SolidWorks Simulation studies fail in predictable ways. Not at solve time — failure is obvious then. They fail quietly during setup, producing results that look plausible but reflect a model that doesn’t match what you assembled. Bolt connectors that don’t attach. Contact sets that miss a mating pair. A material assigned as 1060 Alloy because the template default was never changed.

These issues are systematic. The same five checks catch them before the solver runs and before you hand results to a reviewer who will find them the hard way.

1. Toolbox Component Configuration

SolidWorks Toolbox components (fasteners, bearings, bushings) can be inserted in two configurations: Simplified and Default. The difference matters for Simulation: Simplified bodies have suppressed or absent features, and Simulation’s automatic connector detection expects specific geometry to be present.

The problem: A socket head cap screw inserted as Simplified renders as a cylinder with a flat head — no hex socket, reduced thread geometry. Simulation’s bolt connector algorithm searches for cylindrical body faces to anchor the connector. On a Simplified body, it may find the shank but fail to anchor the head contact correctly, producing a connector that shows in the study tree but contributes zero preload.

Check: In the assembly, select any Toolbox fastener → Properties → Configuration. If the active configuration is Simplified_*, you have a decision to make. For stress analysis around fastener holes, switch to the Default configuration before setting up Simulation. For stiffness studies where fastener geometry isn’t a factor, Simplified is usually fine.

Diagnostic: If a bolt connector is showing Abnormal pretension load warning after setup, the first thing to check is whether the Toolbox component was inserted as Simplified. Switch to Default, delete and re-create the bolt connector. The warning typically disappears.

The bolt connector pretension cycle covers what happens in the two-phase solve and why pretension warnings matter beyond just setup correctness.

2. Bolt Connector Detection Scope

SolidWorks Simulation’s automatic bolt detection (Simulation → Connections → Bolt → Use Simulation Bolt) scans the assembly for cylindrical interfaces and proposes connectors. It misses bolts in two common situations:

Sub-assembly scope: Automatic detection is scoped to the top-level assembly context. Fasteners inside sub-assemblies are detected only if those sub-assemblies are set to Rigid in the Simulation study, not Flexible. If your assembly uses Flexible sub-assemblies and fasteners are inside them, automatic bolt detection will not find them. You need to add connectors manually, selecting the bolt body and mating faces explicitly.

Non-Toolbox fasteners: Detection relies on SolidWorks’ internal fastener recognition. Custom-modeled fasteners or imported STEP fasteners don’t have the required Toolbox metadata. Simulation can still use them as pin or bolt connectors, but you must define the connector manually.

Check procedure:

  1. Run automatic bolt detection and note the count
  2. Visually inspect the assembly with the connector list open — every fastener should have a corresponding connector
  3. For any flexible sub-assembly, expand it in the Simulation tree and verify connector presence manually

When bolt detection count is wrong: Suppress the fastener bodies in the assembly, run automatic detection again. Detection count should drop by exactly the number of suppressed fasteners. If it doesn’t match, some fasteners are either being double-counted or missed.

3. Contact Set Completeness

SolidWorks Simulation has four contact behavior options at the study level: Bonded, No Penetration, Allow Penetration, and Free. The global contact setting applies to all component pairs that don’t have an explicit local contact set defined.

The error: Global contact is Bonded, but two components should slide or separate. This produces artificial stiffness that can underestimate stress by 30-60% in assemblies with mating parts that are meant to bear against each other without being bonded.

What to check:

  • Press-fit interfaces: Two cylinders in a hole — should be No Penetration (or Shrink Fit connector), not Bonded. Bonded here merges the bodies mathematically and prevents any stress concentration at the interface.
  • Bolted joint bearing faces: The face under a bolt head or nut against the surrounding plate should be No Penetration with friction if the study is checking joint separation. Bonded assumes infinite adhesion.
  • Clearance-fit pins: A pin in an oversized hole that can rock — must be No Penetration to capture the correct load path.

The practical check: In the Simulation study tree, right-click Connections → Show All Contact Sets. The list shows every explicitly defined contact. Any interface not in the list uses the global setting. Go through the assembly joint by joint and confirm that structural load-bearing interfaces have the right contact definition.

The subset test: For complex assemblies, use Advanced Component Selection to filter by material or manufacturer to isolate component groups that are likely to have contact issues — purchased inserts, press-fit bushings, rubber isolators.

4. Mesh Quality at Critical Regions

SolidWorks Simulation’s default mesh is curvature-based and handles most geometry without explicit intervention. It fails silently at two feature types:

Small holes relative to part size: A 3mm hole in a 400mm bracket. The mesh generator may apply a default element size of 15mm — creating only one or two elements across the hole diameter. Any stress concentration at the hole will be grossly under-predicted. The minimum number of elements across a curved feature for reasonable accuracy is 4-6. For stress concentration, you need 8+.

Sharp re-entrant corners: A notch or step with no fillet. Simulation’s stress result at a theoretical sharp corner is mesh-dependent and will increase without bound as the mesh refines. This is a modeling problem, not a meshing problem — but it shows up as mesh quality failure.

Pre-run mesh check:

  1. Mesh the assembly with default settings
  2. Open Simulation → Mesh → Mesh Quality → select Curvature-Based Mesh Quality Plot
  3. Any region flagged red (aspect ratio > 10, or Jacobian check failures) needs a local mesh control

Adding a local mesh control: Right-click the study → Mesh Control → select the face around the critical feature → set element size to 1/6 of the feature’s smallest dimension. For a 3mm hole, set local mesh to 0.5mm.

The efficiency tradeoff: A 0.5mm mesh at a 3mm hole in a 400mm assembly will produce a very large element count. Apply local controls only at load-bearing interfaces and stress concentration sites — not globally. For large assemblies, check managing large CAD assemblies for performance thresholds — the same memory limits that affect CAD rebuild apply to Simulation mesh generation.

5. Material Assignment Verification

SolidWorks Simulation applies materials from one of three sources: the SolidWorks material library, the model’s Material property (set before entering Simulation), or a direct assignment inside the study. These three sources can conflict silently.

The trap: You set a part’s material to 304 Stainless Steel in the part file. In the assembly, you copy the study from a previous version. The copied study has an explicit material override set to 1060 Alloy for that component. The study-level override wins. Your results reflect aluminum, not steel.

Check:

  1. In the Simulation study tree, right-click each solid body → Apply/Edit Material
  2. Verify the material source (From SW Material property, or explicitly assigned in study)
  3. For large assemblies, use Simulation → List Result Data after a preliminary run — it produces a material summary per body. Cross-check E-modulus values: steel ~200 GPa, aluminum ~69 GPa, wrong material is immediately visible in this output

The Elastic Modulus sanity check:

Steel (304):    E = 193 GPa,  ρ = 8000 kg/m³
6061 Aluminum:  E = 68.9 GPa, ρ = 2710 kg/m³  
Titanium (6Al-4V): E = 110 GPa, ρ = 4430 kg/m³
ABS Plastic:    E = 2.0 GPa,  ρ = 1020 kg/m³

If any body shows deflection results that seem large by an order of magnitude relative to what you’d expect from the loading, check whether its E-modulus matches the expected material.

After Setup: Two Checks Before Presenting Results

Once the study runs:

1. Reaction force check. The sum of reaction forces at all fixtures must equal the applied loads (within solver tolerance). In Simulation Results, right-click Stress → List Result Force. Sum the reaction forces across all fixture faces. If the sum doesn’t match the applied load within 1-2%, the boundary conditions are incorrect — typically, a fixture that doesn’t constrain all relevant degrees of freedom, or a load applied with the wrong direction.

2. Convergence check for stress peaks. Re-run the study at 50% mesh density (double the global element size). If peak stress changes more than 10-15%, the current mesh is too coarse at the stress peak. The mesh quality diagnostic above applies here — add a local mesh control and re-run.

These two checks catch the majority of result errors before they reach a reviewer. The pre-run checklist above catches the setup errors that produce wrong results that still converge cleanly.