A drawing that says ±0.05 mm on every dimension and "SPI A-2" in the title block looks professional. It is also the single most common reason a quotation comes back high, and the reason two honest parties end up arguing about a part that was never capable of meeting the number on the paper. Tolerance is not a measure of how much you care. It is a specification you will be held to, and the only useful one is the one the process can actually hold.
Why a plastic part cannot be held like a machined part
A machined part is a piece of metal cut to a number. The tolerance is a statement about the machine and the operator, and a good shop can hold ±0.01 mm all day because the material does what it is told.
An injection molded part is a piece of metal that was cut oversize on purpose, filled with hot resin, and then allowed to shrink into its final shape by an amount nobody knows exactly. Four independent sources of error land on every dimension, and they are not the same size.
| Source of variation | Typical magnitude | Who controls it | How to reduce it |
|---|---|---|---|
| Mold machining and assembly | ±0.01 to ±0.03 mm | Toolmaker | Jig boring, jig grinding, fixed EDM offsets, leader pins bored in one setup |
| Shrinkage prediction error | 0.2–1.0% of the dimension — i.e. 0.2–1.0 mm at 100 mm | Resin, part design, gate position | Mold flow analysis, steel-safe allowance, walking the tool in over two trials |
| Process window drift | ±0.03 to ±0.08 mm | Molder | SPC on the critical dimensions, a wider process window in the tool design |
| Measurement and environment | ±0.01 to ±0.02 mm | Both parties | Agreed method, agreed temperature, agreed settling time |
Look at the middle row. A datasheet that gives shrinkage as 1.5–2.0% is telling you the finished dimension is uncertain by 0.5% of its own size. At 100 mm, that is a 0.5 mm spread — a band of ±0.25 mm before a single part has been molded. Any drawing that asks for ±0.05 mm on that dimension is asking the toolmaker to resolve an uncertainty that lives in the resin, not in the machine.
This is why the argument about tolerance usually happens in the wrong place. Buyers push on the machining tolerance, because that is the number they can picture. Toolmakers push back on the process window, because that is the number they can measure. The term that actually decides the outcome is shrinkage, and it is the one nobody puts in the purchase order.
The practical consequence. A precision dimension is not cut correctly on the first attempt. It is cut on the small side of nominal, measured on the first samples, and then adjusted — once, sometimes twice. What you are really buying with a tight tolerance is not a more accurate cut. It is the tool’s capacity to be corrected, plus the trials needed to do it. That capacity has to be designed in before the steel is cut.
The second consequence is about measurement. Because the shrinkage term is large, two parties measuring the same part with different methods will disagree by more than the tolerance. That disagreement is not a quality problem, it is a specification problem — and it is covered further down in how the specification gets measured.
Six kinds of dimension, six different limits
The single most useful thing to understand about molding tolerance is that it is not one number. It depends on where the dimension sits in the tool. Two features cut into the same block of steel, measured in the same direction, are a completely different proposition from a height measured from the opposite half.
| Type of dimension | What actually limits it | Realistic band |
|---|---|---|
| Two features in the same half, measured in the same direction | Cavity cutting accuracy plus shrinkage repeatability | ±0.03 to ±0.05 mm |
| A dimension across the parting line (a height, a depth from the other half) | Shut-off condition, platen deflection, parallelism of the plates | ±0.08 to ±0.15 mm |
| A dimension produced by a slider or a lifter | Slider fit, wear over the run, lock angle, thermal growth of a long slide | ±0.10 to ±0.20 mm |
| A free dimension that ends in air | Warpage and cooling imbalance, not the cavity | ±0.15 mm or worse |
| Plastic-to-plastic assembly stack-up | Two tools, two shrinkage behaviors, two sets of tolerances | ±0.15 to ±0.25 mm combined |
| Plastic onto a purchased metal component | The metal part’s own tolerance is not yours to control | Design clearance, do not chase the number |
Three of those rows are worth dwelling on, because they explain most of the arguments that reach a buyer’s desk.
Anything across the parting line is limited by shut-off, not by cutting. The dimension depends on how completely the two halves meet, under what clamp force, on plates that deflect slightly and heat unevenly. This is the reason a mold can hold ±0.03 mm on the cavity and still be ±0.12 mm on the overall height, and it is the reason a peened parting line shows up first as a dimension problem rather than as flash.
Slider dimensions get worse with time, not with the drawing. A slider is a moving fit. It has clearance when new and more clearance after 200,000 cycles. A tolerance that is only achievable with a fresh slider is a tolerance that will be out of spec for most of the tool’s life, and no drawing note prevents that.
Free dimensions are governed by warpage. An edge that ends in air is not controlled by the cavity at all; it is controlled by how evenly the part cooled. Calling it ±0.05 mm does not make it so — and the honest engineering answer is to make that dimension non-critical by designing the mating part with clearance, which is exactly the kind of decision covered in product design and DFM.
Tolerance grades and the bands that are real
Most drawings either state a general tolerance in the title block or say nothing at all. Four grades cover almost every real requirement. These are empirical shop-floor bands for unfilled to lightly filled resin in a well-built tool, not a quotation from a standard — standards exist, and their tables assume conditions many parts do not meet.
| Grade | 0–30 mm | 30–120 mm | 120–400 mm | Where it is normally seen |
|---|---|---|---|---|
| General | ±0.10 | ±0.15 | ±0.25 | Cosmetic faces, non-mating dimensions, most consumer housings |
| Precision | ±0.05 | ±0.08 | ±0.12 | Plastic-to-plastic mating, snap fits, locating ribs |
| Fine | ±0.03 | ±0.04 | ±0.06 | Sealing faces, small gear teeth, connector keying |
| Special | ±0.015 | ±0.02 | ±0.03 | Optical mounts, instrument bores, single-cavity precision work |
Read the table as a budget, not a menu. Moving a whole part from General to Precision is a modest cost increase and often justified. Moving it to Special is not a tolerance decision at all — it is a decision to build a single-cavity tool, run it in a temperature-controlled room, and accept a slower cycle. Those are not things a note on a drawing can buy.
Two conditions sit underneath every number in that table, and both are frequently missing from drawings:
- Measured on a part that has stopped moving. Plastics continue to shrink and, in the case of polyamides, to grow. The band only means something at a stated time and moisture state.
- One direction per dimension. A dimension measured along the flow is not the same as the same nominal distance measured across it, particularly with glass-filled resin. A drawing that tolerances a diameter as one number is implicitly assuming the part stays round, and it will not.
Shrinkage is a range, not a number
Every resin datasheet gives shrinkage as a range, and the width of that range is the real tolerance floor of the project. The table below is the practical version: what each resin typically does, and what makes it move within its own range.
| Resin | Shrinkage, flow direction | Cross-flow | What to watch |
|---|---|---|---|
| PP homopolymer | 1.4–2.0% | 1.2–1.8% | Moves with wall thickness and melt flow grade; the widest range of any common resin |
| PP + 30% glass fibre | 0.3–0.6% | 0.8–1.2% | Cross-flow runs two to three times the flow value, which is why glass-filled parts warp |
| HDPE | 1.5–3.0% | similar | Thick sections push toward the top of the range |
| ABS | 0.4–0.7% | similar | Forgiving; the usual choice when a new tool has to land close first time |
| PC | 0.5–0.7% | similar | Residual moisture adds dimension error on top of shrinkage |
| PC/ABS | 0.5–0.7% | similar | Behaves closer to ABS in the tool, closer to PC in service |
| PA6, unfilled | 0.5–1.5% | similar | Grows after molding as it absorbs moisture — a 100 mm dimension can move by tenths of a millimetre |
| PA6 + 30% glass fibre | 0.2–0.4% | 0.6–1.0% | Strongly anisotropic; the gate position decides which dimension gets which value |
| POM | 1.8–2.5% | similar | High and consistent, but post-molding shrinkage continues for days |
| GPPS | 0.4–0.7% | similar | Low, but brittle — ejection marks show as stress whitening |
| PMMA | 0.3–0.6% | similar | Optical parts: thickness tolerance matters more than length |
| PBT + 30% glass fibre | 0.2–0.5% | 0.5–0.9% | Fast crystallising; warpage is the practical limit, not shrinkage |
| Rigid PVC | 0.2–0.6% | similar | Low shrinkage, but the resin attacks steel — see the note on corrosion below |
The glass-filled rows are the ones that surprise people. A 30% glass-filled polyamide shrinks roughly 0.3% along the flow and roughly 0.9% across it. On a 100 mm dimension that is a 0.6 mm difference between two directions in the same part. A round boss molded in that resin comes out noticeably oval, and no amount of toolmaking precision changes it — the core has to be cut oval on purpose to compensate. That is a design decision, and it is invisible on a drawing that tolerances a diameter as a single value.
The polyamide rows matter for a different reason: those parts keep changing after they leave the molder. Unfilled PA6 absorbs moisture from the air and grows, by enough to consume a precision tolerance on a large dimension within weeks. If your part is PA6 and your tolerance is ±0.05 mm on 100 mm, the only honest specification adds a conditioning state — and the cheapest fix is usually to change the resin or loosen the dimension, not to fight it.
Selecting for dimensional stability rather than for strength is a legitimate design goal, and it is the same conversation as choosing the mold steel: both are decided before the tool is cut, and both are expensive to revisit afterwards.
Steel safe: the only strategy that survives the first trial
A mold can only lose steel. Every correction — re-spotting a shut-off, polishing a cavity, re-cutting a gate — removes material, and none of them add it back. That single asymmetry dictates how a tool should be cut whenever a dimension is expected to need adjustment.
The rule follows from the direction of material removal:
- An outside dimension gets smaller when you remove steel from the cavity. So cut the cavity slightly small, and you retain the ability to enlarge the part. Cut it large and the part can only get larger still.
- A hole or an internal dimension gets smaller when you remove steel from the core. So cut the core slightly large, and you retain the ability to shrink the hole.
In both cases the allowance is left on the side that material removal can reach. That is what "steel safe" means, and it is the reason a well-built tool is not delivered with every dimension sitting at nominal. A tool with all dimensions dead center has no correction path at all, which is fine only if the first trial lands perfectly — and it usually does not.
The same logic already appears in mold maintenance from the repair side, where it explains why a worn shut-off can be corrected but an oversized cavity cannot. It appears in mold trial approval from the measurement side, where it explains why the first trial should aim at the middle of the band rather than at the nominal. This section is the third view: the allowance has to be decided at quotation, not discovered at trial.
What to ask for. Ask the toolmaker what steel-safe allowance they are carrying on the critical dimensions, and in which direction. A supplier who can answer that question in one sentence has thought about correction. A supplier who answers "we cut to the drawing" has told you that the first trial is the only trial they planned for.
What each step in tolerance actually costs
Tolerance cost is not linear. It is a staircase, because each band crosses a process boundary: at some point you stop milling and start grinding, stop checking a sample and start measuring every cavity, stop trusting the room temperature and start controlling it.
| Band you specify | Relative tool cost | What has to change in the shop |
|---|---|---|
| ±0.15, or no tolerance stated | Baseline (100) | Standard CNC and EDM, ordinary spotting, sample inspection |
| ±0.10 | 100–110 | Nothing structural; better spotting discipline and a written measurement method |
| ±0.05 | 115–135 | Jig boring, jig grinding, steel-safe allowance, CMM report per cavity |
| ±0.025 | 145–180 | Surface grinding, temperature-controlled room, EDM with fixed offsets, a second trial |
| ±0.01 | 200–280 | Few cavities only, wire EDM, climate control, 100% CMM, and a molder running SPC |
The step between ±0.05 and ±0.025 is the expensive one, and it is worth understanding why. At ±0.05 mm, the toolmaker is still working within the accuracy of good CNC and EDM practice. At ±0.025 mm, thermal expansion of the workpiece during machining becomes comparable to the tolerance itself: steel moves about 0.012 mm per 100 mm per degree Celsius. A workshop that swings five degrees between morning and afternoon cannot hold that band by skill alone — it needs a controlled room, and a controlled room is a capital cost that has to be recovered on every tool.
The inspection side is the same story in a different currency. A ±0.025 mm requirement on a multi-cavity tool means measuring every cavity, not one. That is CMM time on the toolmaker’s side and on the molder’s side, every trial, for the life of the tool. None of it appears in the drawing, and all of it appears in the price breakdown.
There is also a hidden cost that shows up later: a tool built to a very tight band is a tool with a narrow process window. It will hit the number in the toolroom and drift in a production hall where the ambient temperature changes with the season. The bill for that arrives as unexplained rejects, and the usual response is to slow the cycle down, which quietly raises the piece price for the rest of the program.
Where tight tolerance pays, and where it does not
The useful test is not "how accurate can this be made" but "what does this dimension do". A dimension that carries a function is worth paying for. A dimension that carries nothing but habit is a donation.
Worth the money
- Sealing surfaces — a gasket groove or a lip that has to compress by a known amount
- Snap fit engagement — the undercut depth and the mating wall that the hook catches on
- Bearing bores and shaft seats — anything that receives a purchased component to a specified fit
- Optical and light-pipe features — where a tenth of a millimetre changes the light path
- Electrical connector keying — where the part must mate with a standard, not with another part of yours
Usually not worth the money
- Free cosmetic surfaces — the outside of a housing that touches nothing
- Wall thickness in a non-structural shell — controlled by the tool’s cavity anyway
- Any dimension followed by a machining operation — you are paying twice for the same accuracy
- Dimensions downstream of a flexible feature — a living hinge or a thin web will not transmit a tight number
A drawing with ±0.05 on every dimension is a signal that nobody separated function from geometry. The cost of that signal is typically 15 to 35% on the tool, and it buys nothing at the assembly station, because the dimensions that mattered were already inside the band.
Not sure which dimensions on your drawing are carrying the cost?
Send us the drawing. We will mark the dimensions we would treat as critical, the ones we would open up, and the ones where the resin rather than the tool sets the limit — and we will say plainly if the tolerance on your part is buying nothing.
Surface finish: SPI, VDI and what each one demands
Surface finish is specified two ways in practice. SPI is the American mold-finish scale, quoted as a letter and a number and defined largely by the abrasive that produced the surface. VDI 3400 is the European scale, quoted as a single number, and defined by a photographic reference plaque rather than by a measured value.
SPI grades run from A-1, a mirror polish, to D-3, a coarse blast texture. The Ra figure attached to each grade is a roughness average, and it is a useful target but not a complete description — two surfaces with the same Ra can look different, because Ra averages out the waviness that the eye actually detects under a gloss highlight.
| SPI grade | Ra (µm) | How the steel is finished | Practical note |
|---|---|---|---|
| A-1 | 0.012–0.025 | #3 diamond, high gloss | Needs clean, hard steel; a fingerprint etched overnight is permanent |
| A-2 | 0.025–0.05 | #6 diamond | The realistic version of "high gloss" for production |
| A-3 | 0.05–0.10 | #15 diamond or fine paper | Gloss reading depends heavily on the resin |
| B-1 | 0.05–0.10 | 600 grit paper | The most commonly specified visible finish |
| B-2 | 0.10–0.15 | 400 grit paper | Hides minor polishing inconsistency |
| B-3 | 0.15–0.20 | 320 grit paper | Where subtle sink starts to become visible |
| C-1 | 0.20–0.28 | 600 stone | Semi-gloss; forgiving on flow marks |
| C-2 | 0.28–0.35 | 400 stone | Matte, common on internal parts |
| C-3 | 0.35–0.45 | 320 stone | Matte; texture direction becomes visible |
| D-1 | 0.45–0.63 | Fine dry blast | Cheapest way to hide weld lines and flow marks |
| D-2 | 0.63–0.80 | Medium dry blast | Holds dirt; needs more cleaning between runs |
| D-3 | 0.80–1.00 | Coarse dry blast | Can bridge and drag if draft is under about 1.5° |
Three practical points about that table.
Ra is not gloss
Gloss is what the customer sees, and it depends on resin, on mold temperature and on packing, not only on the steel. A B-1 cavity in ABS will look different from a B-1 cavity in polypropylene, because the resin replicates the texture to a different degree. If appearance is the requirement, specify the grade and agree a physical sample plaque, molded in the production resin. That plaque is the only finish specification that survives an argument.
VDI is not a conversion of SPI
The VDI number is a reference to a photograph, and the same number produced on different steels, at different etch depths, does not look identical. A supplier who quotes "VDI 27 or SPI B-1" is not describing the same surface twice — they are offering you two different surfaces and hoping one will do. Ask for Ra plus a plaque, whichever scale they use.
Every step up the scale costs polishing time, and polishing time is skilled labour. The jump from B-3 to A-2 is not a small increment; it is a change from abrasive paper to diamond paste, done by hand, on a surface that must not be touched with a bare finger afterwards. It also constrains the steel: a mirror polish needs a clean, homogeneous, hard material, which is one of the reasons free-cutting steel with sulphur additions can never reach A-grade, whatever the polishing effort.
Texture is a one-way door
An etched texture is produced by masking the mold face and exposing it to acid, which removes steel and leaves a grain. Three consequences follow, and all three are decisions that must be made before the tool is cut.
Etching enlarges the cavity. Material is removed, so the part grows slightly and the texture sits inside that growth. The allowance has to be part of the steel-safe budget from the start — it cannot be added later without eating into the tolerance you were trying to protect.
You cannot polish a texture back. Once etched, polishing destroys the grain, and restoring it means re-masking and re-etching the whole face. So a textured tool that develops a flow mark cannot be fixed the way a polished tool can: there is no local polish-and-blend repair. This is the single strongest argument for getting flow analysis right on a textured part before cutting steel.
Deep grain needs extra draft. A leather grain at 0.1 mm etch depth adds effective roughness that the part has to slide over on ejection. The practical rule is 1.5 to 3 degrees of additional draft per side, depending on depth and on how glossy the resin is. A drawing that specifies a texture and leaves draft at 0.5 degrees is specifying a part with drag marks and a mold that has to be re-cut.
Texture is also a maintenance decision, not only an appearance one. A blasted or etched surface holds resin residue and release agent, and it has to be cleaned more carefully than a polished one — the same point that makes a written cleaning routine matter more on textured tools than on mirror ones.
How the specification gets measured
A tolerance with no measurement method is an opinion. Four things have to be agreed, and all four belong on the drawing or in the purchase order.
The gauge has to be finer than the tolerance. The rule of ten is the working standard: the measuring instrument’s resolution should be at least ten times finer than the band you are checking. A ±0.05 mm tolerance needs 0.005 mm of resolution, which means a micrometer or a CMM — a caliper with 0.01 mm resolution and worse accuracy is measuring its own error as much as the part. On a ±0.02 mm tolerance, a caliper is not a measurement, it is a rumour.
The part has to have stopped moving. Molded parts continue to change after ejection: semi-crystalline resins keep shrinking, and polyamides absorb moisture and grow. The convention that prevents most disputes is to measure 24 to 48 hours after molding, dry, at 23 ± 2 °C. Whichever settling time you choose, write it down — because a part measured hot and a part measured two days later are different parts, and both parties will be honest and still disagree.
The datum scheme has to follow function. Datums taken from the parting line are convenient for the toolmaker and usually wrong for the assembly, because the parting line moves as the tool wears while the functional features do not. Set A, B and C on the surfaces that actually locate the part in its application. This is the same logic that makes a trial report readable or unreadable: a report against functional datums tells you whether the part will work, a report against the mold tells you whether the mold is to drawing.
The report has to carry actual values. A report that says OK or NG for sixty dimensions gives you no trend, and trend is what tells you whether the tool is drifting. Ask for the measured value and the deviation from nominal, per cavity, for the critical dimensions. Six numbers you can watch are worth more than sixty numbers you cannot.
One question that saves a program. Ask the molder to send the last three months of SPC data on one critical dimension before you place a production order — not a capability study run for your visit, the routine data. If the dimension has been drifting, you will see it in the trend, and you will see it before it becomes a rejected shipment.
Six lines to add to your drawing
Most tolerance disputes are not about capability. They are about a drawing that did not say what it meant. These six lines close the gap, and none of them costs anything to add.
- "All dimensions apply at 23 ± 2 °C, 48 hours after molding, dry as molded." This alone prevents a large share of measurement disagreements.
- "General tolerance ±0.10 unless noted; dimensions marked ★ are critical and per the table below." One grade for the bulk of the part, an explicit list for the dimensions that matter.
- "Datum A = … B = … C = …" Defined on functional surfaces, not on the parting line, and stated as a real coordinate scheme rather than assumed.
- "Surface finish SPI B-1 on faces marked; balance per SPI C-1; physical plaque approved by both parties." A grade plus a plaque, because the grade alone is not a specification.
- "Flash max 0.05 mm at the parting line; no flash permitted in the sealing area." Flash is the most common cause of a rejected first shipment, and it is almost never specified.
- "Steel-safe allowance to be stated for all critical dimensions before cutting." This is the line that turns a tolerance into a plan.
What those lines have in common is that they describe a decision rather than a wish. A drawing built this way is also cheaper to quote: the toolmaker can see immediately which dimensions drive the process, instead of protecting every one of them and pricing the risk into the total.
For the wider picture of how a drawing becomes a tool, the process is set out in the plastic injection molding guide; for how the finished tool is proven against these numbers, see mold trial approval. And if the part is a new design going into a small first batch, the tolerances you can hold with an aluminum tool are a narrower set — that trade-off is covered in low volume injection molding.
Frequently asked questions
What tolerance can injection molding realistically hold?
For an unfilled or lightly filled resin in a well-built tool, ±0.10 mm is routine, ±0.05 mm is normal precision work, and ±0.03 mm is achievable on dimensions that sit inside one half of the mold. Beyond that, the limit stops being the tool and becomes the resin: shrinkage varies within its own datasheet range by more than the tolerance you are asking for. Anything below about ±0.02 mm should be treated as a special project — few cavities, climate control, a dedicated molder and a second trial — not as a note on a drawing.
Why does my part measure differently at the molder than at my own QC?
Almost always one of four things, in order of likelihood: the part was measured at a different age (molded parts keep shrinking, and polyamides grow as they absorb moisture), at a different temperature, against a different datum, or with an instrument too coarse for the tolerance. A part measured an hour after ejection and the same part measured after a week in a warehouse can differ by more than a ±0.05 mm band on a large dimension. Agree the settling time, the temperature and the datum scheme in writing, and most of these disputes disappear without anyone changing the tool.
Should I specify SPI or VDI surface finish?
Use whichever scale your suppliers quote in, but never rely on the number alone. SPI defines the finish by the abrasive that produced it, VDI defines it by a photographic reference, and there is no exact conversion between them — the same VDI number etched to different depths on different steels will not look the same. The specification that actually holds is a grade plus an approved physical plaque molded in the production resin. If appearance matters, the plaque is the contract and the number is only shorthand.
Is ±0.05 mm reasonable on a 200 mm part?
It depends entirely on which dimension. If it is a feature cut into one half and measured in one direction, ±0.05 mm at 200 mm is demanding but real — it needs grinding and a controlled room, and it will cost meaningfully more. If it spans the parting line, or crosses a slider, ±0.05 mm is not a tolerance but a hope: those dimensions are limited by shut-off condition and fit clearance, not by cutting accuracy. And if the resin is a glass-filled grade, the flow and cross-flow directions shrink by different amounts, so a single ±0.05 on a 200 mm dimension is asking the part to be more isotropic than the material allows.
Does a tighter tolerance produce a better part?
No. It produces a more expensive part, and often a less reliable one, because a tool built to a very narrow band has a narrow process window and drifts when the shop floor temperature changes with the season. What makes a part good is that the dimensions carrying function are controlled and the dimensions carrying nothing are free. A drawing that tolerances everything tightly spends the budget nowhere in particular and buys rejects later.
What does "steel safe" mean and why does it matter?
Steel safe means cutting the tool so that material removal moves each dimension in the direction you may need to correct. An outside dimension gets smaller when you remove cavity steel, so cut it slightly small and you can always enlarge the part. A hole gets smaller when you remove core steel, so cut the core slightly large and you can always shrink the hole. It matters because a mold can only lose steel, never gain it: a tool delivered with every dimension at dead center has no correction path, and the second trial becomes a new tool rather than an adjustment.
