Plastic Rules, Draft and Wall Thickness

Overview#

Injection molded parts have a short list of non-negotiable rules: roughly uniform wall thickness, draft on every face parallel to the pull direction, generous radii, and ribs and bosses sized relative to the wall. Fusion's Plastic tab (part of the Design Extension, a paid add-on) turns these into data. A plastic rule stores material, thickness, draft angle and nominal radius, and commands such as Extrude, Rib, Web, Boss, Snap Fit, Shell and Draft read from that rule. Design Advice then warns when geometry breaks molding guidance.

Note: Autodesk lists Boss, Snap Fit, Rib and Web draft/fillet options and Plastic Rules as Design Extension tools (Plastic Design Tools). Without the extension the commands are locked; you can still model with standard Shell, Draft, Rib and Web in the Solid tab. Autodesk's help pages for Boss, Rest, Lip, Snap Fit and the plastic-rule topics are each marked as Design Extension features. Rib and Web are in the Solid tab and available without the extension; only their draft and fillet options are marked as extension features.

Where to find it#

• Design workspace > Plastic tab > Setup panel: Assign Plastic Rule and Manage Plastic Rules.
• Draft: Solid > Modify > Draft. Shell: Solid > Modify > Shell.
• Design Advice: configured in the plastic rule (see below). Plastic rules can be created, edited and saved to a library for reuse across designs, per Autodesk's extension page.

Step by step#

1. Open Plastic > Setup > Manage Plastic Rules. Create a rule, for example ABS_2.5mm.
2. Set Physical material (for example ABS or polycarbonate), Thickness (nominal wall, such as 2.5 mm), Draft angle (1 to 2 degrees is typical for smooth surfaces), and Nominal radius.
3. Set the Design Advice values: thickness range, thickness variation, minimum draft angle and the knife edge threshold.
4. Save the rule to the library if you want to reuse it.
5. Choose Assign Plastic Rule, select the component, and pick the rule. Do this before creating Shell or Thicken features so they inherit its values.
6. Model the outer shape. Add draft with Draft relative to the pull direction (the direction the mold opens). Use the rule's draft parameter rather than typing the number.
7. Shell inward with the rule thickness. Add fillets using the nominal radius.
8. Run Design Advice (Inspect or the plastic analysis shown after assigning a rule; verify the command location in your version) and read the flagged faces.

Options reference#

Tips and pitfalls#

Tip: Wall thickness drives cycle time (cooling time scales roughly with the square of thickness). Thinner uniform walls are cheaper, as long as the resin can fill them.

Tip: Thicker sections cause sink marks and voids. Keep adjoining features (ribs, bosses) to a fraction of the wall, typically 40 to 60 percent of it for ribs on cosmetic surfaces.

Warning: Draft must be applied relative to the correct pull direction. A part with side actions or undercuts needs more than one pull direction; plan the parting line first.

Warning: Draft after fillet can fail. Apply draft first, then add radii, or let the plastic rule do both in order.

Tip: Use Inspect > Draft Analysis (in the Inspect panel) to colour faces by draft angle against the pull direction. Red or inconsistent colours reveal missing draft.

Warning: Rule values are guidelines. The resin supplier's data sheet and your molder's DFM review override generic numbers.

What a plastic rule contains and how features use it#

A plastic rule is a bundle of manufacturing parameters assigned to a component. Autodesk describes rules as controlling plastic feature properties such as material and thickness automatically. The values flow into commands in three ways.

1. Defaults in dialogs. Draft angle, wall thickness and nominal radius pre-fill in Extrude, Shell, Thicken, Rib, Web, Boss, Snap Fit, Emboss and Draft. You can still override them per feature.
2. Parameters. The rule values are available to feature inputs, so changing the rule from 2.5 mm to 2.0 mm updates all features that use the rule thickness.
3. Advice. Design Advice compares geometry with the rule limits and flags faces that violate them.

Choosing values, with numbers#

These are common starting values for general-purpose parts. Always check the resin data sheet and the molder.

Texture needs extra draft: a common guide is about 1 degree extra for each 0.025 mm (0.001 in) of texture depth. A 0.05 mm texture therefore asks for about 2 degrees more than a polished surface, so 3 degrees in total. Treat this as a rule of thumb and confirm with the texture supplier.

Worked example: wall and rib budget#

A 2.5 mm nominal ABS wall. Ribs at 60 percent are 1.5 mm thick; with 0.5 degree draft per side, a rib 7.5 mm high (three times the wall) is 1.5 mm at the top and about 1.5 + 2 x 7.5 x tan(0.5 degrees) = 1.63 mm at its root. A boss with a 2.5 mm wall around an M3 thread-forming screw (about 2.5 mm pilot) has an outer diameter of about 2.5 + 2 x 2.5 = 7.5 mm, which is about three times the screw diameter, a little above the usual two to two and a half times; reduce the wall to 2 mm to bring the outer diameter to 6.5 mm and thin the boss wall to roughly the main wall.

Uniform wall thickness and Design Advice#

Wall thickness affects cost and quality. Cooling time grows roughly with the square of the wall, so reducing a 4 mm wall to 2.5 mm cuts cooling time by about 60 percent (since (2.5/4) squared is 0.39). Thick sections also cause sink marks and voids. The thickness range and variation values in the rule let Design Advice flag walls outside the band: a 2.5 mm nominal with a range of 1.5 to 3.5 mm will warn on a 5 mm pad. Fix by coring out the pad, or replace it with ribs.

When walls must change thickness, transition gradually. A common guide is a taper of about 3:1 (length to thickness change), so going from 3 mm to 2 mm needs about 3 mm of taper length. Sudden steps trap material and cause sink and flow lines.

Drafting properly#

1. Decide the pull direction (the direction the mould opens) and the parting line before drafting.
2. Draft faces parallel to the pull direction. Draft outside faces so the part is narrower at the cavity opening, and inside faces so the core releases.
3. Draft before filleting where possible, because filleting a drafted edge is more reliable than drafting a filleted one.
4. Verify with Inspect > Draft Analysis. Faces with insufficient draft show in a different colour from properly drafted faces.

Worked draft check#

A 40 mm tall wall with 1 degree draft leaves a difference of 40 x tan(1 degree) = 0.70 mm between top and bottom. With 0.5 degree it is only 0.35 mm, which on a textured surface may cause drag marks on ejection. For a 40 mm deep rectangular core with 1.5 degrees, the core's far end is 1.05 mm smaller per side than the root; plan the internal dimensions with this in mind.

Common failures and fixes#

Practice exercise#

Create a rule, apply it, and test every Design Advice threshold.

1. Create a plastic rule ABS_2.5mm with a 2.5 mm wall, a 1.5 degree draft and a 1.5 mm nominal radius. Set a thickness range of 1.5 to 3.5 mm.
2. Assign it to a new component. Model an 80 x 50 x 25 mm enclosure half. Add draft to the four outer walls relative to the pull direction (Z).
3. Run Inspect > Draft Analysis and confirm all walls pass at 1.5 degrees. Compute by hand that the 25 mm wall shifts by 25 x tan(1.5 degrees) = 0.65 mm top to bottom, and confirm with Measure.
4. Shell inward by the rule thickness, with the open face at the top. Add 1.5 mm radii to the inside corners.
5. Run Design Advice and read the result. Make one wall 5 mm thick (by adding a pad) and observe the warning, then core it out to fix it.
6. Change the rule thickness to 2.0 mm and note which features update.

Expected result: a clean enclosure half with no warnings, a measured draft shift near 0.65 mm over 25 mm, a warning on the 5 mm pad, and a clear list of the features that follow the rule thickness. If the Plastic tab is locked, repeat the exercise with Solid Shell and Draft and compute the same checks by hand.

Related#

• Boss, rib, web and rest
• Lip, groove and snap fit
• Design for manufacture