Injection moulding calculator

Work out the four numbers a plastic part needs before the mould is cut. Clamp force: the machine tonnage for your projected area and cavity pressure. Cooling time: how long your wall takes to reach ejection temperature. Cavity size: the mould dimension for the resin's shrinkage. Draft: the angle and the wall it leaves. Free, no sign-up, runs in your browser.

The cooling formulas are the ones BASF and Covestro print in their processing guides, and Covestro's worked examples are reproduced below. Material presets come from resin makers' datasheets. For the design rules behind ribs, bosses and wall thickness, see the DFM checklist.

BASF and Covestro cooling equations · ASTM D955 / ISO 294-4 shrinkage · checked against an independent solution (832 checks at build) · Updated 22 Nov 2026

Pick a material to load its datasheet values, or type your own in any box.

Projected area of one cavity

Tool and pressure

Projected area is the part's shadow on the parting plane, looking along the mould opening. Through-holes formed by a shut-off (steel on steel) carry no melt pressure, so they come off. Blind holes and the runner do carry pressure.

Clamp force with margin345.6 kN288.0 kN before the 20% margin
Metric tonnes-force35.2 t29.4 t before margin
US tons (2,000 lbf)38.832.4 before margin
  • Projected area per shot 72.00 cm² = 1 × 72.00 cm².
Cavity pressureClamp forceTonnes-forceUS tons

How do you calculate clamp force for injection moulding?

The melt pushes the mould halves apart with the cavity pressure acting over the projected area. The machine's clamp has to hold more than that, or the mould opens a little and the part flashes. Add up the projected area of every cavity and the runner, and multiply by the pressure:

Skill-Lync's plastic and sheet metal design guide uses this example. A 120 × 60 mm switch bezel has 72.0 cm² of projected area. At an assumed 400 bar in the cavity that is 288.0 kN, or 29.4 tonnes-force (32.4 US tons). A 20% margin takes it to 35.2 t, so a 35-tonne machine. A two-cavity tool needs 58.7 t, 59 tonnes, before the margin. The calculator gives these exactly.

Two published examples check the same formula. Keyence's: 400 kgf/cm² on a 16.0 cm² cavity and a 5.0 cm² runner, printed as 8.4 tf; the calculator gives 8.40 tf. RJG's: a 4.6 × 4.6 in lid in an 8-cavity hot-runner tool at 3 US tons per square inch, printed as 507.84 tons; the calculator gives 507.84 US tons. Both are presets above.

What cavity pressure to use. This is the weak point of every tonnage estimate. Keyence says the cavity pressure is generally about 300 to 500 kgf/cm² (294 to 490 bar). RJG quotes tonnage factors of 2 to 10 US tons per square inch (276 to 1379 bar) and recommends 3 (414 bar) as a starting point. SPE's Plastics Engineering gives 2 to 8 by material, 2 to 3 for polypropylene, and 400 bar as a guide value when there is no data. Thin walls, long flow paths and stiff resins push it up. DuPont lists wall thickness, flow length, melt temperature and fill speed among the factors that set the pressure. For a real tool the number comes from a fill simulation (Moldflow, Moldex3D) or from the resin maker's spiral flow-length charts, which this calculator does not try to read.

The margin is a choice. Autodesk's Moldflow help suggests keeping the clamp force below about 80% of the machine's limit, which means a machine 25% above the calculated force. aPriori's cost model multiplies by 1.1. The 20% default is the course example's. Sliding cores and side actions add their own loads, so they need more.

ExampleInputsPrintedThis calculator
Skill-Lync switch bezel72 cm², 400 bar, 1 cavity, +20%288 kN, 29.4 t, 35 t288.0 kN, 29.4 t, 35.2 t
Same, two cavities2 × 72 cm², 400 bar59 t58.7 t
Keyence16.0 + 5.0 cm², 400 kgf/cm²8.4 tf8.40 tf (82.4 kN)
RJG lid8 × 21.16 in², 3 tons/in²507.84 tons507.84 US tons (460.7 t)

How long does a moulded part take to cool?

Cooling is usually the longest part of the cycle. ExxonMobil's moulding guide puts it at 60 to 80% of the cycle time, and Autodesk's Moldflow help says it usually takes 80%. The part can come out once it is stiff enough not to deform on the ejector pins: when its centre (or its average) drops to the ejection temperature TE.

BASF and Covestro both print the same estimate for a plate of wall thickness s, cooled from both faces by a mould at TW:

For a long cylinder of diameter D (a rod, a sprue or a runner) the constant comes from the first root of the Bessel function J₀, 2.4048. BASF and Covestro print it rounded as 23.14; worked out it is 23.133. The difference is 0.03%.

All three are the first term of the exact series solution for heat conduction. For the centre of a plate the full series is:

After a short time the later terms die out, and keeping only the first one and solving for t gives the formula. Covestro warns that the shortcut is poor early in cooling and asks for a check of the Fourier number:

The calculator does better than the check. It also sums the full series and solves it for the time, so you see how far the formula is off. For the walls and presets here, the centreline formula is within 0.05% of the full series. The mean-temperature version is the weaker one: 1.1% short for the PA66 preset, and far off when the ejection temperature is close to the melt temperature (57% short with TE = 200 °C, TM = 240 °C).

Halve the wall, quarter the cooling. The time grows with s². The 3 mm wall above takes 18.0 s; at 1.5 mm it takes 4.5 s. This is why moulders fight thick sections, and why a thick boss or a rib-wall junction sets the cycle time for the whole part.

What a_eff is. The effective thermal diffusivity is k/(ρcp) for the cooling plastic. BASF says the value is chosen so that the computed cooling time matches moulding trials, and that it only describes cooling close to the freezing point. Use the datasheet value, and do not mix it with diffusivities from other tables.

Worked examples: Covestro's ABS panel and nomograms

Covestro's guide Process Variables as Production Cost Factors works a 3 mm ABS panel with aeff = 0.08 mm²/s, melt at 240 °C and a mould wall at 50 °C. Its guide Optimized Mold Temperature Control reads two more off a nomogram. The calculator against the printed answers:

ExampleInputsPrintedFormulaFull series
ABS panel, eject at 100 °Cs 3 mm, a 0.08, 240/50/100 °C18 s17.97 s17.97 s
ABS panel, eject at 80 °Cs 3 mm, a 0.08, 240/50/80 °C24 s23.79 s23.79 s
ABS panel, 30 °C wall at the edges 3 mm, a 0.08, 240/30/100 °C15 s15.28 s15.28 s
Nomogram, plate (mean)s 2 mm, a 0.085, 250/25/70 °C6.6 s6.67 s6.67 s
Nomogram, rod R = 2 mmD 4 mm, a 0.085, 240/20/80 °C14 s14.41 s14.40 s

Covestro prints the steps of the first example as 11.3986 × 1.5766 = 18 s; the calculator's s²/(π²a) is 11.3986 and the log term 1.5766. Dropping the ejection temperature by 20 °C adds 32% to the cooling time; Covestro says "some 30%". The nomogram answers are read off a chart, so they match to two figures.

How do you calculate the mould cavity size from shrinkage?

Plastic shrinks as it cools in the mould and for some time after. ASTM D955 and ISO 294-4 measure that shrinkage against the mould, so the definition and its inverse are:

Toolmakers often use L(1 + S). It is a little short, by L S²/(1 − S): 0.003 mm on a 100 mm dimension at 0.5%, and 0.041 mm at 2%. That is small next to the spread of the shrinkage itself.

The spread is the real problem. A datasheet gives a range, and many resins shrink differently along and across the flow (glass-filled grades most of all). In a fixed tool, a shrinkage range of Slow to Shigh moves the part by the cavity size × (Shigh − Slow). The calculator shows this band for every dimension: it is tolerance the moulding process uses before any machining error.

Changing the resin. The Skill-Lync course page's example: a 100 mm part, a tool cut for ABS at about 0.5% shrinkage (100.50 mm cavity), moulded in polypropylene at about 1.5%. The part comes out 98.99 mm, 1.0 mm short. Switching resin needs a new cavity or a re-cut, not a process tweak.

Material (grade)Melt (°C)Mould (°C)Ejection (°C)a_eff (mm²/s)Shrinkage flow / cross (%)
ABS (INEOS Styrolution Terluran GP-35)220–26030–80100 (Covestro example)0.080.4–0.7 / 0.4–0.7
PP homopolymer (Borealis HF955MO)220–26015–60--1–2 / 1–2
HDPE (Borealis BorPure MB7541)190–25010–40--1–2 / 1–2
PC (Covestro Makrolon 2405)280–32080–120--0.65 / 0.7
PC/ABS (Covestro Bayblend T65 XF)240–27070–90--0.5–0.7 / 0.5–0.7
PA66 (dry) (Celanese (DuPont) Zytel 101L NC010)280–30050–901900.051.4 / 1.4
POM copolymer (Celanese Hostaform C 9021)190–21080–1201400.04852 / 1.9
PBT-GF30 (BASF Ultradur B 4300 G6 HR)250–27560–100--0.5 / 1.3

Values as printed on each maker's datasheet for one named grade, read 22 Nov 2026; other grades of the same resin differ, so use your grade's sheet. Ejection temperature and aeff are given only where the maker prints them (Celanese, for PA66 and POM); the ABS pair are the inputs of Covestro's worked example. Where a datasheet gives one shrinkage range, it is used for both directions. Leave a box blank and the calculator asks for it rather than guess.

What draft angle does an injection-moulded part need?

Every face parallel to the direction the mould opens needs a small angle, the draft, so the part releases without dragging on the steel. Draft is measured per side. Over a depth h it moves the face by h tan θ, so a box or boss drafted on both sides is 2h tan θ narrower at the bottom:

The default wall is 40 mm deep with 1° on the cavity side: each face moves 0.698 mm, and the 100 mm outside dimension becomes 98.60 mm at the bottom. When the core side has more draft than the cavity side, the wall gets thicker towards the bottom:

With 1.5° on the core, the 2.5 mm wall is 2.85 mm at the bottom. Over a deep wall that adds mass and cooling time, which is why both faces usually get the same draft.

How much draft. For smooth faces, DuPont's Zytel moulding guide says 0.5° to 1° per side is usually enough, and softer, more elastic resins may need up to 2°. Protolabs strongly advises at least 0.5° on all vertical faces, says 1° to 2° works well in most cases, and asks for 3° on shut-offs, where steel slides on steel. DuPont's design guide allows less on shallow parts in its own resins, from 0 to ½° under 25 mm deep.

Textured faces need much more, and the sources disagree. Texture is a pattern of small undercuts. Mold-Tech, the texturing company, wrote in 2020 that the "typical 1.5 degrees of draft per 0.001″ / 25 µm of texture depth is no longer a valid guideline" and now asks for 1° per 12.5 to 15 µm. DuPont's design guide and Machinery's Handbook add 1° per 0.025 mm. The calculator shows all three for the texture depth you enter:

Texture depthMold-Tech (2020): 1° per 12.5–15 µmDuPont / Machinery's Handbook: 0.5° + 1° per 0.025 mmOlder rule of thumb: 1.5° per 0.025 mm
0.025 mm1.67–2.00°1.50°1.50°
0.05 mm3.33–4.00°2.50°3.00°
0.1 mm6.67–8.00°4.50°6.00°

These are for faces the part shrinks away from, the cavity side. Mold-Tech says faces it shrinks onto, such as a core, need 2 to 3 times as much. Ask your texture supplier for the figure for the pattern you choose; the rules are only a first estimate.

Checking a CATIA draft analysis. A draft analysis colours each face by its angle to the pull direction against a minimum you set. The same number from a drawing or a measured part: top 100 mm, bottom 98.6 mm, 40 mm deep gives 1.00° per side. Skill-Lync's blog on draft analysis in CATIA walks through the workbench.

What this calculator does not cover

  • Filling and packing. Injection pressure, flow length and gate size need a flow simulation (Moldflow, Moldex3D) or the resin maker's flow-length charts.
  • Warpage. Different shrinkage along and across the flow, or between thick and thin areas, bends the part. Simulation predicts it; the shrinkage tab only sizes dimensions.
  • Cooling channel design. The cooling time assumes an even mould wall temperature. Channel spacing, coolant flow and hot spots decide whether you get it.
  • Rib, boss and wall rules. Thickness ratios for ribs, bosses and corners are in the DFM checklist.
Learn plastic and mould design

Draft analysis, core and cavity, ribs, bosses and dog houses are the plastic design challenges in Skill-Lync's CATIA and SOLIDWORKS courses, built on real trim parts such as a switch bezel and a door trim.

Frequently asked questions

How do you calculate the clamp force for injection moulding?

Multiply the projected area of the part (its shadow on the parting plane, holes that are shut off removed) by the cavity pressure and by the number of cavities, and add the runner. A 120 × 60 mm bezel at 400 bar needs 288.0 kN, 29.4 tonnes; with a 20% margin, a 35-tonne machine.

How is the cooling time of a moulded part calculated?

Resin makers such as BASF and Covestro use the first term of the heat conduction solution for a plate: t = s²/(π²a) · ln((4/π)(TM − TW)/(TE − TW)). It grows with the square of the wall thickness. Covestro's 3 mm ABS panel example gives 18.0 s, printed as 18 s.

Why does halving the wall thickness quarter the cooling time?

Heat has to travel from the middle of the wall to the steel, and conduction time grows with the square of that distance. The formula has s² in front, so a 3 mm wall that takes 18.0 s to cool takes 4.5 s at 1.5 mm. Thick walls cost cycle time more than anything else.

How do I size the mould cavity for shrinkage?

Divide the part dimension by (1 − S), where S is the moulding shrinkage as a fraction. ASTM D955 and ISO 294-4 measure shrinkage against the mould, so this is the exact inverse. L × (1 + S) is a close shortcut: on 100 mm at 0.5% it is 0.003 mm short.

What happens if I change the resin in an existing mould?

The part comes out a different size, because the tool was cut for the first resin's shrinkage. A 100 mm part in a tool cut for ABS at 0.5% comes out 99.0 mm when moulded in polypropylene at 1.5%, 1.0 mm short. Semi-crystalline resins shrink more than amorphous ones.

How do I check the draft angle from part dimensions?

Measure the width at the top and the bottom of the drafted face and its depth. The draft per side is arctan((top − bottom)/(2 × depth)) when both sides are drafted. For example, 100 mm at the top and 98.6 mm at 40 mm deep is 1.00° per side.

Related on Skill-Lync

Sources

Free counselling

From a draft analysis to a plastic design job.

Plastic trim and mould design are core skills for automotive and consumer-product design engineers, in CATIA V5 and SOLIDWORKS. A Skill-Lync counsellor can tell you which course fits where you are now.

Talk to a plastic design course counsellor

Free. We call you back, usually the same day.

By submitting you agree to our Terms and Privacy Policy.

Talk to a career counsellor

Talk to a career counsellor

Free 20-minute call. We'll map the right course to where you want to work.

By submitting you agree to our Terms and Privacy Policy.