What DFM Actually Reviews Before the First Cut

A DFM report that arrives as a list of polite suggestions is not a DFM report. It is a quote with commentary.

The reason it matters is timing. Once the cavity block is cut, every geometry change costs steel, and sometimes costs a new insert. Before that, the same change costs an hour in CAD. DFM sits in that window, which is why a review that only confirms the part is "mouldable" wastes the one chance the project gets.

Here is what the review is actually looking at.

1. Wall thickness and the transitions between walls

Nominal wall is the first number anyone checks, and the least interesting. A 2.0 mm wall on its own is unremarkable. The problem is what happens where the wall meets a boss, a rib, or a step: mass accumulates, the section cools last, and the part sinks on the cosmetic face or pulls a void inside.

So the review maps thickness across the whole part rather than quoting one value. Two things come out of that map.

The first is thick regions that need coring out — a boss with a 4 mm wall next to a 2 mm panel is a sink mark waiting for the first sample.

The second is the ratio between thick and thin sections. Where a part runs from 3.5 mm to 1.2 mm, the thin end sets the injection pressure and the thick end sets the cycle. Both ends have to be acceptable at the same time, on the same machine.

Thin-wall work is its own discipline. On a 0.3 mm wall, flow length to thickness ratio decides whether the tool can be filled at all, and the gate and vent design carries more of the risk than the part geometry does.

2. Draft, shut-offs and what has to slide

Draft is where drawings and moulds disagree most often. A vertical face on the model is a face that will drag, and a textured face needs more draft than the drawing shows, because the texture depth sits on top of the nominal surface.

The review marks every surface that must release, then checks the angle against the finish specified for it. Where the angle is not there, there are three outcomes: change the part, polish the steel, or add a slide. All three are cheap now and expensive after hardening.

Undercuts are counted for the same reason. Every slider and every lifter is a joint that will wear, a witness line on the part, and a maintenance item for the life of the tool. A part with six sliders is not impossible — it is a tool that costs more, runs slower and needs more attention, and the customer should be told that while the geometry can still change.

3. Gate location decides everything downstream

Gate position fixes fill pattern, weld line location, packing, and where the cosmetic defect goes. It is the single most consequential decision in the review, and it is usually made in the first ten minutes.

What the review works through:

• Fill balance. Cavities that fill at different times cannot be packed equally, so parts from the same shot differ. On a 128-cavity tool the gate is a flow-balance problem before it is a cosmetic one.

• Flow length to thickness. Too long, and the part fills short or fills only at a pressure that overpacks the gate area.

• Weld lines. They are going to exist. The question is whether they land on a hidden face or across the Class A surface, and whether the material is one where a weld line is also a strength loss.

• Gate vestige and cosmetics. A gate on a visible face needs a finish and a trimming method agreed in advance, not discovered at sampling.

4. Cooling is a cycle-time decision

Cooling is designed at the same time as the part, not added around it afterwards.

Bore spacing and distance from the cavity surface set how fast heat leaves, and they also set how evenly it leaves. Uneven cooling warps a flat part regardless of how good the fill was. Where the geometry has a tall core or a deep pocket, the review has to decide whether conventional bores will reach it or whether a baffle, bubbler or conformal insert is justified, because that decision is what the cycle time and the price are built on.

On a thin-wall part running a four-second cycle, cooling is not a detail. It is the process.

5. Tolerances the process can hold

A drawing tolerance and a moulding tolerance are different things. Tool steel can be machined to 2 µm, and a mould can hold ±0.005 mm on the steel. Plastic is another matter: the same part in the same tool moves with moisture, with regrind percentage, with packing pressure, and with the direction of flow.

The review checks the tolerance stack against what the process can actually hold, dimension by dimension, and separates them:

• dimensions set by the tool, which are stable and can be held tight;

• dimensions set by the process, which drift and need a capability study before the tolerance is promised;

• dimensions set by shrinkage behaviour, which change between the first shot and the ten-thousandth.

Where a tolerance is tighter than the process supports, the honest answer at DFM stage is cheaper than the argument at PPAP.

6. Material and shrinkage direction

Shrinkage is not one number. Unfilled resin shrinks roughly equally in all directions. Glass-filled resin does not: it shrinks less along the flow and more across it, so a glass-filled part with a long flow path comes out anisotropic, and a flat part comes out warped in a predictable direction.

The review uses the actual grade, not a generic family value, and checks wall, gate and cooling against that. This is also where the material choice gets questioned if the part is asking for something the resin will not give.

7. The cosmetic spec, written down

"Good finish" is not a specification. The review should produce a written cosmetic standard: which surfaces are Class A, what texture and grain, what is acceptable at the gate, what weld line and flow mark are tolerated and where, and what the acceptance method is — visual under what light, at what distance.

Written down at DFM stage, this is a shared reference. Left verbal, it becomes a dispute at first article.

8. What a DFM report has to contain

A report worth reading has these, in this order:

1. Marked-up part model — wall map, draft check, undercut list, proposed gate location.

2. Fill, pack and warp analysis on the proposed gate, with the assumptions stated: material grade, melt and mould temperature, fill time.

3. Tool concept — cavity count, runner type, slides and lifters, ejection layout, expected cycle.

4. Risk list — each item with a severity, an owner, and a decision deadline. Not a paragraph of advice.

5. Tolerance review — which dimensions are tool-held, which are process-held, and which need a capability study.

6. Open questions — the ones that must be closed before steel is ordered.

We issue a DFM and feasibility report within two working days of receiving a 3D drawing. That is partly speed, and partly because a review that takes three weeks gets overtaken by the purchase order and stops being able to change anything.

9. The DFM that is really a quote

Three patterns are worth recognising.

The first is a report that only lists problems and never proposes a resolution — it transfers the risk back to the customer without giving them a decision.

The second is a report written to protect the toolmaker: every risk listed, nothing prioritised, so nothing gets fixed.

The third is a report with no numbers. No fill time, no pressure, no predicted cycle, no tolerance capability. If the analysis has no numbers, it did not run.

10. Before you approve

Four questions close a DFM review usefully:

• Which three features in this part are most likely to cause rework at T1, and what is the plan for each?

• Which tolerances on the drawing cannot be held by the process, and what do we do about them?

• Where will the weld lines and the gate land, and is that acceptable on the surfaces that matter?

• What cycle time and cavity count is the price based on?

The answers belong in writing, before the steel is ordered. After that, the same conversation happens with a deadline, a freight cost and a customer waiting.

FWD Precision — custom injection moulds and production moulding, Shenzhen, China.

• 260 people, including 38 design and programming engineers and 18 in QC

• 2 Makino V90S 5-axis machining centres, 13 high-speed CNC centres up to 42,000 rpm

• 45+ moulding machines, 30T to 550T

• 4 CMM systems, including a Zeiss MICURA 5/7/6

• Class 100,000 cleanroom

• We work to ISO 9001 and ISO 13485

• DFM and feasibility report in 2 working days

Send a 3D drawing (STP, X-T, IGES, DXF, DWG) to lilyfwd@fwdprecision.com

www.fwdprecision.com