---
type: process
name: "Thermoforming"
category: "Forming"
subcategory: "Plastics and Rubber"
materials: ["Plastic"]
tolerances: "±0.030 in (±0.75 mm) on vacuum-formed tool-side features; ±0.015 in (±0.4 mm) pressure formed and on CNC-trimmed edges. Non-tool-side dimensions carry all sheet thickness variation."
volumes: "50–50,000 parts per year for heavy gauge; thin-gauge roll-fed packaging runs into the millions"
lead_time: "1–2 weeks for prototype wood or epoxy tooling; 2–4 weeks for a production aluminum tool; days per run thereafter"
url: https://manufacturingprocesses.org/processes/forming/thermoforming
---

# Thermoforming

Thermoforming heats a plastic sheet until pliable and pulls or presses it over a single-sided mold, producing large thin-walled parts with low tooling cost.

- **Category**: [Forming](https://manufacturingprocesses.org/processes/forming.md)
- **Family**: Plastics and Rubber
- **Materials**: Plastic
- **Typical tolerances**: ±0.030 in (±0.75 mm) on vacuum-formed tool-side features; ±0.015 in (±0.4 mm) pressure formed and on CNC-trimmed edges. Non-tool-side dimensions carry all sheet thickness variation.
- **Surface finish**: The sheet's own surface (gloss, matte, or extruded grain) is reproduced on the non-tool side; the tool side takes the mold finish, and pressure forming can reproduce molded textures
- **Typical volumes**: 50–50,000 parts per year for heavy gauge; thin-gauge roll-fed packaging runs into the millions
- **Lead time**: 1–2 weeks for prototype wood or epoxy tooling; 2–4 weeks for a production aluminum tool; days per run thereafter

## Overview

Thermoforming heats a thermoplastic sheet until it is rubbery, then pulls or presses it over a single-sided mold and cools it in shape. Because the tool forms only one face and never sees melt pressure, tooling is a small fraction of an injection mold's cost and can be cut from aluminum in 2–4 weeks — which makes thermoforming the standard answer for large, thin-walled parts at hundreds to low tens of thousands per year.

It spans a wide range: 0.010 in blister packs and clamshells at one end; 0.250 in machine enclosures, vehicle interior panels, refrigerator liners, and shower trays at the other. Common materials are HIPS, ABS, HDPE, PP, PETG, PVC, polycarbonate, and acrylic.

The defining constraint is that the sheet thins as it stretches. A part drawn near its practical limit typically retains only 20–50% of the starting sheet gauge at the deepest corner, so you buy sheet by the thinnest section you need rather than the average.

## How it works

1. **Clamp and heat.** The sheet is clamped in a frame and passed under radiant heaters until it reaches its forming window: PETG 275–320 °F (135–160 °C), HIPS and ABS 300–360 °F (150–180 °C), PP 290–330 °F (145–165 °C), polycarbonate 375–400 °F (190–205 °C). Semi-crystalline materials such as PP have a narrow window and sag quickly; amorphous materials are far more forgiving.

2. **Pre-stretch (optional).** For deep draws, the sheet is bubble-blown or a mechanical plug pushes it partway into the cavity before vacuum is applied. Plug assist moves material into the deep regions before it touches cold tool surfaces and freezes.

3. **Form.** In vacuum forming, the tool evacuates the space beneath the sheet and atmospheric pressure — a hard ceiling of 14.7 psi (1 bar) — pushes the sheet onto the mold. Pressure forming adds compressed air on the back side at 40–100 psi (3–7 bar), giving four to seven times the forming force and with it sharper radii, crisper detail, and molded-in texture.

4. **Cool.** The sheet gives up heat to the aluminum tool, which is water-cooled on production tooling. Cooling dominates the cycle: roughly 20 seconds for thin-gauge packaging up to several minutes for a 0.250 in enclosure panel.

5. **Trim.** The formed sheet is removed and the part cut free. Thin-gauge packaging is trimmed with steel-rule dies in line; heavy-gauge parts go to a 3- or 5-axis CNC router, which is also where holes and cutouts are made.

### What does twin-sheet thermoforming add?

Two sheets are heated simultaneously, formed in opposing tool halves, and pressed together while still hot so they fuse at designed contact areas. The result is a hollow, double-walled part — pallets, fuel tanks, structural doors — with far higher stiffness per pound than a single-sheet part, at roughly double the tooling and cycle.

## Design guidelines

### Depth of draw

The ratio of draw depth to the smallest opening width is the governing number. Straight vacuum forming is comfortable up to about 1:1. Plug assist or pressure forming pushes it to 2:1 and beyond, but every increment costs wall thickness in the corners. Female (cavity) tools distribute material better on deep parts than male (plug) tools.

### Starting gauge and wall thinning

Order sheet by the thinnest section you need, not the average. In a hard draw the deepest corner retains 20–50% of the starting gauge — a 0.187 in (4.75 mm) sheet drawn aggressively can finish under 0.060 in (1.5 mm) at the corners. Uniform draw depth across the part is the single best defense.

### Draft

Male tools need 3° per side minimum, and 5° is safer, because the part shrinks onto the tool as it cools and has to be stripped off. Female cavities need only 1–2°, since the part shrinks away from the wall. Textured surfaces need more: budget roughly 1° extra per 0.001 in (0.025 mm) of texture depth, the same relationship tabulated for molded textures on [/charts/injection-molding-design-guidelines](/charts/injection-molding-design-guidelines).

### Radii

Minimum inside radius equal to the starting sheet thickness; 2–3× thickness is much better. Small radii are where the sheet stretches fastest and thins most, and on a vacuum-formed part they simply round over, because 1 bar cannot force the sheet into a tight corner. Pressure forming holds noticeably sharper corners for exactly this reason.

### Ribs, undercuts, and detail

Ribs must be wide and shallow — a formed sheet cannot fill a narrow slot. Undercuts require a moving core, a stripper ring, or enough material flexibility to snap the part off; each adds tool cost. Molded-in text and logos are practical in pressure forming and marginal in vacuum forming.

### Tolerances and trimming

Tool-side features hold roughly ±0.030 in (±0.75 mm) in vacuum forming and ±0.015 in (±0.4 mm) in pressure forming. The non-tool side carries all the thickness variation, so never dimension across the sheet. Trimmed edges and hole positions come from the CNC trim fixture and hold about ±0.015 in (±0.4 mm) — put locating features there rather than on formed geometry.

| Feature | Recommended | Limit | Why |
| --- | --- | --- | --- |
| Depth-to-width ratio | ≤ 1:1 vacuum forming | 2:1+ with plug assist | Deeper draws thin the corners past usable wall |
| Draft, male tool | 5° per side | 3° per side | Part shrinks onto the tool and must strip off |
| Draft, female tool | 2° per side | 1° per side | Part shrinks away from the cavity |
| Inside radius | 2–3 × sheet thickness | 1 × sheet thickness | Corners stretch most; 1 bar cannot fill sharp detail |
| Formed wall retention | 50% of starting gauge | 20% at the deepest corner | Sets the sheet gauge you have to buy |
| Forming pressure | 14.7 psi (1 bar) vacuum | 40–100 psi (3–7 bar) pressure forming | More pressure buys detail and sharper radii |
| Tolerance, tool side | ±0.030 in (±0.75 mm) vacuum | ±0.015 in (±0.4 mm) pressure | The non-tool side absorbs all thickness variation |

## Variants

- Vacuum Forming
- Pressure Forming
- Plug-assisted Forming
- Twin Sheet Thermoforming

## Cost drivers

The trade against injection molding is straightforward. Thermoform tooling is a single-sided aluminum form — wood or filled epoxy for prototypes — that costs a small fraction of a two-plate injection mold and arrives in 2–4 weeks. Per-part cost is higher, because you buy extruded sheet, throw away the trim skeleton, and run a longer cycle.

Volume breakpoints:

- Under 50 parts: wood or epoxy prototype tooling, hand trim.
- 50–5,000: machined aluminum single-cavity tool with CNC trim — the classic heavy-gauge sweet spot.
- 5,000–50,000: temperature-controlled cast aluminum tool, pressure forming, dedicated trim fixture.
- Above roughly 50,000 parts a year for a small part, injection molding usually wins on unit cost despite the tooling.

Cost reduction:

1. **Even out the draw depth.** One deep pocket forces you to buy heavy sheet for the entire panel. Redistributing depth lets you drop a gauge, which is a direct material saving on every part.
2. **Nest parts on the sheet.** The trim skeleton is pure scrap on virgin material; multi-up tools and tight nesting cut it substantially, and most thermoformers regrind and blend it back in house.
3. **Choose vacuum over pressure forming when cosmetics allow.** Pressure-forming tools are pressure vessels with a matched top half and cost significantly more.
4. **Put tight tolerances on trimmed features.** CNC-trimmed holes and edges hold about ±0.015 in (±0.4 mm); formed geometry does not.
5. **Use twin-sheet only where stiffness demands it.** It roughly doubles both tooling and cycle, but it replaces an assembly of two formed halves plus fasteners.

## FAQ

### How deep can you thermoform a part?

Straight vacuum forming handles a depth-to-minimum-width ratio of about 1:1 comfortably. Plug assist and pressure forming push that to 2:1 and beyond, but every increment thins the corners further. Female cavity tools distribute material better than male plug tools on deep parts.

### How much does a thermoformed part thin out?

In a hard draw the deepest corner typically retains only 20–50% of the starting sheet gauge. Specify sheet by the thinnest section your part needs, not the average — a 0.187 in (4.75 mm) sheet drawn aggressively can finish under 0.060 in (1.5 mm) in the corners.

### What is the difference between vacuum forming and pressure forming?

Vacuum forming relies on atmospheric pressure alone, a hard ceiling of 14.7 psi (1 bar). Pressure forming adds 40–100 psi (3–7 bar) of compressed air behind the sheet, giving four to seven times the forming force. That buys sharper radii, molded-in texture and lettering, and roughly double the dimensional precision, at higher tooling cost.

### What draft angle does thermoforming need?

Male (plug) tools need at least 3° per side and preferably 5°, because the cooling part shrinks onto the tool and must be stripped off. Female (cavity) tools need only 1–2°, since the part pulls away from the wall. Add roughly 1° per 0.001 in (0.025 mm) of texture depth on textured surfaces.

### When is thermoforming cheaper than injection molding?

Below roughly 5,000–50,000 parts a year, and especially for large, thin-walled parts. Thermoform tooling is single-sided aluminum at a small fraction of an injection mold's cost and arrives in 2–4 weeks. Above that volume the higher per-part cost of sheet and trim scrap usually tips the balance back to injection molding.

### What tolerance can thermoforming hold?

About ±0.030 in (±0.75 mm) on vacuum-formed tool-side features and ±0.015 in (±0.4 mm) with pressure forming. CNC-trimmed edges and holes also hold about ±0.015 in (±0.4 mm), so locating features should be trimmed rather than formed.

### What is twin-sheet thermoforming used for?

Hollow, double-walled parts such as pallets, fuel tanks, and structural doors. Two sheets are formed in opposing tool halves and pressed together while hot so they fuse at designed contact areas, giving much higher stiffness per pound than a single sheet at roughly double the tooling and cycle time.

## Alternative processes

- [Injection Molding](https://manufacturingprocesses.org/processes/forming/injection-molding.md): Injection molding forces molten thermoplastic into a steel mold under high pressure, producing high-volume identical plastic parts.
- [Rotation Molding](https://manufacturingprocesses.org/processes/forming/rotation-molding.md): Rotational molding tumbles powdered polymer inside a heated mold on two axes so it fuses into a seamless, stress-free hollow part with a uniform wall.
- [Reaction Injection Molding](https://manufacturingprocesses.org/processes/forming/reaction-injection-molding.md): Reaction injection molding mixes two liquid reactants that polymerize inside a low-pressure mold, producing large tough polyurethane parts on light tooling.
- [Blow Molding](https://manufacturingprocesses.org/processes/forming/blow-molding.md): Blow molding inflates a heated plastic tube or preform against the walls of a mold with compressed air, producing hollow one-piece containers and tanks.

## Related processes

- [Vacuum Casting (Urethane Casting)](https://manufacturingprocesses.org/processes/forming/vacuum-casting.md): Vacuum casting, known in the US as urethane casting, pours polyurethane resin into a silicone mold under vacuum to copy a master pattern for short runs.
- [Blow Molding](https://manufacturingprocesses.org/processes/forming/blow-molding.md): Blow molding inflates a heated plastic tube or preform against the walls of a mold with compressed air, producing hollow one-piece containers and tanks.
- [Plastic Extrusion](https://manufacturingprocesses.org/processes/forming/plastic-extrusion.md): Plastic extrusion pushes molten polymer through a shaped die and cools it, producing continuous profile, sheet, pipe or film of constant cross-section.
- [Rotation Molding](https://manufacturingprocesses.org/processes/forming/rotation-molding.md): Rotational molding tumbles powdered polymer inside a heated mold on two axes so it fuses into a seamless, stress-free hollow part with a uniform wall.
- [Die Cutting](https://manufacturingprocesses.org/processes/cutting/die-cutting.md): Die cutting presses a shaped steel rule or rotary die through sheet stock, cutting flat outlines in paper, board, foam, film and textile.

---

*Source: [Manufacturing Processes](https://manufacturingprocesses.org/processes/forming/thermoforming)*

*Last updated: August 11, 2026*