SpaceClaim Model Preparation

2.1  Importing CAD

SpaceClaim accepts STEP, IGES, Parasolid, ACIS, and native formats from major CAD systems through available translators. STEP is the preferred neutral format — it preserves topology more reliably than IGES and handles assembly structure better. Export as STEP AP214, verify units before import, and check the result immediately.

Automatic healing runs on import, but it is not complete cleaning. After any import, verify: body count matches the source assembly, the Interference Check reports no overlapping bodies, and mating faces are actually touching rather than separated by a small gap.

STEP from a complex multi-body assembly does not guarantee correct dimensions or correct part-to-part relationships. Tolerance accumulation, unit conversion rounding, and missing assembly constraints are common. These problems are invisible visually but cause immediate mesh failures or silently wrong results.

When imported geometry is unreliable, building the simulation model in SpaceClaim from scratch is faster than repairing it. For simple parts with clean CAD history, import is fine. For complex assemblies with tight tolerances or critical mating surfaces, build what you need directly. A cast-aluminium heatsink, for example, often imports cleanly at the fin surfaces but has a 0.05 mm gap at the fin-to-base junction that is invisible visually and only surfaces when the mesher tries to create conformal elements across it.

2.2  Identifying Mesh-Hostile Geometry

Walk the geometry in SpaceClaim before opening the mesher. The goal is a single repair pass, not an iterative repair-mesh-fail-repair loop.

The most common mesh-hostile features: thin slivers (faces with extreme length-to-width ratio), faces smaller than the target element size, edges shorter than the target element size, near-tangent surfaces (two faces meeting at a shallow angle), gaps between mating bodies, and re-entrant corners with included angles below approximately 20°.

SpaceClaim tools for geometry inspection: Check Geometry (Design tab → Repair → Check Geometry) identifies face errors, open edges, and self-intersections.^[1] Measure (right-click any face or edge) returns area, length, and angles. Interference Check finds overlapping bodies.

Check Geometry reports geometric errors but does not find all mesh-hostile features. Small faces and short edges only appear as mesh warnings or failures, not as Check Geometry errors. Use mesh quality metrics as a feedback loop: after the first mesh, go back to SpaceClaim for features that drove poor quality — not just outright failures.

2.3  Defeaturing for Structural Analysis

Before removing anything, determine the load path. Where are the constraints? Where are the loads? Where are the expected stress concentrations? Features in high-gradient regions must be preserved or carefully assessed. Features remote from the load path and below the structural scale of interest can be removed.

Rules of thumb: holes smaller than 10% of the minimum structural dimension in a low-stress region can be suppressed. Fillets and chamfers smaller than 1/10 of the smallest expected stress feature do not affect results. Decorative features (embossed text, cosmetic knurling) can always be removed. Fastener hardware can typically be replaced with bonded contact at the fastener footprint.

The threshold question: if this feature is removed, does the stress result at the locations of interest change by more than the acceptable error? If the answer is no for a realistic load magnitude, remove it. The answer requires knowing the load path — you cannot make this judgment without it.

2.4  Defeaturing for Thermal and Icepak Analysis

Identify the thermal model requirements before modifying geometry. Which components are heat sources? What is the fluid path? Which surfaces transfer heat by convection? Which interfaces transfer heat by conduction? Features outside the heat path can be simplified aggressively. Thermal interface surfaces — component footprints, TIM layers, heatsink contact — must be preserved exactly.

Icepak requires an explicit fluid volume. If air carries heat in the enclosure, that air must exist as a geometry body assigned air material. Create fluid volumes using SpaceClaim's Fill tool (Design → Fill), which creates a solid body from an enclosed region. Do not create fluid volumes manually face by face.

Thermal interface rules: component footprint faces must be coplanar with the board surface — any gap becomes a thermal air gap in the simulation. A 0.1 mm air gap between a component body and the PCB adds meaningful thermal resistance and will produce incorrect junction temperature predictions.

2.5  Defeaturing for Maxwell

Ansys Learning Hub: Electronics Desktop 3D Modeler Getting Started ↗ · 20 min · E-learning

Maxwell analyses require a bounded domain. Before modifying the device geometry, identify: which conductors carry current, which materials have significant permeability or conductivity, and whether the field distribution has any symmetry planes. Features outside the active field region can be removed. Features that define current paths — conductor cross-sections, insulation gaps — must be exact.

Air region: the most important step. Create a box or sphere enclosing the device with 3× clearance in each direction as a starting point. Verify by comparing results at 3× and 5× clearance — if inductance or loss changes by more than 2%, use 5×.

Symmetry: identify any planes of symmetry in the field distribution and apply symmetry cuts. A half-model solves in half the time. Verify that the excitation is symmetric before applying. Asymmetric excitation (e.g., winding current direction) invalidates symmetry.

Winding simplification: round wire cross-sections can be replaced with equivalent rectangular cross-sections of the same area. The field solution is nearly identical for strand counts above approximately 10 wires. This simplification dramatically reduces element count in winding regions.

2.6  Geometry Repair and Final Preparation

After import and defeaturing, run the repair sequence before meshing. The tools are in the SpaceClaim Repair panel (Design tab → Repair):^[2]

1. Check Geometry — run first. Lists face errors, open edges, and self-intersections. Every item in this list is a potential mesh failure.
2. Fix — automatic repair pass. Stitches open edges, merges duplicate surfaces, closes small gaps within the specified tolerance. Resolves most STEP import artifacts in one step. Set the tolerance to 10× the smallest significant feature dimension.
3. Close Gaps — closes sub-threshold gaps at part interfaces. Set the tolerance to match the tightest acceptable gap in the design.
4. Remove Slivers — eliminates narrow face strips below a specified width. Slivers are the most common source of high-skewness elements in imported assemblies.
5. Merge Faces — combines coplanar or co-cylindrical faces that were split by the import. Reduces face count and produces larger, more uniform mesh elements on flat surfaces.

After mechanical repair, apply Share topology at all interfaces where structural load or heat must transfer between parts (Design → Share).^[3] Share creates coincident node interfaces at part boundaries. Without shared topology, adjacent parts have independent meshes, and the solver uses contact elements to transfer quantities — which is slower and introduces numerical error.

Icepak geometry preparation tool

The Icepak geometry preparation tool (available through the Electronics Desktop integration) performs the repair sequence automatically on an entire assembly in one pass. It constructs a shrinkwrapped exterior mesh and discards all interior geometry. The result meshes very cleanly because it is a simple outer surface.

The tradeoff is irreversible: all internal geometry is discarded — internal conductor paths, component bodies, board layers, and internal structure are gone. Use this tool when: the assembly is too complex to repair manually and only exterior convection surfaces are needed, or when manual repair is exhausted and the mesh still fails. Make a copy of the original geometry before applying it. Do not use it as a default first step.

After running this sequence on a heatsink assembly, for example, the mesh quality histogram typically shifts the mean skewness from 0.42 (post-import) to 0.17 (post-repair) — a systematic improvement from removing the sliver faces and unmerged coplanar faces that import left behind.