Design for manufacture is not a document that proves a part can be molded. It is the list of decisions that are cheap today and expensive in three weeks. This is the ten-point list we walk through before a mold design is frozen.
Why the order matters
Every DFM point sits somewhere on a cost curve that rises steeply the moment steel is cut. A draft angle added at the design stage costs nothing but a modelling minute. The same draft angle added after the cavity is finished means removing material from a hardened block, re-polishing it, and re-running a trial — and on a textured surface it may not be recoverable at all.
So the review belongs before design freeze. Run afterwards, it is not a review; it is a report on which mistakes are now permanent.
The ten points
Work down this list in order. The first three decide whether the part can be molded at all; the rest decide whether it can be molded well and repeatably.
- Wall thickness and uniformity. Nominal wall for the resin, and no thick section next to a thin one. A thick-to-thin transition produces a sink on the thick side and a short shot on the thin side. Where a thick section is structurally necessary, core it out rather than accept it.
- Draft on every vertical face. One degree per side is a workable minimum on a smooth wall; 1.5 to 3 degrees on textured surfaces, because texture depth consumes draft. A zero-draft face drags, scuffs or cracks on ejection.
- Gate location and type. The gate sets weld-line position, flow length and the pressure needed. Put it where a cosmetic mark is acceptable and where the flow can reach the last cavity corner before the resin freezes.
- Shrinkage allowance. The cavity is not cut to the drawing; it is cut to the drawing corrected for the resin's shrink rate, which varies by grade, by flow direction and by wall thickness. This is a tool-side decision, but the part tolerances must leave room for it.
- Ribs and bosses. Rib thickness at roughly 50 to 60 % of the adjacent wall keeps the rib from becoming a sink source. Bosses need their own draft, a wall thickness near the nominal, and support from ribs rather than standing free.
- Undercuts and side actions. Every undercut needs a lifter, slider or split — each one adds tool cost, maintenance and a witness line. Ask whether the undercut is functionally required or a design habit.
- Ejection and witness marks. Decide now where ejector pins are allowed to land. On a visible cosmetic face, no pin position may land there at all; on a structural face it may be acceptable. Deciding after the trial means either a new tool or a visible mark on every part.
- Tolerance stack. Check that critical dimensions come from a single tool-side feature where possible. Dimensions that stack across a parting line inherit both halves' variation.
- Surface texture and standard. Name the standard and the grade: SPI, VDI or Mold-Tech, and the specific number. “Matte finish” is not a specification, and the difference between two adjacent SPI grades changes both draft and polishing hours.
- Material and its behaviour. Glass-filled resins wear gates and cavities; they also change shrink and weld-line strength. Flame-retardant grades can be more corrosive in the barrel. The material specification is a tool decision as much as a part decision.
The one question that catches most problems. For each critical feature, ask: “which single piece of steel creates this dimension?” If the answer is two pieces meeting at a parting line, expect variation and plan a tolerance for it.
The checklist as a table
| Point | What goes wrong | Working value |
|---|---|---|
| Wall thickness | Sink, short shot, warp | Uniform nominal for the resin, no thick-to-thin step |
| Draft | Scuffing, drag marks, cracking | 1° minimum smooth, 1.5–3° textured |
| Gate | Weld line in a visible place, short shot | Flow length reachable before freeze; mark in a hidden area |
| Shrinkage | Dimensions drifting out of tolerance | Cavity corrected by grade and flow direction |
| Ribs and bosses | Sink over the rib, boss cracking | Rib 50–60 % of adjacent wall |
| Undercuts | Unplanned slider, witness line, cost | Removed, or accepted with a named side action |
| Ejection | Pin marks on a cosmetic face | Pin positions agreed in writing before finishing |
| Tolerance stack | Critical dimension varies lot to lot | Single tool-side source per critical dimension |
| Texture | Wrong gloss, extra polishing hours | Named SPI or VDI grade, not “matte” |
| Material | Gate wear, unexpected shrink | Grade and filler stated, tool steel chosen to match |
What a late catch costs
The same defect has four different prices depending on when it is found. This is the argument for reviewing early, in one table.
| Caught at | Typical consequence | Schedule impact |
|---|---|---|
| Part design | Model edit | None |
| Mold design | Drawing change | 1–2 days |
| After roughing | Re-cut with stock available | 2–5 days |
| After finishing or hardening | Weld repair or insert remake | 5–15 days, plus a new trial |
| After production starts | Tool rework on a live line, parts sorted | Weeks, plus containment cost |
How to run the review
A DFM review that returns “looks fine” has not been done. Ask for the output in a form you can act on.
- Every one of the ten points listed, each marked resolved, accepted with a reason, or open.
- Open points assigned to a named person, with a date by which the answer is needed.
- Critical dimensions identified and agreed, rather than every dimension treated as critical.
- Texture standard named to a grade, with a physical sample approved before cavity finishing.
- Ejector pin zones and gate position agreed on a marked-up image, not in prose.
- The review document dated and versioned, so a later drawing revision can be compared against the review it invalidates.
It is also worth asking what the toolmaker would change if the part were theirs. That question tends to surface the one item that a formal list politely leaves out.
On this list. These are the checks we run and the values we work to in typical tooling. Specific resins, thin-wall applications and tight cosmetic programs will move some of them. The written DFM review issued with your quotation is the version that applies to your part.
What is DFM review in mold making?
Design for manufacture review is a written check of a part design against what the mold and the process can actually produce: wall thickness, draft, gate position, shrinkage allowance, rib and boss geometry, undercuts, ejection, tolerance stack, surface texture and material behaviour. It happens before the design is frozen, because every point it catches is cheap before steel is cut and expensive after.
How much draft angle does a molded part need?
One degree per side is a workable minimum for a smooth vertical wall, and 1.5 to 3 degrees is safer for textured surfaces because texture depth consumes draft. Deep ribs, fine grain and soft resins need more. A zero-draft wall will drag, scuff or crack on ejection, and the fix after the cavity is cut is to remove material from the tool, which changes the part.
When should DFM review happen?
Before design freeze, and ideally while the part design can still change. A DFM review run after the mold design is approved is a report, not a review: it can only tell you which decisions are now expensive to reverse.
Do you charge for a DFM review?
No. A written DFM review is part of quoting the tool, and you receive it whether or not you place the order. The only thing we ask is a model and a drawing complete enough to review.
Get the list in writing, against your model
Send the part and we will return each of the ten points marked resolved, accepted or open — with a date for the answers.
Request a DFM review