Send a STEP file plus a 2D PDF drawing. The model carries geometry and the drawing carries intent, and a quote built on geometry alone is either padded for assumed tolerances or optimistic in a way that changes after the drawing arrives. On the drawing, tolerance only what function depends on (usually under 15% of dimensions), define a 3-2-1 datum reference frame on features that sit in one die half, mark cosmetic and hidden surfaces, and state alloy, finish, annual volume and whether draft is already applied. The five submissions that delay quoting most are no 2D drawing, blanket ±0.05 mm on every dimension, no volume stated, a model with zero draft and sharp corners, and a cosmetic requirement communicated verbally.
A die casting quote is a set of engineering judgements about your part: which features can be cast to size, which need machining, how many cavities the volume justifies, whether the geometry needs a slide, and how much of the surface anyone will ever look at. Every one of those judgements comes from something you send or something we have to assume.
The difference between a submission that gets quoted in 24 hours and one that takes two weeks is rarely the complexity of the part. It is whether the intent arrived with the geometry.
The short list
Six items, and the first two are not optional.
- A 3D solid model, ideally STEP.
- A 2D drawing as PDF, carrying tolerances, datums, alloy, finish and cosmetic requirements.
- Annual volume and the three-year outlook.
- Alloy, or the requirement that should drive alloy selection.
- Finish, including a colour reference and any salt spray requirement.
- Assembly context: the mating parts, or at least an envelope.
Everything below is detail on those six.
File formats, and why STEP
| Format | Extension | Verdict | What it carries |
|---|---|---|---|
| STEP AP214 / AP242 | .step, .stp | Preferred | Exact B-rep solids, units, assembly structure; AP242 can carry tolerances as PMI |
| Parasolid | .x_t, .x_b | Very good | High-fidelity B-rep solids, readable by any Parasolid-based system |
| Native SolidWorks | .sldprt, .sldasm | Very good | Full feature tree; state the version so we can confirm we can open it |
| Native Creo / NX / Inventor | .prt, .ipt | Usable | Same benefit, same version caveat |
| IGES | .igs, .iges | Acceptable | Surfaces, frequently unstitched; healing gaps adds a day to quoting |
| Mesh formats | .stl, .3mf, .obj | Not usable for tooling | Triangulated approximation; curvature is already lost |
| 2D drawing | Required | Tolerances, datums, alloy, finish, cosmetic zones, notes | |
| 2D CAD | .dwg, .dxf | Helpful | Useful for trim dies, gauges and fixture design |
STEP is preferred for one specific reason: it is a boundary-representation format, so the surfaces we receive are the surfaces you designed. A die is cut from that geometry, and cavity surfaces are offset, drafted and shrink-compensated from it. Any approximation in the incoming file propagates into the steel.
That is why mesh formats are not usable. An STL of a Ø52 bore is a many-sided polygon, and there is no way to recover the intended diameter from it with confidence. A mesh is fine for a visual check or a 3D print, and it cannot be the source geometry for tooling.
Two practical notes. Export solids rather than surface bodies, and confirm the model is a single closed solid per part. And state units on the drawing even though STEP carries them, because a millimetre-inch mismatch is a failure mode that survives every other check.
Why a 3D model alone cannot be quoted accurately
A model is geometry. A quote needs intent, and the gap between the two is expensive in both directions.
Take a housing with 40 dimensions. If six are critical, machining might be one setup and 2.4 minutes. If we cannot tell which six, we have two options: assume tight and quote three setups at 4.8 minutes, which is roughly double the machining cost and means you pay for tolerance nobody needs; or assume loose and quote one setup, which means the price changes upward when the drawing arrives. The second is worse, because it happens after you have made a sourcing decision.
The same asymmetry applies to alloy, finish, cosmetic requirements and volume. Every unstated input becomes a padded assumption or a deferred surprise. A geometry-only quote is a genuinely useful budgetary number, and it should be treated as one.
Marking critical versus non-critical dimensions
This is the highest-return five minutes you can spend on the drawing.
| Tolerance called out | How it is produced | Cost consequence |
|---|---|---|
| ±0.25 mm or looser | As-cast | Free |
| ±0.1 mm | As-cast, standard capability for the first 25 mm | Free |
| ±0.05 to ±0.1 mm | As-cast on one die half, CMM verified, or a skim cut | Low |
| ±0.02 to ±0.05 mm | CNC machining after casting | Setup plus cycle time per feature |
| Tighter than ±0.02 mm | Grinding, honing, or machine the part from billet | Substantial, and worth challenging |
Three habits worth adopting:
- Balloon the critical dimensions and let a general tolerance block cover the rest. On most housings and enclosures, fewer than 15% of dimensions are genuinely functional. A blanket ±0.05 mm applied to 34 dimensions where 6 matter is the most common avoidable cost we see on incoming drawings.
- Group the critical features onto one or two faces at design time. Setup count drives machining cost harder than cycle time. One bearing bore and one sealing face on the same face is routine; the same features split across four faces turns one setup into three.
- Say what the tolerance is for. A note reading “Ø52 H7, bearing press fit” lets us machine it correctly. A bare ±0.015 mm on a diameter gets machined correctly too, but it removes the chance to point out that a slip fit with a retaining ring would be cheaper.
Datums and the datum reference frame
A casting arrives with no flat, square reference surface anywhere on it, so the datum scheme is not a drawing formality. It is the thing that determines whether every part comes out the same.
Define a 3-2-1 reference frame on the part drawing: three features establishing the primary plane, one for secondary location, one for rotational constraint. Then check it against three constraints specific to casting.
- All datum features should sit in one die half. Parting line mismatch of ±0.1 to ±0.15 mm is normal, and a frame that straddles the line inherits that mismatch as fixture error on every part.
- Prefer features in the fixed die half, which holds position more consistently shot to shot than the moving half.
- Avoid datums on surfaces formed by a slide. A slide has its own position variation, and a reference frame built on one carries it.
Small raised cast pads make better datums than large faces. They are cheaper to clean up, they are unaffected by warp elsewhere on the part, and they give the fixture a defined three-point contact rather than an ambiguous plane. Give them 0.5 to 0.8 mm of extra stock so the first operation can skim them into a true reference.
If the drawing arrives with no datums, we will propose a scheme in the DFM report. It is better to receive one from you, because you know which surfaces the assembly actually references.
Cosmetic surfaces and hidden surfaces
Cosmetic requirements are the single most common source of first-shipment disputes, and almost always because they were discussed rather than drawn.
Mark a zone map on the drawing using three classes:
| Class | Definition | What is acceptable |
|---|---|---|
| A | Visible in normal use | No sink marks, no flow lines, uniform texture, no ejector witness; gate and parting line positioned outside the zone |
| B | Visible during installation or service | Minor flow lines acceptable, light parting line witness, no sink marks in the field of view |
| C | Hidden in the assembly | Ejector pin witness, gate witness and parting line flash acceptable within stated heights |
The reason this matters at quotation rather than at inspection is that a Class A designation is a tooling decision. It constrains where the gate can go, where overflows can go, where ejector pins can land and where the parting line can run. Declaring a large flat face Class A after the die is designed is a die modification. Declaring it before costs nothing but the ink.
Also state the allowable heights for flash, parting line witness and ejector witness on Class C surfaces, so acceptance is measured rather than argued.
Alloy, finish and the requirement behind them
State the alloy if you know it. State the requirement if you do not, because the requirement is the more useful input.
- “Must be pressure tight at 6 bar” leads to A360 aluminum, rated excellent for pressure tightness.
- “Must fill a 1.8 mm wall over a 200 mm flow path” leads to ADC12 and its 9.6 to 12% silicon.
- “Must move as much heat as possible” leads to A413 at 121 W/m·K, in the aluminum-silicon alloy family.
- “Cheapest that will do the job, and it is heavily machined” leads to A380.
One alloy note worth checking before you send: if the drawing says 6061 or 7075, it cannot be die cast. Wrought alloys carry under 1% silicon and will short-fill and hot-tear. If 6061 is on the drawing because it was inherited from a machined predecessor, it is worth revisiting; if it is there because the part is anodized for appearance, welded or heat treated to T6, the drawing is right and the part should be machined from billet instead.
For finish, state the process, a colour reference (RAL, Pantone or a physical sample), a gloss window, a film thickness range if a fit depends on it, and any salt spray hours. Then mark what gets masked: threads, bores, sealing faces, grounding pads and machined datums, because 60 to 120 µm of powder will take an H7 bore out of tolerance. The surface finishing page lists what each process achieves.
Volume, ramp and target price
Annual volume changes the quote more than any other single number, because it sets cavity count, machine selection and whether the machining fixture is manual or hydraulic. Send three figures: first-year volume, steady-state annual volume, and expected program life in years.
A target price is worth including too. It is not a negotiating weakness; it tells us immediately whether to quote a single-cavity or a multi-cavity tool and whether the design needs cost reduction before it is viable. If the target is $6 and the design as drawn quotes at $11, the useful response is a list of the changes that close the gap, which is the analysis in how to reduce aluminum die casting cost.
Draft, fillets and machining callouts
Three model-level items that determine whether the DFM review comes back clean.
Draft. State whether it is applied. If it is, give the values so we can confirm 1 to 2° external and 2 to 3° internal. If it is not, say so and we will add it and return the modified model for approval. The problematic submission is a zero-draft model with no note, because those walls have to be treated as final geometry.
Fillets. Internal corners want 1 mm minimum radius. Sharp internal corners concentrate thermal fatigue in the die and heat-check it at exactly that point, so a model with sharp corners everywhere generates a DFM round trip. The target values for draft, fillets, ribs and wall thickness are all in the aluminum die casting design guide.
Machining callouts. Flag every feature intended to be machined after casting, and say how the allowance is handled. Two conventions work:
- One net-shape model plus a drawing table listing each machined feature and its allowance. Compact, and fine for simple parts.
- Two models, one as-cast and one as-machined. Unambiguous, and worth the effort on any part with more than about six machined features.
Whichever you use, mark the faces that stay as-cast so stock is not added where none is needed. Allowance values by feature are in CNC machining after die casting.
Assembly context
Send the mating parts, or a simplified envelope, or even a screenshot of the assembly. It costs you nothing and it changes what we can suggest.
With assembly context we can see which surfaces are functional and which have 3 mm of clearance behind them, spot an interference before it becomes a tooling change, identify the fasteners so bosses can be sized for proper thread engagement, and, most valuably, notice the adjacent bracket or spacer that could become a feature of your casting. Part consolidation is the largest cost lever in die casting and it is invisible when you only look at one part.
Pre-submission checklist
| Item | Why it matters |
|---|---|
| 3D solid model in STEP, single closed solid | Source geometry for the die; no healing required |
| 2D PDF drawing with a title block and revision | The commercial and quality contract for the part |
| Units stated, mm or inch | Survives every other check if it is wrong |
| Critical dimensions ballooned, general tolerance block for the rest | Sets machining scope and therefore most of the piece price |
| Datum reference frame defined, all datums in one die half | Determines part-to-part repeatability |
| Cosmetic zone map, Class A / B / C | Constrains gate, overflow, ejector and parting line positions |
| Allowable flash, parting line and ejector witness heights | Makes cosmetic acceptance measurable |
| Alloy stated, or the requirement behind it | Drives pressure tightness, conductivity and cost |
| Finish stated with colour, gloss and salt spray reference | Sets finishing cost and masking plan |
| Masked features identified | Prevents coating taking a bore or thread out of tolerance |
| Machined features flagged with allowance convention | Sets fixture design and machining sequence |
| Draft status stated | Determines whether the part can eject as drawn |
| Annual volume, ramp and program life | Sets cavity count and tooling class |
| Target price, if you have one | Tells us whether to quote as-drawn or propose changes |
| Assembly context or mating parts | Enables consolidation and interference checks |
| Special requirements: leak test, X-ray level, PPAP, traceability | Must be priced in, not added later |
The mistakes that delay quotes
| Mistake | What it costs | Fix |
|---|---|---|
| No 2D drawing | 2 to 5 extra days, and a quote we have to caveat | One PDF with critical dimensions, datums, alloy and finish |
| Blanket ±0.05 mm on every dimension | 40 to 100% more machining cost, or a request to re-tolerance before we can quote | Tolerance function; leave the rest at ±0.25 mm as-cast |
| No annual volume stated | Wrong cavity count and wrong tooling class in the quote | First-year, steady-state and program life |
| Zero draft and sharp corners everywhere, with no note | A DFM round trip before quoting can begin | Apply 1-2° and 2-3° draft with 1 mm fillets, or state that we should |
| Cosmetic requirement discussed but not drawn | Rejected parts at first shipment and an argument about who pays | Class A/B/C zone map on the drawing |
| Mesh file only | Cannot be used for die design at all | Send STEP |
| 6061 or 7075 on the drawing | The part cannot be die cast as specified | Change the alloy, or machine it from billet |
| Machined features not identified | Allowance added in the wrong places, or not at all | Flag each one with its allowance |
| Coating specified without masking callouts | Powder in an H7 bore or a tapped hole | Mark every masked feature |
What happens to your files
Confidentiality is a reasonable question to ask before sending anything, so here is the position plainly.
NDA first, if you want one. Send yours and it will be reviewed and returned, usually the same day, before any files are transferred. If you would rather use ours, we can supply a mutual confidentiality agreement.
Access is limited to the assigned team. Files are held on internal, access-controlled systems and are visible to the DFM engineer, the tool designer and the quoting engineer working on your program. Drawings are not circulated outside that team.
Sub-suppliers see only what they need. Some operations, such as specialised coatings, involve a qualified partner. Where that applies, they receive the part and the finish specification, not your assembly drawings or your commercial terms.
Tooling is yours. Once paid for, the die is your property, is dedicated to your part, is not used to produce parts for anyone else, and can be transferred on request.
Records are kept for the program, and then removed on request. Drawings, revisions and inspection records are retained for the life of the program and the traceability period our ISO 9001:2015 system requires. Beyond that, files are deleted on written request.
Nothing is published without written approval. That is why the case studies on this site describe customers by type rather than by name, and why none of them show a photograph of a part we were not given permission to show.
What comes back
A complete submission gets a quotation within 24 to 48 hours, and it comes with a written DFM report rather than just a price: wall thickness and draft assessment, fillet and rib recommendations, a proposed gate and overflow strategy, a datum scheme, the machining scope we assumed, cavity count options with the break-even volume against each, and a note on any feature that will not behave as drawn.
Send files through contact. If the honest answer is that your volume or geometry does not justify a die, the report will say that, and it will say what to do instead.
