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How to Simplify SOLIDWORKS Parts and Assemblies to increase performance

Article by Sanja Srzic created/updated March 2, 2017

We often suggest and discuss methods for improving performance of a SOLIDWORKS large assembly, e.g. using Defeature, Envelope, Large Design Review.  For components with complex geometry, perhaps used for reference, or manufactured elsewhere, the SOLIDWORKS Simplify tool can help reduce the complexity and the time to open and rebuild models.

The simplify tool works for both parts and assemblies.  The command is found in Tools > Find/Modify.  It suppresses fillets, chamfers, holes and extrudes based on their volume or main dimension.  All or some of these feature types can be included in the selection.

SOLIDWORKS Simplify Tool

SOLIDWORKS Simplify Tool

It is useful to select the option ‘Ignore features affecting assembly mates’ to avoid mate errors.

SOLIDWORKS Simplify Tools

The explanation of the simplification factor and search options is found in the tooltips that appear when hovering over them:

SOLIDWORKS Simplify Tooltips

SOLIDWORKS Simplify Tooltips

  • Simplification factor:  Simplification factor is used differently for “Feature Parameter” and “Volume Based” search (see below).  In both cases volume is the actual volume of the model/feature, not the bounding box.
  • Volume Based:  If feature volume is < (volume of part) * (simplification factor), it is considered for simplification.
  • Feature Parameter:  If Primary parameter value of a feature is < 3√ (minimum volume of body associated with the feature) * (simplification factor), it is considered for simplification.  Primary parameter is the critical dimension of the feature.  E.g. “Diameter” in case of hole, “Fillet Radius” in case of fillet.

Clicking ‘Find Now’ starts the calculation and displays the list of features that match the selected criteria.

Matching Features

Matching Features

Suppressing Features

All or some of the found features can be selected for suppression.  They can be suppressed in the active configuration of the assembly/components, or we can choose ‘Create derived configurations.’

Selecting Features

Selecting Features

Derived Configurations option

If the option is selected to create derived configurations, in all parts where selected features are being suppressed, a derived configuration is generated and used in a derived assembly configuration of the same name (if the file being simplified is an assembly).  The name of derived configuration can be changed before clicking Suppress.

Simplify Configurations

Simplify Configurations

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Sanja Srzic

Sanja is the SOLIDWORKS Technical Support Team Leader for Western Canada, and is based in the Javelin Winnipeg Office

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