Your supplier has sent the DFM report and asked you to approve it so steel can be cut. The report is pages of screenshots, colour plots and recommendations — and your signature releases the tool budget.
A DFM report is ready to approve when every finding names the affected feature, states the risk in measurable terms, and gives you a decision: accept the risk, change the part, or change the tool. If a finding does none of those three things, it is a comment, not a review — and approval should wait until the gap is closed.
Design for Manufacturability (DFM) is the structured review of a plastic part’s geometry against the physical limits of injection molding, carried out before the mold is machined. A good report does not only list problems. It tells you which problems matter for your part, what each one costs if it is ignored, and who decides what happens next. This guide shows you how to read one as a buyer, question by question, with a 12-point checklist you can use on any supplier’s report.
What Should a DFM Report Contain?
Before you read a single finding, check that the report is built on the right inputs. A report that reviews the wrong CAD revision or the wrong resin is worse than no report, because it gives you false confidence.
A complete DFM report should identify the part and tool revision it reviews, the exact resin grade, the expected annual volume, the target machine range, and the surface-finish and tolerance requirements it was judged against. If any of those inputs changed after the report was written, ask for the affected sections to be re-checked. A resin change alone can move shrinkage, gate choice and cooling decisions.
The body of the report should then work feature by feature: wall sections, ribs, bosses, draft, radii, undercuts, gates, weld lines, parting line, ejection and tolerances. Each finding should carry a severity — what happens if it is left alone — and a recommendation with an owner. Findings without an owner are the ones that resurface as mold corrections after the first trial.
| Report section | What good looks like | Red flag |
|---|---|---|
| Inputs | CAD revision, resin grade, volume, finish and tolerances stated | "Per customer drawing" with no revision number |
| Findings | Each tied to a named feature with a severity | General advice with no feature attached |
| Recommendations | Accept, change the part, or change the tool — with an owner | "To be discussed" on every line |
| Simulation | Scope stated; results tied to gate, fill or cooling decisions | Colour plots with no conclusion |
| Open issues | Listed with a decision date | Missing entirely, implying there are none |
A DFM report is not a mold design, not a quotation and not a guarantee that the mold will produce good parts. It is a risk review. Its job is to make the risks visible while they are still cheap to fix — in CAD, not in steel.
How Do I Check the Wall Thickness, Rib and Boss Findings?
Wall thickness is usually the first thing a DFM report examines, and for good reason. Uneven walls cool at different speeds, which drives sink marks, warpage, internal stress and dimensional drift. The question to ask is not whether the walls are thick or thin in absolute terms, but whether they are consistent.
Look for the report to call out the nominal wall, the thickest and thinnest sections, and every transition between them. Thick sections that cannot be thinned — a mounting boss, a threaded insert area — should carry a plan: coring, a slower cooling allowance, or a steel-safe decision that lets the dimension be corrected after the first trial. Protolabs’ published wall thickness guidelines explain why uniform walls matter and how a DFM analysis flags thin and thick areas relative to the nominal wall; use them as a cross-check on whether your supplier’s numbers are in a normal range for the resin family.
Ribs and bosses deserve the same treatment. A common published guideline is to keep rib thickness at roughly 40–60% of the adjacent wall, so the rib stiffens the part without leaving a sink mark on the opposite surface. If your report recommends ribs thicker than that on a cosmetic face, ask what evidence supports it. Bosses around screws or inserts need the same question: how is the sink risk handled, and where will the witness mark fall?
| Feature | What to look for | Why it matters |
|---|---|---|
| Nominal wall | One stated value, consistent across the part | Sets fill, cooling and shrinkage behaviour |
| Thick-to-thin transitions | Each one named, with a sink or warp consequence | Transitions drive most visible defects |
| Ribs | Thickness relative to the wall, height, draft | Thick ribs sink; tall ribs warp |
| Bosses | Wall around the boss, gusset or coring plan | Uncored bosses sink and crack |
| Thin sections | Fill risk at the stated gate and pressure | Thin areas short-shot first |
If the report says only "wall thickness is acceptable," that is not a finding. Ask which sections were measured and against what nominal value.
What Should the Report Say About Draft, Radii and Ejection?
Draft is the slight taper on vertical walls that lets the part leave the mold without dragging or tearing. Without it, the plastic shrinks onto the core and the ejector system has to force it off, which scars surfaces and can break clips or thin walls.
A useful rule of thumb, published in Protolabs’ design essentials for injection moulding, is about 1 degree of draft per inch of cavity depth — and more where the surface is textured, because texture grips the steel. Check that your report states the draft on each tall wall and on textured faces separately. A single draft value for the whole part usually means nobody checked the deep features.
Inside corners need radii. Sharp internal corners concentrate stress, restrict flow and make ejection harder; the report should show radii on load-bearing corners and explain where a sharp corner was kept for a functional reason. Ejection is the third part of this check: the report should show where ejector pins land, whether they fall on cosmetic surfaces, and whether the parting line sits where you expect it. Ejector witness marks on a visible face are a cosmetic decision, not a surprise to discover on the first sample.
Ask three questions here: is the draft stated per feature, not per part? Are textured faces given extra draft? And does the ejection layout keep witness marks off the surfaces your customer sees?
How Do I Judge the Gate, Weld-Line and Flow Conclusions?
The gate is where molten resin enters the cavity, and its position shapes almost everything downstream: fill direction, weld lines, sink, shear stress and the visible gate vestige. A good report explains the gate choice in one paragraph per gate — type, location, and what was traded away.
Gates should generally sit at or near the thickest wall section, so resin flows from thick to thin and packs the part before the flow front reaches thin areas. If the report moves a gate to a thin section for cosmetic reasons, it should say what fill or packing risk that creates. Weld lines — where two flow fronts meet — are weaker than the surrounding material, so the report should show where they fall and confirm they sit away from structural or cosmetic surfaces. A weld line across a snap fit or a visible face is a decision you should make deliberately, not discover at trial.
Where the supplier ran a Moldflow or flow simulation, read the conclusion, not the colours. The simulation should answer a specific question: will this gate fill the part, where will the weld lines sit, and is the cooling balanced enough to hold the critical dimensions? Simulation supports gate, flow, pressure, weld and cooling decisions, but it does not replace the physical trial — the mold and the material still have to be proven with real parts. If the report leans on simulation to close a tolerance question, ask what trial evidence will confirm it.
What About Tolerances, Shrinkage and Steel-Safe Decisions?
Tolerances are where DFM reports most often go vague, and where vagueness costs the most. The report should name the critical dimensions, the datum scheme they are measured from, and the measurement method that suits each feature and tolerance. A tight tolerance on a dimension that shrinks unevenly is not a drawing note — it is a trial-and-correction plan, and the report should say so.
Shrinkage deserves a number, not a word. The resin’s published shrinkage range comes from the material data sheet for a stated grade and test condition, and the mold dimensions are derived from it — the working relationship is Mold Dimension = Part Dimension / (1 − Shrinkage Rate). Our shrinkage compensation guide explains how exact-grade data, geometry and flow review, steel-safe assumptions and measured trial results combine into a defensible plan, and why the quotation should state which testing or simulation is included. If your report quotes a shrinkage value without naming the grade and the data-sheet condition it came from, treat the dimensions built on it as unconfirmed.
Steel-safe design is the honest middle ground when a dimension cannot be confirmed before tooling. For selected dimensions, the mold is built with a controlled allowance of extra steel, so the dimension can be corrected precisely after the first trial instead of welded and re-cut. The report should name which dimensions are steel-safe, how much allowance was left, and which trial will confirm the final cut. Steel-safe is a plan, not a postponement — without a named trial and a decision owner, it is just an open issue.
The 12-Point DFM Review Checklist
Use this table on any supplier’s report. A "no" on any row is not automatically a reason to reject the report — it is a question to close before you approve.
| # | Check | What to verify | Pass looks like |
|---|---|---|---|
| 1 | Input identity | CAD revision, resin grade, volume, finish | All four stated and current |
| 2 | Wall thickness | Nominal wall, thickest and thinnest sections | Every transition named with a consequence |
| 3 | Ribs and bosses | Thickness relative to the wall, coring plan | Ribs near 40–60% of wall; bosses cored or justified |
| 4 | Draft | Per feature, including textured faces | Stated values; extra draft where texture grips |
| 5 | Radii | Inside corners on load-bearing features | Radii shown; sharp corners justified |
| 6 | Undercuts | Slides, lifters or design change for each one | Every undercut has a mechanism or a redesign |
| 7 | Gate type and location | Gate at thick section; vestige position | One paragraph per gate with its trade-off |
| 8 | Weld lines | Position relative to structural and cosmetic zones | Away from snaps and visible faces, or accepted in writing |
| 9 | Parting line and ejection | Pin positions, witness marks, flash risk | Marks off cosmetic faces; line where expected |
| 10 | Tolerances and datum | Critical dimensions, datum scheme, measurement method | Each critical feature has a method that fits its tolerance |
| 11 | Shrinkage and steel-safe | Grade-specific data; steel-safe dimensions named | Formula inputs traceable; allowance and trial named |
| 12 | Open issues | Every unresolved item with an owner and a date | Nothing left as "to be discussed" without a date |
Work through the list with the report open, and write your questions back to the supplier in the same numbered form. A supplier who answers in the same structure is showing you their working; a supplier who answers in generalities is telling you the review was general too.
What Should I Do When the Report Raises a Problem?
Every real DFM report raises problems. That is its purpose. What matters is what happens next, and there are only three honest responses: accept the risk in writing, change the part, or change the tool.
Changing the part means a controlled CAD revision — the geometry moves, the revision number moves with it, and the DFM findings that depended on the old geometry are re-checked. Changing the tool means the mold design absorbs the problem: a different gate, a slide instead of a redesign, a steel-safe allowance. Accepting the risk means writing down what was accepted, by whom, and what the fallback is if the trial proves the concern right. Verbal acceptance disappears; a one-line email does not.
Do not approve a report that lists problems and proposes no response for them. And do not let schedule pressure turn approval into a formality — the cost of a DFM change is a CAD revision; the cost of the same change after steel is cut is a mold correction, a re-trial and a moved delivery date. Our mold testing and validation process shows how T0, T1 and later trials are planned as decision stages, so the corrections your DFM review identifies have a trial waiting to prove them.
What to Send With Your DFM Review
If you are asking a supplier to review your part — or to review a DFM report another supplier produced — send the package that lets them answer in specifics: the STEP file and 2D drawing at a stated revision, the resin grade or the performance requirement it must meet, the expected annual quantity, the key tolerances with their datum scheme, the surface finish, the delivery region and your timing. A request for quotation with that package attached gets a review of your part, not a review of a generic shape.
A careful DFM review is the cheapest quality step in the whole project. It happens before steel is cut, before the trial is scheduled and before the delivery date is at risk. Read it like a decision document, not a formality — because once you sign it, it becomes one.
FAQ
Does approving a DFM report mean the mold will produce good parts?
No. DFM approval means the known geometry and process risks have been reviewed and decided. The mold still has to be proven by trial: T0 checks that the tool operates safely, T1 produces corrected samples for dimensional, appearance, assembly and functional review, and only the evidence from those trials closes the remaining questions.
Who owns a change the DFM review finds — the buyer or the supplier?
It depends on what changes. Part geometry changes belong to the buyer’s CAD revision and need the buyer’s approval. Tooling changes belong to the mold design and need the supplier to record them. What matters is that the report names an owner for each change; an unowned change is an unresolved one.
Should every project include a Moldflow analysis?
Not necessarily. A flow simulation is justified when fill balance, weld-line placement, cooling or warpage is genuinely uncertain — a complex geometry, a long flow path, a tight tolerance on a warpage-sensitive feature. For a simple part with a proven gate and resin, a simulation adds cost without changing the decision. Ask the supplier to state what question the simulation answers before you pay for it.