Casting Part Design Principles: Draft Angles, Fillet Radii, Parting Lines, and Castability

Introduction

Casting is one of the oldest manufacturing processes, and designing parts that cast well requires internalizing a set of principles that are fundamentally different from those governing machined or sheet metal parts. The liquid metal filling a mold cavity, solidifying under thermal gradients, and shrinking as it cools is a complex physical process — and designs that ignore this complexity produce parts with porosity, cracks, misruns, and geometric distortion.

This article focuses on the four most critical design elements for cast parts: draft angles, fillet and corner radii, parting line selection, and general castability considerations. Whether you’re working with sand casting, die casting, or investment casting, the underlying principles are consistent, though the specific numerical requirements differ.

Draft Angles for Casting: Similar Logic, Different Numbers

Like injection molding, cast parts require draft on surfaces parallel to the mold opening (or pattern extraction) direction. The purpose is the same: allow the part to be removed from the mold without tearing. The required angles differ by process:

Draft requirements by process

• Sand casting (external surfaces): 1–3 degrees minimum. The rougher surface condition of sand molds requires more generous draft than smooth metal tooling. Typical design standard: 2 degrees.
• Sand casting (cores/internal surfaces): 3–5 degrees minimum. Cores experience the full shrinkage force of the surrounding metal and are more difficult to remove. Be generous with draft on core surfaces.
• Die casting (aluminum, zinc): 1–2 degrees for external surfaces, 2–3 degrees for internal surfaces. Die casting uses metal dies with smooth surfaces, allowing less draft than sand, but cavity pressure during injection requires reliable part release.
• Investment casting: 0–0.5 degrees is often achievable due to the expendable ceramic mold process. This is one of investment casting’s key advantages for complex geometry.

Draft direction and parting line relationship

Draft angle direction is always referenced to the mold opening direction. Features on the cope (top) half of a sand casting draft upward; features in the drag (bottom) half draft downward. This means the parting line location fundamentally determines where draft is required and in which direction — making parting line selection a prerequisite to draft analysis.

Fillet Radii and Corner Radii: Critical for Both Quality and Strength

Sharp internal corners are among the most common causes of casting defects. During solidification, metal at an internal sharp corner experiences triaxial tensile stress as it shrinks against the constraint of the surrounding solidifying metal. This stress can exceed the material’s strength while it is still partially solid, causing hot tearing — a particularly destructive defect that creates cracks in the casting.

Fillet radius guidelines

• Minimum internal fillet radius: At internal corners (where two walls meet at a concave angle), use a minimum radius of 3–5mm, or approximately 0.5× the thicker adjacent wall section, whichever is larger. In practice, be more generous where possible — larger fillets reduce stress concentration in service and reduce hot tearing risk in casting.
• External corners: Sharp external corners are generally acceptable in casting (they don’t create the same stress concentration as internal corners) and are often preferred to avoid flash and maintain dimensional accuracy at external edges. However, small chamfers or radii on external corners improve finished appearance.
• Radius uniformity: Avoid abrupt transitions between sections. Where a thick section transitions to a thin one, use a gradual taper or blending radius rather than a step change. Abrupt thickness transitions create shrinkage concentration that leads to porosity.

Parting Line Selection

The parting line is the boundary between the two (or more) mold halves. Its selection affects everything: draft requirements, core complexity, dimensional accuracy of critical features, and flash location. Parting line selection is a collaboration between designer and foundry — but designers who understand the principles produce better outcomes from that conversation.

Principles for parting line placement

• Place the parting line at the largest cross-section: For simple geometries, placing the parting line at the widest point minimizes the volume of material in each half and simplifies draft requirements.
• Avoid parting through cosmetic or precision surfaces: The parting line produces a witness mark (flash line) on the casting surface that requires grinding or machining to remove. Place it on surfaces that will be machined anyway, or on hidden/non-cosmetic faces.
• Minimize cores: Features that cannot be drafted from the parting line require cores — separate sand or metal inserts that create internal cavities or recesses. Cores add cost, tooling complexity, and potential for core shift (dimensional error from core movement during casting). Simplify the parting line to eliminate core requirements where possible.
• Consider machining datums: If the casting has features that will be machined post-cast, the parting line should not pass through the machining datum surfaces. Parting line location introduces a dimensional discontinuity; locating machining references there creates tolerance problems.

Wall Thickness and Section Design for Castability

Unlike injection molding where uniform wall thickness is paramount, casting can accommodate more variation in section thickness — but still benefits from thoughtful management of how sections transition.

Section thickness rules for casting

• Minimum wall thickness: Sand casting: 4–6mm for iron and steel, 3–4mm for aluminum. Die casting: 1.5–3mm for aluminum. These minimums ensure the metal can flow to fill thin sections before freezing.
• Avoid isolated thick sections: Isolated thick sections are the last to solidify, and without a feeder (riser) to supply liquid metal as the section contracts, they develop shrinkage porosity at their center. Either provide an adequate riser or redesign to core out the section.
• Section transitions: Where section thickness must change, use tapered transitions over a length of at least 3–4× the thickness change. Abrupt steps concentrate shrinkage stress.
• “Hot spots” analysis: Any enclosed volume of metal surrounded by thinner sections will solidify last and is a hot spot candidate. Simulation tools can identify hot spots early; experienced foundry engineers can spot them from geometry inspection.

Key Casting Design Reference

Post-Cast Machining Considerations

Most castings require post-cast machining for precision features: bores, mating surfaces, threaded holes. Design for this from the start:

• Add machining stock (2–5mm per surface, more for large sand castings with significant distortion potential) on surfaces that will be finish-machined
• Identify and protect machining datum surfaces from the parting line flash and casting features that could compromise their use as references
• Design machining datum surfaces that are accessible for fixturing — a boss or pad specifically intended as a datum surface rather than an incidental casting face
• For threaded features, consider whether to cast the thread form (only practical for coarse threads in ductile materials) or machine tap after casting — machined threads are almost always more accurate and reliable

FAQ

Q: How do I handle undercuts in a casting design — features that cannot be drafted from the main parting line?
A: Undercuts require either cores (which create the undercut feature independently from the main cavity), collapsible cores, or side-actions in the mold. Each option adds tooling cost and complexity. Before accepting an undercut, ask whether the functional requirement can be achieved by redesigning the feature to eliminate it — for example, replacing an internal groove with an external groove accessible from the parting line, or splitting the part at a different location. If the undercut is essential, involve the foundry in the core or side-action design early.

Q: When should I specify casting versus machining from solid for a complex part?
A: Casting is generally preferred when: the part has complex internal geometry (passages, cavities) that cannot be produced economically by machining; the production volume is high enough to amortize tooling cost; and near-net-shape material efficiency matters (reducing material waste compared to machining from solid). Machining from solid is preferred for: small quantities where tooling cost is prohibitive; parts with very tight tolerances throughout; materials that cast poorly; and geometries where casting complexity would require extensive coring that makes the casting cost comparable to or higher than machining cost.

Q: What is the significance of casting simulation, and when should I insist on it?
A: Casting simulation predicts fill pattern, solidification sequence, hot spot locations, and shrinkage porosity risk before the mold is built. For complex, high-value, or safety-critical castings, simulation is standard practice. For simple, low-risk castings with well-established geometry, foundry experience is often sufficient. The threshold for requiring simulation: any casting where internal porosity would compromise function (pressure-containing parts, structural castings), any first-article casting with tight tolerances, and any geometry with complex sections where hot spots are not obvious from visual inspection.