thick mass at the intersection
[ ] Rib direction aligned with the principal bending load
[ ] Sink on the opposite face checked at the rib locations

Ask: are the ribs carrying load, or just filling space? Ribs added without a load path simply add weight and sink marks.

5. Bosses

[ ] Boss wall thickness ≤ 60% of the nominal wall (or ≤ 0.6 × the mating wall)
[ ] Boss outside diameter appropriate to the fastener
[ ] Boss connected to a wall or a rib rather than standing free
[ ] Gussets added where the boss is tall or loaded
[ ] Bosses drafted
[ ] Core pins sized so the boss core can be cooled
[ ] Boss base filleted into the wall
[ ] Boss height within practical core-pin limits

Ask: which boss is the tallest and thinnest? That is the one that will snap in transport.

6. Holes, slots and threads

[ ] Holes molded where practical (molded holes cost less than drilled holes)
[ ] Core-pin length to diameter ratio within limits (typically ≤ 4:1 for a robust pin)
[ ] Blind holes specified with a depth that suits the core pin
[ ] Hole axis parallel to the mold opening direction
[ ] Threads specified as molded, inserted or self-tapping and consistent with the joint load
[ ] Thread relief and lead-in provided
[ ] Side holes assigned to a slide or a secondary operation, with the cost understood

Ask: which feature needs the most fragile core, and does the design need it at all?

7. Gating and flow

[ ] Gate type and location proposed
[ ] Gate location approved by the customer if it leaves a visible mark
[ ] Gate positioned so the melt fills thick sections first
[ ] Gate positioned so weld lines fall in low-stress areas
[ ] Gate size appropriate to the wall and the resin
[ ] Runner system balanced for multi-cavity tools
[ ] Cold runner versus hot runner decided, with a reason
[ ] Degating method defined, and its cost estimated
[ ] Flow analysis run for parts with long flow, tight tolerance or critical appearance

Ask: where does the flow end, and what is there? The last-filled point is where burns, short shots and weak welds live.

8. Cooling

[ ] Cooling circuits laid out with adequate coverage
[ ] Core cooling provided, not just cavity cooling
[ ] Cooling distance from the surface consistent (typically 1.5–2.5 × the wall thickness)
[ ] Baffles, bubblers or thermal pins specified for deep cores
[ ] Cooling around thick sections given extra attention
[ ] Circuit design matched to the warpage requirement
[ ] Water fittings positioned so they do not clash with the machine or robot

Ask: which section of the part will be hottest at ejection? That is where the cycle time and the warp come from.

9. Ejection

[ ] Ejector pin locations proposed
[ ] Ejector pins land on rigid features, not on cosmetic surfaces
[ ] Adequate ejection area for the part stiffness
[ ] Ejector pins not interfering with cooling channels
[ ] Stripper plate or air ejection considered for thin-wall or deep-draw parts
[ ] Positive return and safety switches specified
[ ] Part will not stick in the cavity by vacuum or by undercut

Ask: what is the ejection strategy, and does the part have enough stiffness to survive it?

10. Tolerances and dimensions

[ ] Tolerances assigned only to functionally important dimensions
[ ] General tolerance note stated on the drawing
[ ] Tolerances achievable by molding, with machined or inserted features used only where needed
[ ] Datum scheme defined for the checking fixture
[ ] Warpage and flatness requirements realistic for the geometry
[ ] Critical-to-quality dimensions identified and flagged for control
[ ] Mating parts reviewed against the tolerance stack

Ask: which dimension, if it drifts, stops the assembly line? That one earns a tight tolerance; the others do not.

11. Material and process

[ ] Resin grade specified with supplier and grade code
[ ] Resin suitable for the wall thickness, flow length and environment
[ ] Drying requirements documented
[ ] Masterbatch carrier compatible with the base resin
[ ] Regrind percentage allowed stated
[ ] Shrinkage data available for the specific grade
[ ] Additives, flame retardants or UV packages declared
[ ] Cycle time and machine tonnage estimated

12. Quality, cost and program

[ ] Appearance requirements defined (which surface is class A, which is hidden)
[ ] Surface texture specified on the drawing, with the mold finish standard referenced
[ ] Inspection plan and sampling frequency agreed
[ ] Critical dimension list agreed with the supplier
[ ] Quotation assumptions documented: cavitation, cycle time, tonnage, scrap rate
[ ] Tooling ownership, maintenance responsibility and cycle-count expectation stated
[ ] Change control process agreed for post-tool-release changes
[ ] Timeline agreed with realistic time for tool trials and correction loops

Running the review

A DFM review works best as a live session with the part on screen, the tool designer present, and someone empowered to say no. Practical habits that make it effective:

Review the drawing before the 3D model, then check the model against the drawing. Discrepancies are common and expensive.
Walk the part in the direction of pull, feature by feature. Most moldability problems appear during this walk.
Log every issue with an owner and a date, not just a note. Unassigned findings are decoration.
Separate must-fix from nice-to-have. A DFM report that lists fifty equal-severity items gets ignored.
Re-review after changes. A geometry change made late can invalidate the whole review.

The point of the checklist is not to produce a document. It is to move the discoveries that would otherwise appear at tryout — where they cost weeks — to the desk, where they cost an afternoon.

Quick reference - key checks and values for DFM Review Checklist for Injection Molded Parts

Figure 2. Quick reference: the key checks and reference values from this guide.