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Note

All SolidPractices are written as guidelines. It is a strong recommendation to use these documents only after properly evaluating your requirements. Distribution of this document is limited to Dassault Systèmes SolidWorks employees, VARs, and customers that are on active subscription. You may not post this document on blogs or any internal or external forums without prior written authorization from Dassault Systèmes SolidWorks Corporation.

This document was updated using version SOLIDWORKS 2023 SP01. If you have questions or need assistance in understanding the content, please contact your designated reseller.

Preface

As your assemblies grow larger, they will invariably consume more computer resources. Your system must load more geometry, solve more functions, and display more data. This can lead to slower performance within assembly and drawing documents.

Broadly speaking, a large assembly is a file that uses all of your computer system resources while performing common operations. Common operations include opening, closing, and saving files; rebuilding assemblies; creating drawings; rotating and viewing; and inserting and mating components. For this reason, there can be a decrease in performance, which can hurt productivity.

You can minimize the additional overhead by building your assemblies more efficiently and by using SOLIDWORKS features designed to optimize workflows within large data sets.

This guide walks you through various techniques proven to improve the performance of your largest assemblies and drawings.

The SOLIDWORKS Help contains additional consolidated information.

You can find answers to specific questions in the SOLIDWORKS Knowledge Base, in online forums, and through your local Value Added Reseller (VAR).

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SOLIDWORKS Activities When Opening and Updating an Assembly or Drawing

To understand the benefits of the best practice suggestions, it is useful to understand what happens when you open or update an assembly or drawing. The following flow chart illustrates the activities that must happen. Suggestions in this document address different aspects of this flow chart to help improve all-around performance.

Load all of the referenced parts and sub-assemblies (may be thousands of files)

Update any parts or sub-assemblies that are out-of-date

Solve all mates and position components

Update in-context features and assembly features

Paint display for updated assembly

No component has changed since assembly was last saved

Open Assembly or Assembly Drawing

Solve mates again if they reference assembly features

Update all configurations of the assembly referenced by the drawing

For Drawings, continue processing

Show updated assembly in draft quality views (projection and named views)

Solve dependent views like Section View

Rationalize layers and line fonts to display final drawing views

Solve High Quality views in background

Finished

Best Practices to Improve File Open Times

When opening large assemblies and drawings, you can spend a significant amount of time waiting for the data in the referenced components to load. Opening thousands of files can take a while. The following series of techniques are designed to optimize your files and settings to make this operation as fast as possible.

Work Locally

It takes longer to open and save files over a network than opening or saving files locally. Depending on your network environment and load at any given time, open and save time can be much slower than performing the same operations locally. Even if you maintain documents on a central server, it is more efficient to copy the files locally, make your changes, and then copy the files back than it is to work directly over the network. This is what many Product Data Management (PDM) solutions do, including the SOLIDWORKS PDM software.

For more information about the limitations of working with SOLIDWORKS files over a network, see the Knowledge Base solution S-051256 or QA Article QA00000112222.

If you are working remotely, or from home, review the SOLIDWORKS Knowledge Base solution S-077757 or QA Article QA00000123656, which provides tips and suggestions for working from home using SOLIDWORKS® 3D CAD.

Use Large Assembly Mode or Lightweight Mode

With Lightweight Mode, you can load less than half the data as a fully resolved assembly. Lightweight Mode does not load the SOLIDWORKS feature data from parts that are not necessary at the assembly level.

Why load everything? Lightweight Mode loads only the body and the mate data. In most cases, this is all that is necessary for further modeling, mates and drawing creation. Therefore, your assembly may load faster than fully resolved.

By default, Large Assembly Mode loads assemblies as lightweight. Additionally, Large Assembly mode activates several options at once, which contribute to improvements in performance.

From the release of the SOLIDWORKS 2023 software, you can optimize resolved mode automatically. On Tools > Options > System Options > Performance > under ‘Assembly loading’, the ‘Automatically optimize resolved mode, hide lightweight mode’ option enables selectively using lightweight feature when you load components in resolved mode. If you choose to manually manage when to resolve lightweight components, switch to ‘Manually

manage resolved and lightweight modes’ option.

For more information, refer to the SOLIDWORKS Help and the “What’s New” documentation.

Large Design Review (Assembly)

Effective with the release of the SOLIDWORKS 2012 software, Large Design Review (LDR) is a powerful tool to help manage large assemblies. While Lightweight Mode opens only the body data from the referenced components, Large Design Review only loads the display data, which is even lighter than lightweight.

You can use the measure tool within Large Design Review mode. It is also possible to isolate and strategically load only the necessary components needed, instead of loading an entire assembly. The ‘Automatic check and update all components’ option makes it possible to determine whether to check components for out-of-date graphics data and to update components when opening an assembly in Large Design Review mode.

Effective with the release of the SOLIDWORKS 2020 software, there are further enhancements to Large Design Review mode. In addition to the ability to insert components when you edit an assembly, available already in the SOLIDWORKS 2019 software, you can now create and edit linear and circular component patterns, driven, and sketch driven component patterns. Be aware that this functionality is available for top-level assemblies only.

Furthermore, you can create mates not only to faces and edges of components, but also to the reference geometry of components when editing an assembly in Large Design Review mode.

From the release of the SOLIDWORKS 2022 software, you can open a subassembly in Large Design Review mode or resolved mode from an assembly opened in Large Design Review mode. Also, you can open a drawing in Detailing mode from an assembly opened in Large Design Review mode.

For more information, refer to the SOLIDWORKS Help and the “What’s New” documentation.

Detailing Mode (Drawing)

Effective with the release of the SOLIDWORKS 2020 software, you can use Detailing Mode to open large drawings quickly. Detailing Mode is particularly useful if you need to make minor changes to drawings of large assemblies or drawings with many sheets, several configurations, or in presence of resource-intensive views.

With Detailing Mode, the model data does not load, but you can add and edit annotations, create general and revision tables, copy or cut drawing views and paste them onto the same or other sheets within the same drawing, and more.

From the release of the SOLIDWORKS 2021 software, Detailing Mode enhancements include the creation of break views, crop views, detail views, and the ability to add dimensions and annotations to these views. You can also create or edit hole callouts for different hole types and cut features.

From the release of the SOLIDWORKS 2022 software, you can create hole table and drag standard views (such as front, top, back) from the View Palette to the drawing in Detailing Mode.

Detailing mode is available for all drawings (except detached drawings), regardless of the SOLIDWORKS version in which you saved the drawing or whether you saved the drawing in Detailing mode.

With the release of the SOLIDWORKS 2022 software, the ‘Detailing Mode’ option has been moved from System Options (Tools > Options > System Options > Drawings > Performance, ‘Include Detailing Mode Data when saving’ option has been removed) to Document Properties Options (Tools > Options > Document Properties > Performance) with these two new options:

• Save model data: Saves all drawings with model data to use in Detailing mode.
• Include standard views in View Palette: Let’s you create standard views when you add drawing views from the View Palette.

Note to fully use the ‘Detailing Mode’ functionalities on legacy files where ‘Detailing Mode’ data where not saved, you first need to open the file and save it with ‘Save model data’ option enabled. For the full list of capabilities and limitations available in Detailing Mode, refer to the SOLIDWORKS Help and the What’s New documentation.

Use Simplified Versions of Models and SpeedPak Subassemblies

Cosmetic features add edges and faces without helping assure their fit and function within assemblies. In some cases, these features can double the total number of faces in an assembly and lead to a degradation of performance in assemblies and especially in drawings. You can use a detailed version for the part design, and a simplified version for higher-level assemblies referencing the part design. Each version can be stored as a different configuration.

In some cases, such as purchased parts, a highly detailed model is not necessary. Use the Defeature tool or the Simplify utility to automatically reduce the face count, edge count, and file size of the model. Effective with the release of the SOLIDWORKS 2019 software, Defeature in an assembly allows you to create groups to simplify files by using the silhouette method.

You can also strategically target cosmetic features. You should first target the parts used most often. Common examples include:

• Internal components, such as rollers in bearings
• Threads
• Extruded text
• Vents and fasteners on purchased parts

Use the

Assembly Visualization

tool to identify components that have a significant amount of detail relative to other components. Add the Graphics-Triangles column, and sort the column to identify the components.

Using SpeedPak derived configurations can help reduce the amount of data in subassemblies. The graphics data generated using SpeedPak may be enough to represent a subassembly within the top assembly. A good application of SpeedPak is with purchased and imported parts and assemblies. When a part does not import cleanly and has many unknit surfaces, you can use SpeedPak to keep only the fundamental geometry that is necessary.

Faces and references geometry defined within the SpeedPak can be used for mates.

An important consideration about configurations and SpeedPak: Adding a simplified configuration increases the file size of the part because you will add a new configuration to the existing fully detailed part. Despite this, it is faster to open a model in a simplified configuration because the SOLIDWORKS software only opens the data necessary, ignoring the detailed configuration data.

Note with the release of the SOLIDWORKS 2022 software, import of large DXF or DWG file and STEP file has been improved, which further enhance the overall performance when working with imported data.

Use Display States Instead of Configurations Where Possible

You can and should use configurations to store different designs of an assembly. However, if you want to show different displays of an assembly or part, use display states. Think of display states as a skin that overlays one assembly. Think of a configuration as an entirely new assembly contained in one file. Parts and assemblies with configurations contain much more data than parts and assemblies that use display states.

For example, if you want to show different colors or if you want to hide components or isolate some components for your work, it is more efficient to represent that with a display state and not a configuration.

Likewise, if you plan to show different displays in drawings, you should also use display states instead of configurations. If your drawing references multiple configurations of an assembly, you must update each of those configurations before the drawing can update. A single configuration in multiple display states needs to update only once.

Convert Data Forward to the Latest Version

You may need to convert your models to a new version to prepare them for code changes in the latest release. This happens when you open an older file version in a new version of the software. This can increase opening times. After conversion, this step is no longer necessary. You can perform conversions on an active project or model as necessary by opening and saving a file within a newer version of SOLIDWORKS. You can also use Task Scheduler or SOLIDWORKS PDM software solutions to convert entire data sets or projects.

Be aware that it is possible to open SOLIDWORKS 2023 assemblies by using the SOLIDWORKS 2022 Service Pack 5 software. However, when doing so, the SOLIDWORKS 2023 files do not display most of the FeatureManager® design tree data. For more information, refer to the SOLIDWORKS Help and the What’s New documentation.

Use the ‘Assembly Open Progress’ Indicator to Help Understand Where the Most Time is Spent While You Open an Assembly

Effective with the release of the SOLIDWORKS 2018 software, the

Assembly Open Progress

indicator provides information about the status of operations while you open an assembly.

The dialog box displays the total number of components opened and the total number of files in the assembly, model updates (including mates, assembly features, patterns, and in-context models), graphic updates, time to open the assembly, and the previous time to open the assembly document.

View open performance information for a specific assembly from Tools > Evaluate >

Performance Evaluation

.

Use ‘Assembly Visualization’ to Sort Components by Their Opening Time and Rebuilding Time in Assembly

An enhancement to the

Assembly Visualization

tool allows you to view the open and rebuild times for the components, and the total number of graphics triangles for all instances of components.

Beginning with SOLIDWORKS 2017, the SW-Open Time property stores the time taken to open each of an assembly’s components the last time you opened and saved the assembly. You can access this property from Tools > Evaluate >

Assembly Visualization

. This information is useful to determine which components take the longest to open. You can then simplify or remove those components to decrease the time it takes to open the assembly.

Note from the release of the SOLIDWORKS 2023 software, SOLIDWORKS calculates more Assembly Visualization columns without setting the lightweight components to resolved, allowing better performance with the

Assembly Visualization

tool.

Beginning with SOLIDWORKS 2018, the Performance Analysis utility provides additional information to isolate components based on their opening and rebuilding time in an assembly. The Performance Analysis utility displays the following properties:

• File Name
• Quantity
• Total Graphics-Triangles (indicating the graphics burden)
• SW-Open Time
• SW-Rebuild Time

Best Practices to Improve Update Times

If there is a change to any part of any component within an assembly, it will become necessary to rebuild the assembly, and eventually, the drawing to reflect that change. Use of the following techniques will help optimize the activities associated with the SOLIDWORKS update cycle, thus ensuring that they run as efficient as possible.

Limit In-Context Features

Components without in-context features do not rebuild their feature tree and can even avoid loading their feature tree altogether in Lightweight Mode. Conversely, a component with in-context features must rebuild its tree when the assembly changes. At that point, all child features of that in-context feature must update also. If you have multiple in-context components, this continues for each one. This process can be time consuming because the total number of regenerating features grows. Imagine 30 components that have 10 features that are in-context or dependent on an in-context feature. Any change to the model will result in the update of 300 features. This does not include the solving of mates.

Effective with the release of the SOLIDWORKS 2020 software, consider activating the Tools > Options >

System Options

> External References > Allow creation of references external to the model option to limit how external references are created.

• Reference component type:
  • Any Component or Only Envelope Component
• In the context of:
  • Top level assembly or Same subassembly

For more information, refer to the SOLIDWORKS Help and the What’s New documentation.

 

Limit Equations at Top-Level Assembly

When you open an assembly in lightweight mode, if there are components referenced by equations in the top-level assembly, they display as resolved. Also, when you resolve a part or subassembly that has equations and the equations reference another lightweight component, the referenced component will be resolved. Consider limiting equations at assembly level, to avoid automatic resolving referenced components.

 

Limit Mates by Using Rigid Subassemblies

SOLIDWORKS treats a subassembly as a rigid body with the exception of flexible subassemblies. This means that it is possible to locate even the largest subassembly with only three mates. By using rigid subassemblies, you can simplify your mate structure within large assemblies. This improves performance and makes troubleshooting much easier.

 

Limit the Use of Flexible Subassemblies

Mates within a flexible subassembly also solve with the current assembly document mates. Therefore, they influence the performance as well. There is additional overhead to solve the positions of flexible subassemblies, and this may result in additional time to solve mates within an assembly document.

 

Avoid Mating to Patterned Instances and to Assembly Geometry

Examples:

• An assembly level hole feature
• An assembly plane or axis defined by faces of a component
• A face of a patterned component

The SOLIDWORKS software is optimized to solve all mates simultaneously. The software then follows the assembly tree order to rebuild. Mating to assembly geometry creates an order dependency. First, the mates are solved to determine the location of the components. Then, the components update their position and the assembly features solve. Finally, the mates solve again to account for the new positions.

'Suspend Automatic Rebuild’, Skip Rebuild After Editing Components and Other Options to Improve Update Times

Since the release of SOLIDWORKS 2017, you can select

Suspend automatic rebuild

as the default system option for Large Assembly Mode from Tools > Options >

System Options

> Assemblies. Upon activating this option, in-context parts will show a rebuild light instead of automatically rebuilding, when opening assembly with Large Assembly Settings enabled. This allows you to make multiple changes and then update at once. The

Suspend Automatic Rebuild

option is especially useful in complex routing assemblies that rely on in-context sketches by their nature. The option has no effect on other common assembly updates, such as mates and display.

Similarly, from the SOLIDWORKS 2017 software, the Do not rebuild when switching to assembly window option lets you skip the rebuilding of a large assembly after editing a component in a separate window. The Disable verification on rebuild system option lets you suspend the advance body checking verification on rebuild when working in Large Assembly Mode. Both of these options are available in the

Large Assembly Mode

system options.

In assemblies with tens or hundreds of fastener stacks at the top level, the number of mates can have a noticeable impact on assembly performance when solving mates, adding mates, dragging components, and so on. Since SOLIDWORKS 2019, you can use the Lock rotation of new concentric mates to Toolbox components option to automatically lock rotation for new concentric mates to Toolbox components. Upon clearing this option, you will see performance improvements when working in assemblies that have several Toolbox components inserted and mated at the top level. Then, clearing the Automatic Update for Toolbox Mates option (right-click on the Mates folder in the FeatureManager design tree) allows you to disable the solving of mates to Toolbox components temporarily. This makes it quicker to edit mates, add more mates, and manipulate components with clear performance improvements.

Reduce the Graphical Demands of Your Assembly

In assemblies, the following recommendation will improve the time needed to paint the display during updates. This will also improve your ability to zoom, pan, and rotate assemblies. Many of these options are set automatically when you enable Large Assembly Mode.

• Move the image quality slider (Tools > Options > Document Properties > Image Quality) to the Low position.
• Turn off HLR Edges in the Shaded Display mode.
• Turn off RealView.
• Limit the use of transparency.
• Hide items that you do not need from the View menu.
• Move the Level of detail slider (Tools > Options > System Options > Performance) to the Less (faster) setting.
• Disable the Verification on rebuild (enable advanced body checking) option (Tools > Options > System Options > Performance).

Also, consider switching off the following options:

• Tools > Options > System Options > Display
  • Highlight all edges of features selected in graphics view
  • Dynamic highlight from graphics view
  • Anti-aliasing
• Tools > Options > System Options > FeatureManager
  • Dynamic highlight

The latest releases of the SOLIDWORKS software, beginning with SOLIDWORKS 2019, provide a new graphics architecture for displaying parts and assemblies, which results in a smoother, more responsive real-time dynamic model display. This architecture significantly improves dynamic display performance, maintaining a high level of detail and frame rate when you pan, zoom, or rotate the model. These dynamic performance improvements scale up with higher-end graphics cards, taking advantage of Modern OpenGL (4.5) as well as hardware accelerated rendering, which were not fully supported in previous versions of the SOLIDWORKS software.

To enable the new graphics architecture, select Tools > Options >

System Options

>

Performance

> Enhanced graphics performance (requires SOLIDWORKS restarts) option.

Use Performance Evaluation to Help Find Bottlenecks in Assembly

Performance Evaluation diagnostic tests display information about how your assembly is performing.

Starting with the SOLIDWORKS 2018 software, the

Performance Evaluation

utility (Tools > Evaluate >

Performance Evaluation

) includes increasingly more information on the open, display, and rebuild performance of models in an assembly.

Effective with the release of the SOLIDWORKS 2021 software, Performance Evaluation detects circular references in assemblies (under Rebuild Performance in the

Performance Evaluation

dialog box , review the Circular References section for issues).

For more information, refer to the SOLIDWORKS Help and the What’s New documentation.

These details can help you target your efforts for optimizing your assembly.

Best Practices to Improve Drawing Update Times

Opening a drawing document also opens referenced part or assembly documents in memory. Improving assembly performance in general also improves drawing performance.

Effective with the release of SOLIDWORKS 2019, multi-sheet drawing update is smarter, which means that drawing updates are no longer required if there is no change to the geometry. Examples include creating a sketch, editing and cancelling features, or deleting an unabsorbed sketch.

Use Hidden Line Removed (HLR) Drawing Views

When possible, avoid using Hidden Line Visible (HLV) and Wireframe drawing views. These views are more expensive to draw than HLR drawing views. HLR drawing views have fewer edges to draw, so they generate and update faster.

Use Simplified Versions of Models (Again)

This is a helpful strategy to improve open and update times in assemblies. However, this strategy is especially useful in improving drawing update times. Generating high quality drawing views is a time-consuming operation. Therefore, removing unnecessary geometry has an even greater impact in the drawing environment.

Limit Section Views

Section views may be necessary for some tasks, but consider other ways to represent interior details where possible. Section views are the most expensive drawing views in terms of calculation time. To generate a section view, the SOLIDWORKS application must create an assembly level cut across the model located at the section line. It must then generate the view based on the cut faces and then draw hatching. With each model update, SOLIDWORKS recalculates and redraws the assembly level cut and regenerates the section view.

Turn Off the ‘System Options’ > ‘Drawings’ > ‘Performance’ Options

When working with large drawings, you can tactically turn off the Show contents while dragging drawing view, Allow auto-update when opening drawings, and Save tessellated data for drawings with shaded and draft quality views options to improve performance.

Effective with the release of the SOLIDWORKS 2015 software, the Allow auto-update when opening drawings option is available to systematically control Automatic View Updates for all drawing files. When you deactivate this option, you can strategically update your drawing views as needed instead of allowing the SOLIDWORKS application to update all views automatically upon activation of the drawing. Out-of-date views appear with red hatching. You can update these views individually by using the right-click context menu.

Effective with the release of SOLIDWORKS 2019, the Automatic View Updates option is saved within the drawing file and behaves more consistently across various SOLIDWORKS sessions. In previous SOLIDWORKS versions, the option was effective only in the specific session in which it was set.

Use Performance Evaluation to Help Find Bottlenecks in Drawings

Since the release of SOLIDWORKS 2018, the

Performance Evaluation

tool is available for drawings from Tools > Evaluate >

Performance Evaluation

. Use of this tool in a drawing examines your drawing file and lists the rebuild times for drawing elements such as drawing views, sketch entities, and referenced files. These statistics, along with the performance evaluation information available in the assembly, can help you determine if the items that take longer to load and rebuild are in your assembly or your drawing. Then you can focus on these items to improve performance.

Be Strategic

Whether you make one change or you make 30 changes to the model, your drawing views will need to recalculate and redraw. For efficiency, it is better to make multiple changes and then update the drawing views only once.

High quality drawing views typically take more time to create and rebuild, but less time to save when compared with Draft quality drawing views. For improved performance, consider creating the drawing by inserting Draft quality drawing views and then convert all of the views to High quality in preparation for detailing (insert of dimensions, annotations, etc.) or drawing export.

File export formats with high quality export options such as Save as DWG/DXF and Save as PDF require High quality views in drawings.

Improve Assembly Update Time

Generally speaking, drawing update time relates directly to the update time of referenced assemblies. Work to improve the update times of the referenced assemblies to have better performance in drawings.

Hardware Considerations

These best practice suggestions can help improve performance by reducing the amount of workload on your system. You can apply the suggestions to existing systems with significant results. Another approach to improve performance is to increase the power of your system.

When using well-maintained and current professional workstations, you will experience only an incremental improvement by adopting the fastest machines available. If your computers are older or underpowered, a hardware upgrade may be more justifiable. The SOLIDWORKS Rx tool includes a benchmark test that you can use to help evaluate systems. CAD Admin users can also use the CAD Admin Dashboard to monitor the performance and hardware status of designers’ workstations.

The following general guidelines can help to determine if improvements to hardware will improve your performance.

RAM

Make sure that you have enough physical RAM to avoid paging. When you exceed the physical memory, your operating system borrows space on your local disk drives to supplement the RAM. This can cause a dramatic drop in performance. Increasing RAM to avoid paging is one of the most economical upgrades you can make.

To help understand how much RAM may be necessary, open all applications typically used during a standard workday. Then open an example of a Large Assembly Design and review the available physical RAM consumption in your environment.

CPU

A faster CPU is better. Faster processors are helpful for most, but not all operations. For example, file open times are more dependent on disk and network speeds than on the processor speed.

Most current workstations have a minimum of 4 to 8 processors or cores. This does improve overall performance through general multi-tasking. Additional processors or cores will be helpful only for some operations, such as PhotoView360 rendering or Simulation studies. Extra cores may have little effect on open or update times, which are sequential and not simultaneous operations. Benchmark your system before committing to a purchase.

Graphics Card

The SOLIDWORKS development team does not test graphics cards for performance but instead recommends that customers use graphics cards that are certified for use with the SOLIDWORKS software. For large assemblies, look for the mid to high range of offerings in the NVIDIA® Quadro and AMD cards, and Virtual GPU.

Low-end cards may not have enough memory and they may become outdated too quickly.

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