SOLIDWORKS 2016 What’s New – Performance Evaluation – #SW2016

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The Performance Evaluation tool within SOLIDWORKS has been renamed from Assembly Xpert. What this function does is analyze the performance of large complex assemblies and also makes suggestions as to how to improve the performance of your assembly.

Please note that although any conditions found by this tool can degrade the performance, they are still NOT errors. It was intended for you to weigh the recommendations of the tool against your design intent because some of them can improve performance while others can compromise your design intent.

You can find Performance Evaluation on the Assembly toolbar or under the pull-down menu Tools > Evaluate > Performance Evaluation. There are icons that indicate the status of each diagnostic:

ICON

Status

Action

SolidWorks

Passed

No further action required

SolidWorks

Warning

Review and make changes

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Information Only

No further action is required

Diagnostic Tests

When you launch the Performance Evaluation, one of the items in the Open Summary report contains items such as warnings or error messages that you dismissed (setting found under Tools > Options > System Options > Messages/Errors/Warnings). If you click Show these Parts SolidWorks it will also list any parts or components that could not be opened, including the path of the part and the reason it could not load.

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There are different tools you can select based on the result of the diagnostic:

ICON

Status

Action

SolidWorks

Show these Parts

Lists affected components

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Turn on Large Assembly Mode

Activates Large Assembly Mode and updates the diagnostic results

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Analyze and Fix

Changes the assembly to fix the problem

 

Please note that if the model has not been rebuilt in the current version of SOLIDWORKS, there is no rebuild data available, so not all the tests can be performed. If the assembly takes more than 10ms to rebuild, Performance Evaluation provides a Rebuild Report for the total assembly. This report shows the time taken to rebuild significant components and features.

As we all know, opening a document from an earlier release might take extra time. If you have parts within the assembly that are Previous Version References and have not been updated to the current version of Solidworks, Performance Evaluation reports that as well. You can click on Show these Parts to view their filename and path:

SolidWorks

You can select one or more of the components to highlight it in the graphics area. Isolate Components would display only the selected components while Exit Isolate would return to the list. After a file is converted to the latest SOLIDWORKS version, subsequent opening time returns to normal.

Performance Evaluation can also report if whether or not Large Assembly Mode SolidWorks is ON, which is a collection of system settings that improves the performance of assemblies. You can turn on Large Assembly Mode at any time, or you can set a threshold for the number of components, and have Large Assembly Mode turn on automatically when that threshold is reached. Large Assembly Mode usually includes using Lightweight components.

Since lightweight components have only a portion of their model data loaded into memory, these components rebuild faster because less data is evaluated. The remaining model data is loaded on an as-needed basis. You can manually set single components, subassemblies, or entire assemblies to lightweight mode, or automatically load components lightweight as part of Large Assembly Mode.

Many of the settings in Large Assembly Mode are related to display performance, so even if the assembly does not have a large number of components, Display Speed can improve significantly in Large Assembly Mode. Additionally, you can also turn off Shadows in Shaded Mode SolidWorks, RealView Graphics, SolidWorks as well as minimizing the use of textures because as the complexity of the model increases, that can also slow down the performance. You can either NOT apply textures until you need them or create a derived configuration and apply textures to that.

Certain mating conditions can result in slower rebuild times. If mates rebuild slowly, Performance Evaluation reports any Mates that reference Assembly features or Patterned components.

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Mates that reference assembly features rebuild SLOWER than mates that reference component geometry. The same goes for mates that reference instances of components, because those generated by a component pattern rebuild SLOWER than those that reference non-patterned components.You can click Show these Parts in Performance Evaluation and select any of the mates for it to display highlighted in the graphics area.

Performance Evaluation also reports when in-context relationships as well as circular references established at the top level of your assembly contribute to a significant percentage of the assembly rebuild time. Clicking Show these Parts lists these components, as well as Isolate Components to highlight only the selected components in the graphics area. The software re-evaluates all in-context relationships established at the top level of the assembly when an assembly is rebuilt. By evaluating its mates and sometimes rebuilding the driving component, the location of the driving component is determined. After that, the driven component is rebuilt, and if it's a complex part with many features, rebuilding it can take a significant amount of time. There are a couple of things to note:

  • If you are making changes that require the driven component to be resolved, then the increased rebuild time is unavoidable.
  • If you are working on components that are not related to the driven component, you can improve the rebuild performance of the assembly by suppressing the driven component.

In-context Relationship Performance is another statistic available by Performance Evaluation, which reports which components need to be rebuilt multiple times when the top level assembly is rebuilt. You can select a component and click Analyze and Fix SolidWorks within the dialog box and the software updates the order of the assembly to reduce the number of times the component rebuilds.

Performance Evaluation reports if a subassembly contains a conflict within a single-configuration component that is driven by an in-context relationship to a multiple-configuration component. The result can be conflicts when rebuilding the assembly.

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SolidWorks

   

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You can select a component and click Analyze and Fix SolidWorks within the Performance Evaluation dialog box and the software adds a derived configuration to the selected component.

We've all come across the situation where one or more components within an assembly are very far from the assembly origin that the assembly seems to disappear when you zoom to fit. There are times where the assembly seems to zoom very far out to include the components near the origin, but also displays those very far from the origin.

SolidWorks

You can click Analyze and Fix SolidWorks within the Performance Evaluation dialog box to move the stray components closer to the origin. This will correct the extents of Zoom to Fit SolidWorks and make the entire assembly visible. At that point, it should easier to decide if you want those components to remain in the assembly or not.

The Verification on rebuild option provides an rigorous evaluation of the model during rebuild, but can also slow down rebuild performance. A couple of notes worth mentioning:

  • When this option is OFF, the software checks every new or changed feature against any adjacent faces and edges around it. For most situations, this default level of error checking is adequate, and results in faster rebuilding of the model.
  • When this option is ON, the software checks every new or changed feature against all existing faces and edges, not just adjacent ones. This has a negative impact on performance, which means that rebuilding the model is considerably slower and more CPU-intensive.

Finally, Performance Evaluation reports statistics about the components and mates in an assembly:

SolidWorks

We hope this part of this series gives you an understanding of how to use the SOLIDWORKS Performance Evaluation tool to help optimize your design. Please check back to the CATI Blog as the Dedicated Support Team will continue to break down each of the new functions in SOLIDWORKS 2016. All of these articles will be stored in the category of "SOLIDWORKS What's New."

George Brañes

CATI Support Engineer

Computer Aided Technology

SolidWorks