Plastic Body Panel Design for Injection Moulding

The problem

Electric two-wheelers use many large plastic panels, and their cost is dominated by tooling. A panel that has no draft, uneven walls or hidden undercuts either cannot be moulded or needs complex side actions that raise tool cost. Learning moulding rules in CAD lets a student design a panel that a toolmaker can quote without major redesign.

Objectives

• Model a side panel from a given styling surface with nominal wall thickness and pull direction.
• Add draft, ribs, mounting bosses and snap fits according to common moulding rules.
• Check draft and undercuts and define a parting line and core and cavity split.
• Optionally run a fill simulation to predict fill time, weld lines and sink.
• Document the panel with a drawing and a design-for-moulding checklist.

What you need

Key concepts

Draft

A taper on walls parallel to the mould opening direction so the part releases from the tool. Textured faces need more draft than polished ones.

Uniform wall thickness

Even walls cool at the same rate, avoiding sink marks, voids and warp. Thick sections are cored out rather than left solid.

Undercut

A feature that blocks the part from being pulled straight out of the mould. It needs a side action or lifter, which adds tooling cost.

Rib-to-wall ratio

Ribs are usually kept to roughly half to two-thirds of the wall thickness at the base to avoid sink marks on the visible face.

Step-by-step guide

1. 1

   Define the panel and its environment

   Pick an example rear side panel of a scooter, about 500 × 250 mm. Write requirements: material (for example a PP or ABS/PC moulding grade), a textured outer face, mounting to the frame at four points, two snap fits to a neighbouring panel and outdoor UV exposure. Set the pull direction, which is usually normal to the main visible face. Get shrinkage and recommended wall thickness from the material datasheet.

   Checkpoint: A one-page brief with material, pull direction, mounting scheme and a nominal wall thickness, for example 2.5 mm.

2. 2

   Build the outer surface

   Start from a given styling surface, an IGES or STEP export from Alias if available, or create a simple one with Boundary Surface and Lofted Surface from section sketches. Check curvature with Zebra Stripes and Curvature display so the surface is smooth before you thicken it. Trim the surface to the panel outline and extend edges where they will tuck under neighbouring panels.

   Checkpoint: A single trimmed outer surface with no gaps, smooth zebra stripes and the agreed outline.

3. 3

   Thicken and add the flange

   Use Thicken inwards to the nominal wall thickness. Add a return flange around the edge with a Swept Boss or an offset surface plus Thicken so the edge looks finished and stiff. Keep the flange the same thickness as the wall. Check minimum radius on inner corners so that Thicken does not fail and inside corners are at least half the wall thickness to avoid stress concentration.

   Checkpoint: A solid panel with uniform thickness, checked with section views at three locations.

4. 4

   Add draft

   Apply Draft to all walls parallel to the pull direction: an example of 1 degree on smooth faces and more on textured ones, following the texture supplier's guidance. Use Neutral Plane or Parting Line draft types as fits the geometry. Then run Draft Analysis with the pull direction and a minimum angle, and colour the model to show positive, negative and insufficient draft faces.

   Checkpoint: Draft Analysis shows no faces below the minimum angle except ones you have deliberately listed for a side action.

5. 5

   Add ribs, bosses and snap fits

   Add stiffening ribs on the inner face with the Rib feature, thickness about 60 per cent of the wall and with draft on both sides. Add four Mounting Boss features for self-tapping screws, sized for a screw manufacturer's recommendation and tied to the wall with gussets. Add Snap Hook features for the neighbouring panel and calculate their strain using a cantilever formula. Core out any thick junctions where a boss meets a rib.

   Checkpoint: Section checks show no wall thicker than about 1.3 times nominal at rib and boss roots.

6. 6

   Check undercuts

   Run Undercut Analysis with the pull direction to find faces that cannot be seen from either side of the mould. Snap hooks usually create undercuts. For each, decide whether to redesign (for example a through-window under the hook so the core can form it), accept a lifter, or change the pull direction. Record the decision and the likely tooling cost impact in words rather than numbers.

   Checkpoint: An undercut list with a decision for each one, and as few side actions as the function allows.

7. 7

   Create the parting line and split

   Use Parting Lines on the drafted model to find the boundary between core and cavity, add Shut-off Surfaces for through-holes and windows, and create a Parting Surface. Apply a Scale feature with the datasheet shrinkage before Tooling Split so the tool blocks are oversized correctly. Run Tooling Split to generate core and cavity bodies. This shows the panel can actually be moulded with the chosen pull direction.

   Checkpoint: Tooling Split creates separate core and cavity bodies without errors.

8. 8

   Run a fill study (optional)

   If SOLIDWORKS Plastics is licensed, mesh the panel with a shell or solid mesh, select the material from its database and place a gate at the thickest central region or along a hidden edge. Run a fill analysis and look at fill time, pressure at the end of fill, weld line locations and sink marks. Move the gate or add a second gate if weld lines fall on visible faces or near snap fits. Without the licence, sketch expected flow fronts by hand from the gate position.

   Checkpoint: Predicted weld lines avoid visible areas and snap hooks, or the hand flow sketch reasons through the same question.

9. 9

   Drawing, checklist and report

   Create a drawing with views of the outer and inner faces, sections through ribs and bosses, draft and texture notes, material and shrinkage, and general tolerances. Fill in a design-for-moulding checklist covering wall thickness, draft, ribs, bosses, undercuts, gates and weld lines. Report what you changed after each analysis and what a toolmaker would still need to decide. Include screenshots of the Draft Analysis, Undercut Analysis and Tooling Split results as evidence for each checklist item.

   Checkpoint: A drawing and checklist with every item addressed, and a list of before-and-after changes driven by analysis.

Testing & validation

• Section checks confirm uniform wall thickness within the stated ratio.
• Draft Analysis passes at the stated minimum angle.
• Undercuts are listed with a decision for each.
• Tooling Split completes, proving a viable parting line.
• Fill study or flow sketch places weld lines away from visible and loaded areas.

Expected results

A mouldable scooter body panel with uniform walls, draft, ribs, bosses and snap fits, an analysed parting line with core and cavity, optional fill results and a moulding checklist.

Take it further

• Compare two materials for warp and sink with SOLIDWORKS Plastics.
• Design the mating panel and check the gap and flush with the panel assembly.
• Print a scaled prototype to check snap-fit assembly.

Viva and review questions

Learn it at DIYguru

These DIYguru courses and programmes teach what this project needs.