A drawing stuck at quotation: first ask "can it be made stably?"
Last week we reviewed a thin-walled deep-cavity part: wall thickness 1.2 mm, depth 60 mm, with snaps on the side. For the same STEP file, CNC quoted 380 yuan/piece, and injection molding quoted 120 yuan/piece, but injection molding required an additional mold cost of 40,000. Purchasing asked "which one to choose," but the question itself was wrong—a threefold unit price difference is not the basis for selection; whether it can be made stably is. In thin-walled deep-cavity injection molding, pressure loss at the end of fill is large, and the probability of short shots and sink marks is high; CNC cuts a deep cavity from a solid block, and tool deflection and chatter marks are also hard to suppress. Both routes have risks, just at different points.
This article gives an executable judgment sequence: batch size → precision definition → appearance standard → structural risk. First rule out unstable options, then talk about cost. If the order is reversed, the unit price saved will be paid back in scrap and rework.
Five dimensions lay out the processes: batch size, tolerance, appearance, structure, inspection
Put the five processes in the same table, first look at common industry reference values, then confirm item by item according to the drawing. The values in the table are a starting point for judgment, not acceptance standards.
| Process | Applicable batch size | Minimum wall thickness (reference) | Conventional tolerance (reference) | Typical risk points |
|---|---|---|---|---|
| CNC machining | 1–500 pieces | Metal 0.8 mm / plastic 1.5 mm | ±0.05 mm (general features) | Deep-cavity tool deflection, thin-wall chatter marks, clamping deformation |
| 3D printing | 1–200 pieces | SLA 0.5 mm / SLS 0.8 mm / FDM 1.2 mm | ±0.2 mm or ±0.3% (whichever is greater) | Layer-line anisotropy, warping, hole position deviation |
| Sheet metal | 1–5000 pieces | Sheet thickness from 0.5 mm | ±0.1 mm (bent parts) | Springback, hole position offset, insufficient bend radius |
| Injection molding | From 500–10000 pieces | 0.8–1.5 mm (depending on material) | ±0.1 mm (general parts) | Sink marks, short shots, weld lines, warpage |
| Vacuum casting | 10–200 pieces | From 1.0 mm | ±0.2 mm | Shrinkage voids, air bubbles, defects near the gate |
How to compare? Three criteria: Batch amortization threshold—injection mold costs must be amortized over the number of parts; typically below 500 pieces the unit cost is higher than CNC or 3D printing; Precision must be calculated together with the inspection scope—it's easy to mark ±0.05, but CMM inspection costs may exceed machining costs, so key dimensions and sampling ratios must be noted on the drawing; Appearance defined by the A-surface—whether parting lines, ejector pin marks, gates, tool marks, and repair points are on the A-surface directly determines post-processing costs and yield.
Selection criteria: three if/then rules and an exclusion checklist
Turning the table from the previous section into actions requires only three criteria. Batch ≤50 with deep cavities, undercuts, or irregular curved surfaces—go with CNC or 3D printing first, don't touch molds—the tooling cost won't be recouped, and one design change wastes a whole set of steel. With mating surfaces and batch consistency requirements (hole positions, flatness, assembly clearance), prioritize CNC or injection molding; FDM's interlayer anisotropy and vacuum casting's curing shrinkage will push mating surfaces out of tolerance. For thin-sheet cladding parts and brackets, prioritize sheet metal, but first confirm the bend inner radius is not less than the sheet thickness and whether springback needs compensation, otherwise the developed dimensions won't match.
Exclusion checklist (execute in order)
- Does the structure have wall thickness transitions, sharp corners, or air trap locations? If yes, fix the structure first before discussing processes—no process can save it.
- Is the tolerance band for key dimensions smaller than the process's normal capability? If smaller, change the process or adjust the inspection scope—don't force it.
- Does the appearance A-surface cover parting lines, ejector pin marks, gates, or tool marks? If covered, post-processing steps must be added and costs recalculated.
- Which side of the amortization threshold does the batch fall on? Don't open molds for single pieces/small batches; don't force 3D printing for medium batches and above.
- Has the inspection method been decided? CMM, calipers, or gauges directly determine whether precision can be proven.
The solutions remaining after running the checklist are the ones that can be quoted and compared. If the order is reversed, you'll end up using a process that can't hold tolerance to beat down the price of another process that can't hold tolerance.
Failure warnings: four types of problems visible before the first article
Many rejections aren't caused by machining—they're baked in at the quoting stage. The following four types of problems can be flagged in advance by looking at the drawing and structural features, without waiting for the first article.
- Sink marks and short shots in thin-wall injection molding: Features—wall thickness ratio greater than 2:1, locally thinner than 0.8 mm, no transition at rib roots. Consequences—sink marks on the A-surface, short shots at the far end, unstable dimensions. Early signals—check whether filling simulation shows hesitation flow and weld lines, check whether wall thickness changes abruptly.
- Tool deflection and chatter marks in large flat-surface CNC: Features—tight flatness requirements, large overhang, no intermediate support. Consequences—tool deflection, step marks, chatter marks, poor fit during assembly. Early signals—listen for dull or squealing cutting sounds, check whether tool mark direction changes abruptly with feed; if necessary, do a semi-finish test cut first.
- Springback and hole position shift in sheet metal bending: Features—bend radius close to sheet thickness, holes too close to the bend line, cumulative multiple bends. Consequences—angle springback, hole position shift, assembly holes don't align. Early signals—measure developed dimensions and bend angles on the first article, don't just look at the outline.
- Shrinkage voids and air bubbles in vacuum cast parts: Features—abrupt wall thickness changes, gate position far from thick areas, insufficient venting. Consequences—shrinkage voids, air bubbles, surface pinholes; appearance parts are directly rejected. Early signals—check gate layout and wall thickness transitions, whether thick areas are downstream of the gate.
What these four have in common is: they can all be written on the quote. If a supplier only returns a unit price without flagging risk points, self-check against the features above before deciding whether to hand over the part. When structural risk is high, it's better to make one verification part first than to go straight to production.
Frequently Asked Questions (FAQ)
The following are the most commonly asked questions during drawing review and quoting. Answers are given from an engineering perspective, without committing to specific lead times or precision.
At how many pieces should I consider injection molding?
The common industry threshold is a few hundred to one or two thousand pieces: for small batches and complex structures, CNC or 3D printing has lower unit costs; as batch size increases, mold costs are amortized and injection molding becomes cost-effective. But material also matters—when engineering plastic performance is needed, it's often worth switching to injection molding earlier. The specific threshold depends on part size and mold complexity—don't decide based on piece count alone.
How tight should tolerances be?
Only tolerance the dimensions that function requires. Mating surfaces and locating holes should be toleranced per actual assembly requirements; non-mating surfaces can use general tolerances. Each step tighter in tolerance increases machining and inspection costs, and also increases the risk of out-of-tolerance. When unsure, start with standard values and let engineering evaluate before deciding whether to tighten.
Can 3D printed parts be used as structural components?
Yes, but it depends on the process and load direction. SLA and MJF are suitable for appearance and general load-bearing parts; FDM has weak interlayer strength and obvious anisotropy, so load-bearing directions should avoid the interlayer direction. For critical load-bearing parts, it's recommended to make a sample for actual testing first, or switch to CNC. Don't estimate printed part strength based on injection-molded parts of the same material.
How to choose between vacuum casting and injection molding?
Vacuum casting is suitable for small batches of tens to hundreds of pieces—molds are cheap and lead times are short, but dimensional stability and surface consistency are inferior to injection molding, with higher risks of shrinkage voids and air bubbles. Injection molding is suitable for large batches and parts requiring good consistency. If the batch isn't large but speed is needed, use vacuum casting first to verify the structure, then decide whether to cut a steel mold.
Several quotes differ greatly—what should I check first?
First align three things: whether material grades are the same, whether tolerances and inspection scope are the same, and whether appearance standards (A-surface definition) are the same. If these three differ, the quotes aren't comparable. Next, check whether post-processing, inspection reports, and mold cost amortization methods are included. If differences remain large, have each supplier write out their process route before comparing.
Key takeaways
- First determine the route by batch size: for single pieces up to a few dozen, prioritize CNC/3D printing; for hundreds, then evaluate vacuum casting; only at thousands or more is it worth discussing injection molding and mold opening. Before crossing this threshold, mold amortization will drive the unit price up.
- Tolerances are not better the tighter they are: only specify dimensions that truly mate, and give free tolerances to the rest. One extra ±0.02 callout usually means one more setup or one more finishing operation, increasing cost while assembly may not benefit.
- For appearance acceptance, define the A surface first: write the allowed locations of parting lines, ejector pin marks, gates, tool marks, and layer lines into the drawing. This is much easier than arguing afterward about whether "this counts as a defect."
- Structural risk determines yield: deep cavities, thin walls, sharp internal corners, undercuts, and large flat areas are high-incidence features for warping, sink marks, springback, and trapped air; mark them before quoting, don't wait for the first article.
- The selection sequence is a process of elimination: first eliminate unstable options, then compare cost and lead time among the remaining options, rather than first asking who is cheaper.
