A DFM report normally arrives at the end of the design, lists thirty recommendations, and is read after the model is frozen and the tool is quoted. By then four of those thirty mattered, and all four have already cost what they were going to cost. The useful version of this work happens earlier, inside a much narrower window, and it asks a shorter question — not "what could be improved" but "what will this drawing force the tool to do".
DFM only pays inside a narrow window
Design for manufacturability is not a quality activity. It is a timing activity. The same change — moving a boss two millimetres, adding a draft angle, thinning a wall — costs radically different amounts depending on when it is made. The difference is not ten percent. It is an order of magnitude, and then another one.
| When the change is made | What it actually costs | How it usually goes |
|---|---|---|
| Concept sketch | A different sketch | Five minutes and an eraser |
| 3D model, before release | Hours of CAD, no schedule impact | The cheapest good outcome available |
| Quotation issued, tool designed | One to three days of redesign and a re-quote | Still cheap, still easy |
| Steel ordered, not yet cut | One to two weeks; the block is re-sourced or scrapped | The first real money |
| Steel cut, before first trial | Two to four weeks; welded inserts, lost polish, a weaker tool | Five to ten times the same change made earlier |
| After the first trial | Three to six weeks; often a new insert block | Ten to twenty times |
| In production | Six weeks or more, plus a mold stop, plus every part already made | No longer a design decision — it is a recovery plan |
Read the last three rows again. Between the first row and the fifth, the same correction goes from a five-minute edit to a five-week recovery, and the part is no better at the end of it. This is the entire economic case for looking at manufacturability early: not that the advice is different, but that the advice is still cheap.
The practical consequence is that a DFM review which happens after the tool drawing is approved is not a review. It is a negotiation about which of the remaining problems you are willing to live with. That is still worth doing, but it is a different conversation, and it usually ends with a note on a drawing that nobody reads again.
What a useful review actually produces. Not thirty recommendations. A short list of decisions, each one attached to a number: this rib will sink because it is 0.8 of the wall instead of 0.5; this wall cannot fill at 0.9 mm in this resin; this undercut adds a slider and three weeks. A recommendation without a number is an opinion, and opinions lose to deadlines every time.
Wall thickness: uniformity beats the number
Ask ten molders for a minimum wall and you will get ten answers, all defensible, because the real limit is not a number on a chart. It is the ratio between flow length and wall thickness in the specific geometry, in the specific resin, at the pressure the machine can deliver.
What is not negotiable is uniformity. A part with a 1.5 mm wall everywhere is easy. A part that runs 1.5 mm, then 3.5 mm, then 1.5 mm is difficult no matter how good the resin is, because the thin sections freeze while the thick section is still liquid and packing. The thick section then shrinks against nothing, and you get a sink mark on the cosmetic face or a void inside the boss.
The working rules are unglamorous and they hold:
- Keep the variation under about 25% of the nominal wall across the whole part. Beyond that the flow front stops advancing evenly and the thick section starts to dictate the cycle.
- Transition over a length of at least three times the thickness difference. A step is a stress riser, a flow restriction and a cooling imbalance at the same point.
- If you need stiffness, remove material rather than add it. A 3 mm wall replaced by a 2 mm wall plus ribs is lighter, stiffer, faster to mold and cheaper per part. This is the single most reliable improvement available in plastic part design.
| Resin | Workable wall | What goes wrong thin | What goes wrong thick |
|---|---|---|---|
| ABS | 1.5–3.0 mm | Below 1.2 mm the flow front freezes before the cavity fills, and every gate has to move | Above 4 mm: sink over ribs, internal voids, and a cycle that never comes down |
| PP homopolymer | 1.0–3.0 mm | Forgiving — high-flow grades will fill 0.8 mm over a short distance | Warpage is the first symptom, sink the second; PP hides voids well and shows sink badly |
| HDPE | 1.0–3.5 mm | Living hinges are cut to 0.25–0.4 mm on purpose — that is a feature, not a thin wall | Heavy sink; the surface reads every internal rib |
| PC | 1.5–3.5 mm | Below 1.0 mm needs a hot tool and very high pressure; residual stress shows as crazing later | Long cooling, and blush around the gate |
| PC/ABS | 1.5–3.0 mm | Tolerates thin sections better than PC but not much better | Same as PC, with a wider process window |
| PA6, PA66 (unfilled) | 0.8–3.0 mm | Fills thin sections well; the problem is moisture, not thickness | Voids and post-molding growth that continues for weeks |
| PA6 / PA66 + 30% glass | 1.0–3.0 mm | Glass fibres bridge and block thin gates; expect short shots at 0.8 mm | Anisotropic shrinkage and severe warpage |
| POM | 1.0–3.0 mm | Sharp corners plus thin walls equal stress cracking in service | Long, slow cycles; post-molding shrinkage for days |
| PBT | 0.8–3.0 mm | Fast crystallising, so thin sections need speed, not pressure | Warpage, especially on glass-filled grades |
| GPPS | 1.0–3.5 mm | Brittle: thin ribs snap on ejection | Sink and internal stress whitening |
| PMMA | 1.5–3.5 mm | Flow marks are permanent on a transparent part | Optical distortion from uneven cooling, not from thickness |
| Rigid PVC | 1.5–3.5 mm | Burns at slow fill; thin sections force high shear and degrade the resin | Corrosion of the steel is the real limit, not the wall |
| TPU / TPE | 1.0–3.0 mm | Very thin sections tear on demolding — soft resins grip the core | Long cooling; soft parts deform on ejection |
The cooling term deserves its own sentence, because it is the one people underestimate. Cooling time scales with the square of wall thickness. Going from 2 mm to 3 mm does not add 50% to the cooling time — it adds about 125%, and the cooling share is usually the largest single block of the cycle. A wall that was made thicker "for strength" is usually the reason a part costs more than the quotation assumed.
Every corner is a stress riser
A sharp inner corner does two things at once, and both of them are bad. In the part, it multiplies the stress that arrives there. In the mold, it creates a corner that cannot be machined cleanly, cannot be polished, and concentrates heat treatment stress in the steel — which is where cavity inserts crack.
The radius that matters is the inner one. The outer radius matters for a different reason: if the outer radius does not equal the inner radius plus the wall thickness, the wall is thinner at the corner than it is on the flat, and the corner becomes the weak point even after you have radiused it. Getting this right is a two-second CAD operation and a permanent improvement.
| Inner radius ÷ wall | Stress concentration factor | What it means in practice |
|---|---|---|
| Sharp corner (R ≈ 0) | 3.0 or worse | The part fails here first, and the mold erodes here first — two failures at one corner |
| 0.1 | ≈ 2.0 | Half the nominal strength is gone before any load arrives |
| 0.25 | ≈ 1.5 | Acceptable only on non-structural corners |
| 0.5 | ≈ 1.3 | The normal target for a general part |
| 1.0 | ≈ 1.15 | The normal target for anything that carries load or takes an impact |
| 2.0 and above | ≈ 1.05 | Effectively no concentration left; further radius buys nothing structural |
A useful default: inner radius at half the wall for a general part, and equal to the wall for anything that carries load, takes an impact, or acts as a snap-fit root. Above twice the wall the curve is flat — more radius buys nothing structural, though it may still help flow.
This is the one item on the list that costs nothing and gives something back. Radii reduce EDM time, reduce polishing time, reduce the chance of a cracked insert, and make the part stronger. There is no trade-off to weigh. If a drawing arrives with sharp internal corners, that is the first thing to change and the easiest argument to win.
Draft is not optional, and texture changes it
Draft is the one feature that has no structural argument attached to it and is therefore the one most often left off. A vertical wall at zero draft will mold — once. Then the surface starts to scuff, the ejection force climbs, the part comes out with white stress marks at the corners, and by the time anyone connects the problem to the missing half-degree, the tool needs to be re-cut in a place where re-cutting is difficult.
The number depends on the surface, not on the resin. Polished steel releases easily. Every tool mark, every EDM recast layer and every etched texture is a drag point. That is why texture is not a cosmetic decision alone: a grain etched 0.025 mm deep adds roughly one degree of draft per 0.025 mm of depth, on top of whatever the base surface needed.
| Surface | Minimum draft | Draft we would design to | Note |
|---|---|---|---|
| Polished cavity wall, along the draw | 0.5° | 1.0° | Polished steel releases easily, so the minimum is genuinely usable |
| Machined or EDM wall, Ra 1.6 µm and coarser | 1.0° | 1.5–2.0° | Every tool mark is a drag point; this is where most scuffing starts |
| Fine texture, 0.5–1.0 mil deep | 1.5° plus 1° per 0.001 in | 2.0–2.5° | Texture is etched into the steel and grips the part on the way out |
| Coarse texture, leather or heavy grain | 3° | 3.0–5.0° | Quoted at 1.5° and etched anyway is the classic unbuildable part |
| Core side, any surface | 1.0° | 1.5–2.5° | The part shrinks onto the core and holds it — the core always needs more than the cavity |
| Deep cavity, depth over 3× the opening | 1.5° | Add 0.5° per further 1 mm of depth | Long draw, long contact, high release force |
| Small deep holes, core pins under 6 mm | 1.5° | 2.0–3.0° | Thin pins deflect, so the effective draft is less than the number on the drawing |
| Ribs and bosses | 0.5° per side | 1.0° per side | Ribs are deep and thin: they are the first feature to scuff |
Two rules that are worth stating separately, because they are the ones that get missed:
- The core side needs more draft than the cavity side. The part shrinks onto the core as it cools and grips it. The cavity lets go; the core holds on. A tool designed with equal draft on both halves will drag on the core every cycle.
- Ribs and bosses need draft per side, not total. A 1° per side on a rib that is 1.2 mm thick at the top means it is 2.4 mm wider at the base — which may put it over the thickness that sinks the opposite face. Ribs are where draft and wall thickness collide, and where the compromise has to be made deliberately.
If the part genuinely cannot take draft — a straight-sided cosmetic wall, a bore that has to be parallel — then say so on the drawing and expect the tool to be built with a strip-and-replace polish schedule. That is a real option. It is just not the option you get by leaving the draft off and saying nothing.
Ribs and bosses: where sink marks are born
Ribs are the answer to the previous section — they let you delete wall thickness — and they are also the most common source of the defect that sends a part back. The mechanism is simple: a rib is a local thickening. If the rib is as thick as the wall it sits on, the junction is twice the wall, and the junction cools last and shrinks away from the cosmetic face on the other side.
The numbers that keep this under control:
- Rib thickness at 50–60% of the main wall. For PC and PC/ABS go lower, 40–50%, because those resins sink readily. For PP and PE, 60–70% is workable because they sink less.
- Rib height up to about three times its own thickness. Beyond that the rib needs its own draft and often a gusset, and it becomes hard to fill at the base.
- Rib spacing at least twice the wall thickness between ribs, or the gaps between them stop cooling properly and the whole panel warps.
- Root fillet at 0.25 to 0.5 times the wall. A square root is a stress riser exactly where the bending moment is highest.
Bosses — the screw pillars — fail the same way for the same reason. A boss with walls as thick as the panel sinks a ring into the face above it, every shot, no matter what the process does. The fix is threefold: boss wall at about 60% of the main wall, a fillet or a pair of ribs tying the boss to the nearest side wall so it is not a free-standing cylinder, and a bore depth no more than about three times the bore diameter so the core pin does not deflect.
For a self-tapping screw the geometry follows the screw: an M3 screw wants a pilot bore around 2.5–2.8 mm and an outside diameter around 6.0–6.5 mm, which puts the boss wall near 1.8 mm. If the panel is 2.5 mm, that boss is at 0.7 of the wall and it will show. Either thin the boss and accept lower strip torque, or thicken the panel locally and accept a slower cycle. There is no third answer, and finding this out at the trial is expensive.
Send us the model before the tool drawing exists
That is the point where a wall, a rib thickness or a missing draft still costs an hour instead of a month. We will mark the features that will not fill, the ribs that will sink the face opposite, and the undercut that needs a slider — and tell you which of them matter.
Count the undercuts before you design them
Every undercut is a mechanism. Every mechanism is a part of the mold that moves, wears, needs clearance and eventually jams. This does not mean undercuts should be avoided — plenty of parts need them — but it does mean they should be counted, deliberately, before the design is frozen, rather than discovered by the toolmaker.
| Method | Where it works | What it costs you |
|---|---|---|
| Slider (cam action) | Outside undercuts, any depth; the default for a housing with a side opening | A second motion in the tool, wear plates, a lock block, and a maintenance item that returns every few hundred thousand shots |
| Lifter | Inside undercuts with short travel, typically under 10–15 mm | Occupies space on the core, needs clearance, and leaves a witness mark on the adjacent wall |
| Angled pin | Small inside undercuts, a thread relief, a snap groove | Cheap to build, wears quickly; fine for a short run, not for a long one |
| Bump-off / strip | Flexible resins — PP, PE, TPU — with an undercut under roughly 5% of the wall or 0.5 mm | No mechanism at all, so the cheapest option; the cost is stress whitening and a tool that wears at the bump |
| Collapsible core | Internal threads and ring grooves, molded in place | The most expensive mechanism in common use, and the one that needs the most maintenance |
| Redesign the undercut away | Whenever the function allows it | Usually nothing — and it removes a failure mode permanently |
Two habits make a real difference here. The first is aligning undercuts to one direction: three separate undercuts that all pull the same way can be served by one slider, and one slider costs far less than three — not three times less, but close to it, because the second and third motions share the base, the wedge and the setup. The second is asking whether the undercut is functional. A snap groove that holds a cover on is functional. A groove that exists because a draft angle was applied in the wrong direction is not, and removing it removes a permanent maintenance item.
Strip-off is worth knowing about because it is free and it is frequently overlooked. In PP, PE or TPU, an undercut of up to about 5% of the wall thickness, or 0.5 mm, can be pushed out of the tool by the part’s own flexibility, with no mechanism at all. The cost is a witness mark and some stress whitening at the bump, and a tool that wears at that edge. On a high-volume part in a soft resin that is usually the right trade. On a glass-filled engineering resin it is not a trade at all — the part will crack at the bump.
Gate position decides where the weld line lives
The gate is not a detail added at the end of the mold design. It is a decision made on the part, and it fixes three things that are very hard to change afterwards: where the weld line runs, which direction the material shrinks in, and where the gate mark lands on the visible surface.
Weld lines are the part of this that catches designers out. Whenever two flow fronts meet, they meet cold, and the joint they make is weaker than the surrounding material. Unfilled amorphous resins retain roughly 70–90% of their strength across a weld line; semi-crystalline resins 60–80%; glass-filled grades can drop to 40–60%, because the fibres do not cross the boundary — they lie parallel to it. A weld line across a load path is a designed failure point that will not appear in any FEA model that treats the material as isotropic.
Two consequences follow, and both are geometric:
- A hole always creates a weld line behind it. The flow splits around the core pin and rejoins downstream. Never put a hole on a sealing face, in a pressure boundary, or directly in a bending path, unless the gate is positioned so the rejoining happens somewhere harmless.
- The gate cannot be wherever the runner arrives. It has to be on a thick section, not a thin one, or it jets; it has to avoid a visible face, or the mark becomes an appearance issue; and it has to be far enough from thin walls that the material is still fluid when it gets there.
Where the gate mark is acceptable is a specification question, not a manufacturing one. "Gate mark on the inside surface, no witness ring wider than 2 mm" is a specification. Saying nothing and rejecting the first samples is not, and the argument that follows is unwinnable for both sides. For how the runner layout itself is chosen, see hot runner versus cold runner.
The four tolerance notes that cannot be met
Tolerance is covered in its own right in what to put on your drawing, so this section is only about the four notes that appear regularly and cannot be met by any tool, at any price. Recognising them early saves an argument later.
- ±0.05 mm on a dimension that crosses the parting line. That dimension is set by shut-off condition and platen parallelism, not by how accurately the cavity was cut. The band is ±0.08 to ±0.15 mm in a good tool and worse in a big one.
- ±0.05 mm on a dimension produced by a slider. Slider fit clearance, lock angle and wear over the run all enter. ±0.10 to ±0.20 mm is the honest range.
- A single bilateral tolerance on a glass-filled part. Flow-direction shrinkage and cross-flow shrinkage differ by a factor of two or three. One number cannot describe both, so either the drawing has two, or the part is measured in the wrong place.
- A tolerance with no datum scheme. If the drawing does not say where zero is, two inspectors will pick two different references and both will be right. This is the most common cause of a "dimensional problem" that turns out to be a measurement problem.
There is a fifth, softer one worth mentioning because it is so common: tolerancing everything. A drawing where every dimension carries the same tight band does not signal seriousness, it signals that nobody decided which dimensions carry function. The tool then protects all of them, and the price reflects the risk that was never real. For how those dimensions are proven once the tool exists, see mold trial approval.
Assembly features are designed, not added
Most plastic parts end up joined to another plastic part, and the joint is usually where the design was finished last. Four features account for most of the trouble.
Snap fits
A cantilever snap is a beam, and it fails at its root. The root fillet should be at least half the beam thickness, the undercut is usually 0.5–1.0 mm or 2–3% of the beam length, and the strain at assembly should stay under about 60% of the material’s yield strain — because you want the snap to work in service, not only on the day it was assembled. In glass-filled resins the allowable strain drops sharply, which is why glass-filled snap fits crack and unfilled ones do not.
Locating features
Two pins and a plane locate a part. Four pins over-constrain it and fight each other, and on a molded part with a tolerance of ±0.15 mm they fight hard enough to distort the assembly. If the housing needs to be located at four corners, two of those corners should be slots, not round holes — molded, the slot costs nothing.
Ultrasonic weld lines
A triangular energy director 0.3–0.5 mm high on one half, meeting a flat land on the other, welds reliably. A butt joint between two flat faces does not, because there is nowhere for the energy to concentrate and nowhere for the melt to go. The weld line is a feature that has to be drawn into the part before the tool is cut; it cannot be added to a molded part afterwards.
Plastic-to-plastic stack-up
When two molded parts mate, their tolerances add — two tools, two shrinkage behaviors, two measurement schemes. A ±0.15 mm band on each becomes ±0.3 mm at the interface, which is more than most cosmetic gaps allow. The fix is not tighter tolerances on both parts; it is designing the joint so the gap is set by one part and absorbed by the other. If the product is going to be made in small batches first, the same logic applies to the aluminum tooling described in low volume injection molding, where the achievable bands are wider again.
The twelve checks, in order of what they cost
This is the list, ordered so that the items which are most expensive to fix later come first. It is not a complete DFM methodology. It is the set of questions that, in our experience, account for most of the money.
- Is the wall within the resin’s range, and uniform to within 25%? If not, nothing downstream will be stable.
- Can every thick section be hollowed out and ribbed instead? This is where cycle time and part cost are won.
- Does every inner corner have a radius of at least half the wall? Free strength, free tool life.
- Is the outer radius equal to the inner radius plus the wall? Otherwise the corner is thin and the whole radius was wasted.
- Is there draft on every vertical face, sized to the surface and the texture? And more on the core than the cavity.
- Are ribs at 50–60% of the wall, with roots radiused and spacing at least twice the wall? This is the sink-mark check.
- Are bosses at 60% wall, tied to a side wall, and no deeper than three diameters?
- How many undercuts are there, and can any be aligned, removed or stripped off? Count them as mechanisms, not features.
- Where is the gate, and therefore where is the weld line? Ideally decided before the cosmetic surface was agreed.
- Are there tolerance notes that cross a parting line, cross a slider, or apply one number to a glass-filled part? These will not be met.
- Does the drawing have a datum scheme? Without one, inspection becomes an opinion.
- Are the snap fits, locating features and weld lines drawn in? They cannot be added after the steel is cut.
Run in this order, the list takes about an hour on a finished model and rather less on a sketch. The point of the order is that answers to the first four change the geometry, answers to the middle four change the mold, and answers to the last four change the specification — and the further down the list a problem sits, the more of the previous answers it invalidates.
What each decision does to the tool
Design decisions are usually discussed in the language of quality, which makes them sound like costs with no return. They are better discussed in the language of what they do to the tool and the cycle, because that is where the trade-offs actually live.
| Decision | What it does to the mold | What it does to the lead time | What it does to the part |
|---|---|---|---|
| Wall thickened by 30% | Almost nothing — the cavity is slightly smaller | Nothing to the tool | Cooling time rises with the square of thickness: roughly 1.7× the cooling share of the cycle |
| One slider added | A larger base, a second motion, wear plates, a lock block | Two to three weeks | No direct cost, but a maintenance item for the life of the tool |
| Undercut designed out | Simpler tool, fewer things that can jam | One to two weeks shorter | None, if the function survives the change |
| Inner radii added everywhere | Less EDM, easier polishing, stronger mold corners | Slightly shorter | Stronger part for no extra cost — the only improvement here that is free |
| Draft raised from 0.5° to 1.5° | None | None | Fewer scuff and drag rejects, which shows up as yield rather than price |
| Tolerance tightened from ±0.15 to ±0.05 mm | Jig grinding, wire EDM, a CMM on the bench, steel-safe allowances | One to two weeks, plus one extra trial | Nothing in the part, everything in the price — and a narrower process window forever |
| Finish raised from SPI B-1 to A-1 | Many more polishing hours, and a steel that will take a mirror: S136 or NAK80 rather than P20 | One to two weeks | No dimensional effect; every surface defect becomes visible |
| Coarse texture specified | Deep etch, and draft has to go up to match | About a week for the etch | Hides flow marks, which is usually why it was chosen |
| One more cavity | Larger base, longer build, a runner layout that has to balance | Three to four weeks | Lower cost per part, if the volume is really there |
| Cold runner changed to hot runner | Manifold, controller, wiring, more sensors | Two to three weeks | Less scrap mass and a shorter cycle — worth it above a volume threshold, wasteful below it |
| P20 changed to H13 | Different steel, different heat treatment, different machining hours | One to two weeks | No effect on the part; several times the tool life |
Two entries in that table are worth pulling out. Adding inner radii is the only line where the design change makes the tool cheaper and the part stronger at the same time; there is no reason ever to skip it. And tightening tolerance is the only line where the part gets no better at all — everything it buys is a narrower process window that has to be held for the life of the tool. Both facts are counter-intuitive to buyers who read tolerance as a proxy for quality, which is why they are worth putting in front of a customer early rather than late.
For the tooling side of these decisions — what the steel, the base and the surface treatment each contribute — see how mold steel is selected and what actually drives mold cost. For how the resulting tool is classified and what that implies for a given production volume, see the classifications of injection molds.
Frequently asked questions
When in the project should a DFM review happen?
Twice. Once at concept, when the geometry can still change freely — that review is short and it is where most of the value is. Then once on the finished 3D model, before the tool drawing is released, to catch what the concept stage could not see: wall transitions, rib thickness, draft, gate position. A third review after the tool drawing exists is not a DFM review, it is a change order. If you only get one, take the one on the finished model, because that is the last moment when a change costs days rather than weeks.
Will DFM change my design intent?
It should change the geometry and leave the intent alone, and if it cannot, the intent was not achievable in the first place. A good review does not tell you to make the part thinner and less stiff; it tells you that the stiffness is better obtained from ribs than from a thicker wall, which is a different route to the same function. When a recommendation does threaten the function, it comes with the trade-off stated: this radius will add 1.5 mm to the corner, or this undercut needs a slider and three weeks. Those are decisions for the designer, not for the toolmaker.
How much draft do I need on a textured surface?
Roughly one degree per 0.001 inch (0.025 mm) of texture depth, on top of the draft the base surface needed anyway. A fine matte grain around 0.5 mil ends up at about 1.5°; a heavy leather grain at 3 mil ends up at 3° or more. The trap is that texture is often chosen for appearance after the draft has been fixed, which turns a buildable part into one that scuffs on every shot. Decide the texture first, then the draft, then cut the steel — because the etch happens after the polish and the mold cannot be given more draft at that point without welding.
Can I avoid a slider by allowing a witness mark?
Sometimes, and it is worth asking. Two routes exist. The first is strip-off, which works on flexible resins with an undercut under about 5% of the wall or 0.5 mm, and leaves a witness line plus some whitening. The second is redesign: split the undercut between the two halves of the tool so the parting line runs through it, which turns a slider into a shut-off. Both change the appearance of the part somewhere. What you should not do is ask the toolmaker to "make it work" without deciding which of those two marks you are accepting, because the answer will be whichever one happened to be easier to build, not whichever one you can live with.
Is a 1.0 mm wall too thin?
Not in itself — 1.0 mm is routine in ABS, PP, PA and PBT, and 0.8 mm is common in small electronic housings. What decides it is the flow length to thickness ratio and the resin. A 1.0 mm wall that has to carry material 150 mm from the gate is a different proposition from one that carries it 30 mm, and a glass-filled grade needs more pressure to fill the same section than an unfilled one. The question to ask is not "is 1.0 mm thin" but "how far does 1.0 mm have to flow in this resin" — and if the answer is long, the fix is another gate or a hotter tool, not a thicker wall.
Who should do the DFM review — me or my molder?
The designer owns the intent, and the toolmaker owns the consequences, so the review has to be a conversation rather than a hand-off. In practice the most useful arrangement is that the designer runs the structural and functional checks and the toolmaker runs the manufacturability ones — fill, draft, ejection, undercuts, gate position — and both look at the same model at the same time, before the tool drawing is released. A review done entirely by the molder tends to optimise the mold and quietly give away function. A review done entirely by the designer tends to produce a part that is beautiful in CAD and impossible to eject.
None of the twelve checks requires special software or a specialist. They require a model, a resin, and about an hour of someone asking what the tool will have to do in order to make the part that is on the screen. The tool and the process behind it are set out in the plastic injection molding guide; the point at which the design becomes a mold drawing is covered in mold design and mold building; and if the design work itself is the gap, that is what product design, reverse engineering and DFM covers. Choosing who builds it is a separate question, answered in how to screen an injection molding supplier.
