What's Covered?

• Optimal Hardware for efficient Modeling and Drafting
• System option settings
• 3DExperience Integration
• Several Option settings for optimal performance
   

Applies to the following Roles:

• 3DEXPERIENCE SOLIDWORKS Standard, Professional, Premium
• SOLIDWORKS Desktop

Summary:

This SolidPractices document contains recommendations for CAD administrators related to organizing and managing the CAD environment. By adhering to these recommendations, CAD administrators can significantly improve the organization and management of their CAD environment. These guidelines address key areas that directly impact the efficiency and effectiveness of SOLIDWORKS usage, leading to enhanced productivity, reduced errors, and improved overall project outcomes.

Revision History 

Note 

All SolidPractices are written as guidelines. You are recommended 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. This document may not be posted 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 SP4.0 and 3DEXPERIENCE R2023x FD04. If you have questions or need assistance with understanding the content, please get in touch with your designated reseller. 

Acknowledgments  

This document was authored by TriMech Solutions and reviewed by Dassault Systèmes SOLIDWORKS. 

1) Preface 

To maximize efficiency when using SOLIDWORKS, companies should consider optimizing three critical components: 

• Hardware specifications 

• Software settings 

• User knowledge and modeling procedures 

This SolidPractices document contains recommendations for CAD administrators related to organizing and managing the CAD environment, especially in these three areas. 

Designers should read the “Efficient Modeling” and “Efficient Drafting” SolidPractices documents, which cover modeling and drafting procedures. 

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2) Optimal Hardware for Efficient Modeling and Drafting 

When configuring the hardware for SOLIDWORKS end-user workstations, there are two approaches to avoid: 

• Trying to save money and choosing underpowered or incompatible components that impact user productivity 

• Spending too much on components that are not required for the type of work performed on that workstation 

For SOLIDWORKS desktop solutions, see the SOLIDWORKS system requirements. 

For 3DEXPERIENCE SOLIDWORKS, run the Cloud Eligibility tool. 

The system requirements indicate the minimal specifications that are necessary to create simple models in SOLIDWORKS. To create complex models, your system requires higher specifications. 

Keep in mind that your workstation is as fast as the slowest component used by your software. 

That is why it is ideal to analyze the type of work each workstation is expected to perform and configure it accordingly. While some workstations perform many different functions in a company, others could be dedicated to performing specific tasks like: 

• Modeling, editing and detailing parts, assemblies and drawings 

• Performing simulation studies (FEA, Motion, CFD, etc.) 

• Generating realistic renderings

• Batch processing for any of the above tasks (unattended workstation) 

Due to the rapid pace of improvements in the hardware performance, SOLIDWORKS does not recommend a specific type of CPU, graphics card, solid-state drive (SSD), network adapter or other hardware. Instead, this document lists the main characteristics that are critical for each main component, for each use case. 

To better understand the recommendations from this section, it is important to consider the way SOLIDWORKS processes information. Two of the activities that users perform most frequently are opening assemblies (Figure 1) and opening drawings (Figure 2). 

Figure 1 

Figure 2 

Table 1 

a) CPU

There are many myths about the criteria for selecting the CPU. The main myth is that “SOLIDWORKS is single threaded, so choose the CPU with the highest max turbo frequency for the single-core”. 

While relevant, the frequency is no longer the most important factor in choosing a processor. The latest generation CPUs have the same or even lower frequency than older generation CPUs, but their performance when used by SOLIDWORKS is much higher. You can expect an increase in performance of 10-20% per generation. 

The good news is that the latest generation CPUs with the highest single thread performance also have an adequate number of cores to support the multicore processes for all use cases: general modeling, simulation and rendering with SOLIDWORKS Visualize. 

One resource for comparing CPU performance relevant to SOLIDWORKS is: 

https://www.cpubenchmark.net/singleThread.html. 

b) RAM

At the time of publication, SOLIDWORKS recommends a minimum of 16 GB RAM for a SOLIDWORKS installation. Consider these use cases to adjust the amount of RAM for enhancing performance:

Table 2 

c) Local hard disk drive 

The good news is that most of the hard disk drives available today are SSDs. To maximize performance, consider using PCIe-based SSDs that adhere to the Non-Volatile Memory Express (NVMe) protocol. 

Make sure you have enough space on the SSD to host the working folders from which you open and save SOLIDWORKS files. If you use SOLIDWORKS PDM or 3DEXPERIENCE

SOLIDWORKS, place the vault view or the 3DEXPERIENCE local work folder on the SSD. 

d) Graphics card 

The latest versions of SOLIDWORKS take full advantage of the graphics card power. That is why it is important to match the use cases with the graphics card level. 

Table 3 

*or equivalent 

 For the list of certified graphics cards, see the SOLIDWORKS Hardware Certification website. (https://www.solidworks.com/support/hardware-certification) 

e) Network

The recommendation is to load and save all files from the local drive. The network speed is still very important for the traffic between the PDM vault and the local vault view, or the 3DEXPERIENCE platform and the local work folder. 

f) Data management versus non-data management environments 

For the scope of this article, a data management solution refers to one of the following: 

• SOLIDWORKS PDM Standard 

• SOLIDWORKS PDM Professional 

• 3DEXPERIENCE SOLIDWORKS 

• Collaborative Designer for SOLIDWORKS 

This document focuses on the performance when working with files on the local computer. 

Working with files from the local SSD compared to files opened from a network server: 

• Reduces crashes 

• Reduces file corruption 

• Minimizes file load and save times 

When IT specialists tell you that your company has the fastest possible network and huge files could be moved around extremely fast, they are correct. Windows® is optimized for moving large amounts of data on the network. Unfortunately, SOLIDWORKS does not load entire files into memory during the opening process, and that is a good thing. Some people create assemblies that have file sizes of tens of GB, and it would be impossible to load that much data in the RAM. 

Instead, SOLIDWORKS performs repeat reads of small packages of data from each file. Imagine this dialog between SOLIDWORKS and the file when loading a component of an assembly: 

Figure 3 

And the questions continue until all the relevant data loads into the RAM. 

Performing repeat reads of small packages of data is much slower when the file resides on the network compared to the local drive. Figure 4 illustrates why: 

Figure 4 

Local SSD drives are several times faster for finding and reading small amounts of data compared to the network drives. However, manually copying the files back and forth between network drives and your local drive is tedious and prone to error. This is the task for data management systems. 

When you open a file, the data management system verifies that the latest copy of the file exists on the local drive. Because copying large amounts of data is fast, the data management system transfers the data as necessary without your intervention. SOLIDWORKS performs the multiple small reads from that local file. 

For large assemblies, the time savings are spectacular, as shown in Figure 5. 

Figure 5 

In summary, if your team has more than one user, having a data management system can dramatically improve your productivity. 

g) Performance benchmarking 

Even when computer specifications appear comparable, the performance of the systems, including both hardware and software, can exhibit significant disparities depending on the SOLIDWORKS users. In such instances, it is advisable to conduct the SOLIDWORKS performance test on all the computers. 

After that, you can compare the scores for each computer to understand which components are responsible for generating different results. 

In addition, you can expand the comparison beyond your team using the Share Your Score tool to see how your computer results compare with the results collected from the larger 

SOLIDWORKS community. 

This comparison is especially useful when similar computers exhibit significant differences in performance. If that happens, the next thing to investigate is the differences between the SOLIDWORKS system options for each computer. 

These topics are covered in the later sections of this document. 
 

3) Impact on Performance When Using Files Saved in Older Versions 

When opening files saved in an older version, SOLIDWORKS converts the data read from the file to the format of the current version. This is time-consuming and could have other unexpected side effects like: 

• Unnecessary rebuild of components during loading 

• Unnecessary drawing view updates when such components exist in the model 

If these files load in read-only mode, they do not update during saving. This means that the entire conversion process repeats every time the files load as components of assemblies or drawings. 

To automate the upgrade process, companies that do not have a data management system can use the SOLIDWORKS Task Scheduler for batch processing multiple files. The only limitation with using this tool is that there are no options for defining the processing order. Ideally, the conversion observes the parent-child relationships between files, starting with stand-alone part files and progressing to simple assemblies all the way to top-level assemblies and drawings. 

This ensures that when the upgrade process is complete, all the files are up to date and require no unnecessary self-updates during opening (See Phase 2 in Figure 1.) 

To bulk upgrade all the files in one or more folders, or even in the entire SOLIDWORKS PDM vault, you can use the SOLIDWORKS PDM File Version Upgrade tool. This tool automatically checks out, upgrades and checks in SOLIDWORKS files that are stored in the SOLIDWORKS PDM vaults. File references, revision tags and workflow states remain intact. 

Only the SLDPRT, SLDDRW and SLDASM file formats are upgraded. You must upgrade the SOLIDWORKS template and block files manually. 

Several workstations, each running the upgrade tool, can perform concurrent upgrades to reduce the upgrade time. 

4) SOLIDWORKS System Options at the Team Level 

SOLIDWORKS is built on the principle that: “Users tell us how the software should work, not the other way around”. Therefore, with almost 6 million active users of the software, the options for customizing the SOLIDWORKS environment accommodates for the differences in needs, modeling techniques and hardware systems that exist in the SOLIDWORKS community. As the usage needs shift from individual users to teams and companies, consistency in SOLIDWORKS settings and modeling techniques becomes more important than the personal preferences of each user. 

There are hundreds of system options and covering all of them in a short document is unfeasible. Fortunately, the SOLIDWORKS Help contains comprehensive information about the system options. 

The system options are stored in the Windows registry and are independent of the SOLIDWORKS documents and document properties. 

The CAD administrator can lock some options to ensure compliance with a company’s policies. 

Before changing your settings, be sure to perform your own internal validation. 

a) Model integrity versus operational speed 

As a parametric, associative CAD software, it is no wonder that SOLIDWORKS prioritizes the model and drawing validity over everything else. Ideally, the model or drawing is always up to date after opening, and to ensure that, the software can prompt frequent events for rebuilding features, checking the validity of topology, updating assemblies, generating graphics data or updating drawing views. 

Automatically recomputing data is time-consuming and often unnecessary. Finding the right balance between using existing data and recomputing is key for maximizing users’ operational speed while working with current models and therefore the need for optimizing the system settings. An example is allowing the software to always update all drawing views on open or allowing the user to decide which drawing views to update and when. 

b) Default system settings 

After a fresh installation, the system settings offer an acceptable balance of performance and security. Every year SOLIDWORKS adds new options that might not be easy to discover after upgrading. Figure 6 depicts an easy way to reset all system options to the factory defaults or to only those options on specific pages. 

Figure 6 

The following sections discuss the pros and cons of optimizing the most critical SOLIDWORKS system options for: 

• Minimizing the opening times for large assemblies and drawings. 

• Minimizing the operational slowdowns after opening the model or drawing. This is caused by: 

  • Repetitive model rebuilds. >Repetitive assembly updates. >Repetitive graphics generation. >Repetitive drawing views updates. 

• Maximizing operational efficiency by: 

  • Reducing repetitive interactions with the user interface. 

  • Eliminating unnecessary interactions with the user interface. 

  • Reducing the steps needed for finding or accessing: 

    • Tools 

    • Commands 

    • Feature tree items 

    • Modified dimensions 

• Reducing clutter in the: 

  • Graphics area >FeatureManager® design tree 

• Creating robust models and drawings (model integrity). 

• Ensuring drawing consistency. 

5) Finding a Specific System Option 

Because of the large number of options, browsing to a specific system option can be challenging. 

Fortunately, SOLIDWORKS includes the Search Options field, which makes it easier to find any option (Figure 7). 

Figure 7 
 

6) General System Options 

Figure 8 

a) Include documents opened from other documents  

The Recent Documents tab of the Welcome dialog box is one of the best time savers when working with a set of files and folders for a long time. It allows users to perform multiple actions instantly, including: 

• Open files in multiple modes: 

  • Quick View (parts) oResolved 

  • Lightweight (assemblies and drawings) o Large Design Review (assemblies) 

  • Detailing (drawings) 

• Select the configuration or display state. 

• Open faster without loading hidden components. 

• Insert a component into an assembly (drag and drop). 

• Insert a part into another part (drag and drop). 

• Create drawing views by dragging a model onto a drawing. 

• Open File Explorer, find and select the file, 

To maximize the value of this tool, activate the Include documents opened from other documents option (Figure 8). 

b) Allow cosmetic threads for upgrade 

Many companies create fasteners in SOLIDWORKS 2018 or older versions. SOLIDWORKS 2019 optimizes the rebuild and update behavior for cosmetic threads. 

To upgrade cosmetic threads, you must open each part, right-click the FeatureManager tree and then click Upgrade cosmetic thread features. This may cause existing annotations to dangle. The Allow cosmetic threads for upgrade system option (Figure 8) allows you to postpone the upgrade to a more convenient time. 

Over time, upgrading all cosmetic threads helps to increase the efficiency of your team. You can perform this operation in bulk using a macro with the Task Scheduler, the Vault Upgrade tool or other third-party batch processors. 

7) 3DEXPERIENCE Integration 

Figure 9 

Refer to the help article “3DEXPERIENCE Integration Options”. 

Users of 3DEXPERIENCE SOLIDWORKS have an extra section in the System Options. The decision to activate the Update SOLIDWORKS files for compatibility with the 3DEXPERIENCE platform option depends on how your company decides to load files. 

• It is best to leave this option as inactive (the default) when working with files that are not managed by the 3DEXPERIENCE platform. 

• It is best to activate this option when working with files that are shared with users who do not have access to your collaborative spaces on the 3DEXPERIENCE platform. 

8) Drawings Options 

a) Automatically populate the View Palette with views 

Figure 10 

Activating the Automatically populate View Palette with views option could be beneficial when creating new drawing views of parts and small assemblies. However, this can significantly increase the open time and update time for drawings of large assemblies, especially if the models contain a large number of custom orientation views or 3D views. 

For example, activating this option increased the rebuild time by 98% in the example shown in Figure 11. Waiting 21 minutes for the drawing to open or update is a high price to pay for the convenience of being able to create drawing views by dragging them from the Task Pane. 

Figure 11 

b) Allow auto-update when opening drawings 

Figure 12 

Having the drawing views update automatically upon open could be very beneficial when performing unattended batch operations such as printing or saving multiple files to the PDF, DWG or DXF formats. That would ensure that the final product is up to date, even when the referred models require rebuild. 

When detailing complex drawings over multiple days, users must open the same file multiple times. For drawings with many sheets and complex drawing views, activating this option could increase the opening and update time by an order of magnitude. 

In this case, the recommendation is to deactivate this option as long as you instruct your users about the best practices for performing incremental updates of specific sheets or only specific drawing views. 

Figure 13 - Updating one sheet on-demand 

Figure 14 - Updating one or more views on-demand 

9) Colors Options 

a) Use specified color for changed drawing dimensions on open 

Figure 15 

Activating the Use specified color for changed drawing dimensions on open option is highly beneficial during drawing updates. When the model is revised, the user needs to see what dimensions have changed and by how much, compared to the old values. 

There are a number of benefits that include: 

• Faster revisions. Adding revision flags can be streamlined, because all the changed dimensions are clearly highlighted. In addition, filling in the revision description is also helped because both the old and new dimension values are easily accessible by the user (Figure 15).

• Ensure accuracy. The changed dimensions are highlighted on the screen, so the user can easily spot any unwanted or accidental changes that appear in the drawing (Figure 16). 

Be aware that after saving the drawing, the changes are considered approved by the user and the color of all dimensions return to the default settings. 

10) Performance Options 

This is one of the most important pages of system options that could impact the performance of your system. It allows for fine-tuning the amount of computations the CPU and GPU perform for the most basic and frequent tasks to suit your hardware specifications and the type of models that you work with. 

Figure 18 

a) Verification on Rebuild (Figure 18) 

Heavy impact on CPU – Single Core 

To understand the effect of activating the Verification on rebuild option, it is worth remembering the importance of having solid and surface bodies with clean topology in your models. One of the typical factors that invalidates a body in SOLIDWORKS is the intersection of its faces without generating an edge along the intersection curve. 

Imagine how much work the software must perform to validate every feature that adds or modifies faces. Ideally, it is best to examine any new or modified face for invalid piercing against all the faces of the model, regardless whether or not they share a common edge with the new face. 

That is the effect of activating the Verification on rebuild option. All faces are involved in this validation process. If the software spots a piercing condition, an error tag appears on the feature that generates the invalid faces. That could affect the rebuild time tremendously as shown in Figure 18 and Figure 19. 

To save time, experienced users can deactivate this option. In this case, only the faces that share edges or vertices with the new faces are selected during the rebuild process. There is little chance of such errors appearing, but it is important for users to know how to spot them before performing more work on a flawed body. 

Activating the Verification on rebuild option is probably the biggest slow-down factor for users of complex parts or large assemblies. This is independent of how experienced the users are with using the software. 

While this setting controls the checks that the software performs during the rebuilding of parts, it could also dramatically affect the assembly performance if one or more of the following conditions exist: 

• Components missing body data (that would trigger their rebuilding). 

• Assembly features. 

• In-context relations that require updating. 

• Changing configurations when the configuration data is not precomputed. 

To mitigate these issues, when using Large Assembly Settings, the Verification on rebuild option could be deactivated automatically when an assembly meets the conditions that you define for qualifying it as a large assembly (Figure 21). 

Figure 21 

b) Enhanced graphics performance (Figure 18) 

Before SOLIDWORKS 2019, the graphics engine was based on OpenGL 2.0. When manipulating the viewport (zoom, rotate, pan or select) the CPU and the GPU (graphics card) shared the work. This engine was old and slow and was not optimized to take full advantage of the power of modern graphics cards. There was almost no difference in performance between an entry-level graphics card and a high-level card. 

SOLIDWORKS 2019 and later versions offer a new graphics engine based on OpenGL 4.5 is offered as an option, using much more the GPU power. Despite some initial discrepancies, much progress has been made to eliminate these issues. Therefore, this engine is more reliable and efficient than ever. In addition, starting with SOLIDWORKS 2021, the graphics performance of drawings has also been enhanced. 

The only reason that you might want to deactivate this option is for troubleshooting. Also, remember that after modifying this option, be sure to restart SOLIDWORKS for the change to take effect. 

c) Level of detail (Figure 18) 

This option is heavily dependent on the type of GPU and the setting of the Enhanced graphics performance option. 

If you have a certified graphics card newer than 5 years, do a simple test. Move the Level of detail slider to the extreme left (Off) position, open the most complex model you have and see how smooth the viewport manipulation becomes. If it is acceptable, leave the slider there. 

Figure 22 – Rotating with 328 frames per second with no dynamic graphics simplification. 

This slider exists for legacy reasons. Several years ago, both the software and the hardware were ill-equipped to dynamically manipulate large sets of graphics data. To mitigate that, any dynamic viewport manipulation (zoom, spin or pan) was broken into four phases: 

1. Inspect the model and identify bodies or components with a high level of complexity. 

2. Replace these components with the representation of their bounding boxes. 

3. Perform the dynamic manipulation requested by the user (zoom, pan or rotate). 

4. Replace the bounding boxes with the full graphics detail. 

This was a smart way to temporarily decimate the graphics complexity, enabling underpowered computers to perform acceptably. 

Modern graphics cards are perfectly capable of storing and dynamically manipulating an entire graphic set, eliminating the need to perform 3 out of the 4 phases in the list. Because of that, the fastest results are achieved when no graphics simplification is performed. This is the reason for the recommendation to move the slider to the Off position. 

Please be aware that if you use the Large Assembly Settings, you will likely move the slider elsewhere. That is why for specific use cases, it is best to avoid using the Large Assembly Settings. 

d) Purge cached configuration data (Figure 18) 

Never activate the Purge cached configuration data option, unless you need to reduce the size of a file with multiple configurations knowing that doing so would dramatically slow down any assemblies or drawings using that as a component. 

Backstory 

About 10 years ago, during the Top 10 Ideas season, users with a different CAD software background started a campaign for implementing a Purge function in SOLIDWORKS. 

The users argued that the other software had a fantastic purge function that would quickly remove unused data and dramatically reduce the file size. They thought the SOLIDWORKS files were bloated and that such a function would be beneficial. 

There is a reason behind having a larger file in any CAD software, including SOLIDWORKS and other software. When computing a certain data set is time-consuming, it might be more efficient to save that data in the file for future reuse. Avoiding the computation of unchanged data over and over could save users a lot of time. 

Purging simpler 2D data might not have a huge impact on performance, because such data could be recomputed relatively fast. The situation is different for many SOLIDWORKS cases. 

When developers considered what type of data could be purged safely from a SOLIDWORKS part or assembly file, they came up with configuration data. 

Configurations in SOLIDWORKS could save the following types of data in the part or assembly file: 

Table 4 

When thinking about configuration data, you can make an analogy between baking a cake and building a SOLIDWORKS model. 

When baking a cake, you follow a recipe. Features, mates and custom properties are part of the SOLIDWORKS recipe. They must be saved as part of the file. 

To create a variation of that cake, modify the recipe. The look and the taste will be different. A recipe is pure information, typically written on a piece of paper. It cannot be eaten. To produce the cake, you must bake it according to the recipe. 

It is the same thing with SOLIDWORKS. To generate the body data, you must build the model feature by feature. In addition, to generate the graphics data, you must tessellate the body data in tiny triangles and pass it to the graphics card to display. 

The body data and graphics data consume a lot of space, so purging them may have sounded like a good idea. It is true that usually computing the graphics is fast. After all, it always occurs after loading the file, so there is no big loss here; other than the inactive configurations are not accessible in the eDrawings® application or in the Large Design Review mode. 

At the first sight, even computing the body data is usually pretty fast at the part level. However, assemblies and drawings are a different story. 

When the body data for a component of the assembly is missing (think of a small bolt that the assembly requires in one of its inactive configurations), the part requires rebuild during the loading phase of the assembly. After rebuilding, it is identified by the assembly as a changed component. That causes the rebuilding of all subassemblies that contain the component all the way to the top level. This dramatically increases the opening time. 

As you can imagine, the slowdown is even worse for the drawing of the assembly. Because the assembly is identified as modified, all drawing views require updating. Depending on the number and types of drawing views, this could be a painful experience. 

When the assembly or drawing is saved, because this setting is active, the body data for all inactive configurations gets purged. Therefore, an unnecessary rebuild happens again the next time the files open. 

When SOLIDWORKS 2013 was released, the introduction of a feature for purging configuration data received significant attention and positive feedback. This led to enthusiasm among IT departments because it resulted in a notable reduction in the size of SOLIDWORKS files and an increase in the amount of available server storage space. 

Complaints about a decrease in performance began trickling in much later, because it took a while for the users to notice. The decrease in performance was gradual; the more files that were saved, the more body data was lost, affecting mostly the library files. 

Even now, many technicians, instructors and presenters still recommend activating the purge option without considering the implications on user performance when working with large assemblies and drawings. 

User should be very cautious when using the Purge cached configuration data setting. 

11)     Assemblies Options 

Figure 23 

a) Automatically check and update all components in Large Design Review mode (Figure 23) 

Large Design Review is a powerful tool, but with great power comes great responsibility. The reason assemblies open so fast in this mode is that only the graphics data saved in the assembly file is required. When this option is inactive, users see the assembly in the state that it was last saved. If a component was updated since then, the graphics data is out of date, and you would receive no warning. The consequences can be very costly. 

Users who want to use this mode without first obtaining professional training, should always activate the Automatically check and update all components in Large Design Review mode option. The good news is that while the check and data update operation is performed, users can continue to interact with the assembly because multiple CPU cores are used. 

Trained users do not activate this option if they know how to update the graphics data of the entire assembly or of selected components on-demand. 

b) Change mate alignments on edit (Figure 23) 

Did you ever add a mate only to have several existing mates flip automatically? You can maintain control of your model by choosing the Prompt or Never options for the Change mate alignments on edit option. 
 

12)     External References Options 

 Figure 24 – SOLIDWORKS Desktop page shown 

The following options are specific to SOLIDWORKS desktop products and do not exist in SOLIDWORKS Connected: 

• Open referenced documents with read-only access 

• Don’t prompt to save read-only referenced documents (discard changes) 

• Reference Documents specified in File Locations 

a) Open referenced documents with read-only access and Don’t prompt to save read-only referenced documents (discard changes) (Figure 24) 

Be cautious when checking both options simultaneously. Some users who have done so reported they lost many hours of work. They opened assemblies with all their components loaded read-only and performed modifications affecting components. When saved and closed the files, there was no notification about all changes being discarded. 

b) Search external references (Figure 24) 

Unless users are familiar with the search routine for referenced documents, it is best to leave the Search external references option inactive. Not only do they save time by not forcing SOLIDWORKS to perform unnecessary searches, but they also avoid the risk of having the wrong component loaded into an assembly or drawing. 
 

13)     File Locations Options 

This is one of the most important settings for ensuring consistency at the team level. It is important for all users to work using the company standards. 

 Figure 25 

The Edit All function allows access to all file locations in a single dialog box (Figure 26). This is very useful, especially after upgrading the software, when using the Find/Replace functionality is a great time saver (Figure 26). 

Figure 26 

14)     FeatureManager Options 

Figure 27 

a) Scroll selected item into view (Figure 24) 

For large assemblies, if you experience a lag when selecting components, consider deactivating this option. Even better, use a macro that switches this option on or off as required and assign a new button on the CommandManager. 

b) Dynamic highlight (Figure 24) 

This is another setting where opinions are divided about the impact on operational speed. When working with large assemblies on underpowered systems, users could experience a lag when moving the pointer over the model. On modern systems, this is typically not a problem. 

The benefit of activating this option is huge for all tasks that require accurate selection of entities (edges, faces, vertices, planes, axes, sketches and more). 

Sometimes, users who struggle to select edges on the models or drawings turn this option off. Often, they select the wrong entity and either repeat the operation, or do not notice, and apply the wrong mate or dimension. 
 

15)     Hole Wizard/Toolbox Options

 Figure 28 

a) Make this folder the default search location for Toolbox components 

*This option is not available in SOLIDWORKS Connected. 

When this option is active, it facilitates the opening of models with Toolbox components that do not reference the Toolbox folder. If you deactivate this system option, SOLIDWORKS does not automatically search the Toolbox folder for references to Toolbox components. 

Be aware that if you customize the Toolbox or the Hole Wizard database, it is important for all users to access the same location. Users have the best experience (for SOLIDWORKS desktop) when SOLIDWORKS PDM manages the database. This allows the users to open files from their local vault image, while still using the same common data.      

16)     Messages/Errors/Warnings – Dismissed Messages Options 

Figure 29 

It is a recommendation to review all dismissed messages frequently. Many times, users select a specific choice (Yes or No) when dismissing an error or warning message that may not be suitable for other operations later. 

17)      Saving Time by Using Efficient Templates at the Team Level 

This document shares best practices for creating and using part and assembly templates. The section related to drawing templates is covered in the “Efficient Drafting” SolidPractices document. 

The use of templates is critical to foster consistency within your team. By ensuring that all users are using the same template files, the template management is also easier. 

a) Establishing file locations 

If you are using SOLIDWORKS Connected, you can manage SOLIDWORKS templates from the 3DEXPERIENCE platform. 

If you have a SOLIDWORKS PDM system, you can manage SOLIDWORKS templates using PDM. This way, all users are able to keep their template files on their local drive always synchronized with the templates in the vault. 

If you do not have a PDM system, you can save the templates on a network share and point the document templates folder to this location on all workstations (Figure 25). 

b) Document properties for all types of templates 

i) Units 

Define the default units to comply with the standards of your company. 

 Figure 29 

ii) Image Quality 

The number of graphics-triangles representing the shape of the model is a direct result of the image settings. The CPU computes the graphics-triangles, which are handled by the graphics card. 

 Figure 30 

• Shaded and draft quality HLR/HLV resolution 

Controls the tessellation of curved surfaces for shaded rendering output. A higher resolution has more accurate curves, but increases the file size and the time for graphics processing. The recommendation is an image quality setting of 10%. 

• Optimize edge length 

To help understand the effect of this setting, see Figure 31. When this option is not active, SOLIDWORKS applies a common sense mesh of graphics triangles. For example, the software represents any rectangular face with only two triangles, regardless of the image quality setting. 

When this option is active, SOLIDWORKS attempts to create a consistent mesh. That results in a huge number of graphics-triangles. 

Be aware that when the upper slider is in the red, the Optimize edge length option become active automatically, but is not editable in that state. 

 Figure 31 

• Apply to all referenced part documents This option is available for assemblies only. 

• Save tessellation with part document (Parts only) 

This option is available for parts only. The option saves the display information. When the option is not active, the file size is reduced (often significantly). However, the model does not display when the file is open in view-only mode, in the SOLIDWORKS Viewer, or in eDrawings. When the file is opened again in SOLIDWORKS, the display data regenerates. 

• Wireframe and high quality HLR/HLV resolution 

This option controls the image quality of the model edges in drawings. 

Low (faster) - High (slower) 

The slider changes the image quality. If you want to redraw the screen more quickly and the display quality is not of great importance, move the slider to Low. Move the slider to High (slower) for a high display quality, but a slower redraw. If you experience problems with the HLR image display, move the slider to the right. 

• Precisely render overlapping geometry (higher quality, but slower) 

This option applies to drawing documents only. When a drawing contains many tiny intersections, deactivate this option to enhance performance. 

• Improve curve quality at higher settings 

This option applies to drawing documents only. When active, this option improves the curve quality when regenerating drawings by allowing the specification of a finer tolerance for tessellated curves. Because this option affects performance, use the option only when you require a very high curve quality. 

Important: If the image quality setting is identical for all components of an assembly, the software performs the graphics computation phase (#5 in Figure 1) using multi-core processing. That is why it is critical for all users to start their models from the same templates. 

After creating the files, there are two strategies companies use to ensure that the image quality setting remains consistent on all files: 

When users work with models, they are allowed to temporarily modify the image quality setting to suit their needs. For example, when performing a visual check on a tubing routing, the components seem to interfere with a low image quality setting. To enable quick image quality resets, macros could be used (Figure 32). 

 Figure 32 

You could replace the Save button with a macro that resets the image quality setting to the company standard. Doing so removes the need for the user to reset it manually. For example, in Figure 32, that is the Save for Check-in macro. 

For existing files with various image quality settings, the solution to achieve consistency is to use Task Scheduler or the SOLIDWORKS PDM File Version Upgrade tool to batch process all files using a macro that sets a consistent image quality in all the files. 

Be aware that virtual components require resetting the image quality manually. 

c) Document properties for part and assembly templates 

Document properties apply only to the active document. That is why defining the optimal properties in the part or assembly templates ensures that all models start with a consistent set of properties. This document discusses the properties that affect the most modeling efficiency. 

i) Model Display 

See the SOLIDWORKS Help article “Document Properties - Model Display”. 

 Figure 33 

Considerations: 

• Store the appearance, decal and scene data in the model file. 

• Stores custom appearances, decals and scenes with the model for easier sharing. This increases the file size of the model. Alternatively, use Pack and Go to package custom files with the model. 

• Take advantage of the Comments functionality to color code comments based on your company standard. 

d) Document properties for drawing templates 

Document properties apply only to the active drawing document. That is why defining the optimal properties in the part or drawing templates ensures that all new drawings start with a consistent set of properties. This document discusses the properties that affect efficiency and consistency the most. 

i) Drafting Standard 

Defining the company drafting standard in the document properties is the best way to ensure consistency in detailing your company drawings. It is worth knowing that you can save the drafting standards in external files and load them on demand in older drawings that do not conform to the current company standards. 

 Figure 34 

It is a recommendation to treat the saved drafting standards as another type of template to store in the vault or in a common location on the network (for those not using a data management system). Inform your users that whenever they need to apply the company drafting standards on a non-conforming drawing, they could simply load these files. ii) Detailing 

To take full advantage of the options on the Detailing page, it is important to study the workflows that your designers use and identify repetitive tasks that you could automate using the options shown in Figure 37. 

For example, it is possible to import a large number of annotations automatically when adding new drawing views. 

 Figure 35 

Be aware that you can activate and deactivate some of these options from other areas of the user interface. For example, you can access the Import annotations box from the View Palette (Figure 38) or the Model View (Figure 39).

iii) Performance 

The state of this setting could have a critical impact on: 

1. The speed of opening drawings. 

2. The time to save drawings. 

3. The size of drawing files. 

When the Save model data option is active, the software writes more edge-related data in the drawing file to allow the fast opening of the drawing independent of its model for detailing purposes. 

In most projects, 90% to 95% of the drawings are of parts or small assemblies. Therefore, the recommendation is to deactivate this option in your drawing templates. 

When users begin experiencing slowdowns as they increase the complexity of a drawing, they could decide to activate the Save model data option (Figure 38), save and close the drawing, and then reopen the drawing in Detailing mode. 

Be aware that when the Save model data option is active, the software assigns a unique Silhouette Edge ID to each edge of the model. Therefore, it is critical to ensure that all drawing views specify the High quality option in one of these 3 display states: 

• Hidden lines removed 

• Hidden lines visible 

• Wireframe 

For such drawing views, the Silhouette Edge IDs are already assigned, so the saving time is minimal. 

For drawing views that specify the Draft quality, Shaded or Shaded with Edges options, the Edge IDs would generate during saving, increasing the saving time tremendously. That is reasonable considering that in draft quality views, the edges are computed based on the graphics-triangles extracted by tessellating the mathematical body data of the model. Imagine the sheer number of tiny triangle edges that must be stored for each individual edge. 

It is also worth knowing that if your drawings refer to components with imported geometry errors, the drawing views could always be draft quality, and the saving operation then suffers accordingly. 

e) Other template types 

As your CAD administrator experience grows, you can help your team take advantage of other types of templates, including: 

• Bill of Materials 

• Costing Reports 

• Costing 

• General tables 

• Hole Tables 

• Property Tabs 

• Punch Tables 

• Revision Tables 

• Sheet Metal Bend Tables 

• Sheet Metal Gauge Tables 

• Weld Tables 

• Weldment Cut Lists 

18) Professional Training Solutions for Your Users 

SOLIDWORKS is the most popular professional software for parametric 3D CAD modeling. 

Thanks to a large community of users who enthusiastically share, there is a lot of 

SOLIDWORKS-related content on all social media platforms, especially in the SOLIDWORKS User Forum. 

Such information is a treasure when searching for answers to specific questions, however, it is not ideal for structured learning. Because we do not know what we do not know, self learning is a time-consuming exercise. Information from the internet could be low quality, obsolete or even dangerous.

Attending professional training courses developed by SOLIDWORKS is the quickest way to develop your proficiency and learn the skills that are relevant to your position the right way. 

This section describes the various training options that are available for your users. 

a) Live Instructor-Led Classes 

These training courses were written by SOLIDWORKS and are the gold standard of learning in the industry. The characteristics of this training include: 

• Offered by SOLIDWORKS value added resellers (VARs). Contact them directly to schedule such courses. 

• Physical or electronic manuals are included for each course. 

• Delivered by SOLIDWORKS-certified instructors. 

• Delivered in-person or live online. 

• Use real-life case studies to illustrate processes. 

• Hands-on practical experience. 

• Official SOLIDWORKS certificates of completion at the end of the course. 

• Courses can be combined to form learning paths. 

• Your satisfaction is guaranteed. 

• Offer the highest return on investment. 

b) MySolidWorks eCourses 

These video-based structured training courses are available 24 hours per day. The characteristics of this training include: 

• Perfect complements to the instructor-led training. 
• Complete courses converted by SOLIDWORKS from the instructor-led training manuals into self-paced eLearning. 
• Guided practice. 
• Offline exercises. 
• Highly interactive content. 
• No manual is provided. 
• Yearly subscription. All courses are available for a small fee (not included in the SOLIDWORKS subscription benefits). 

c) MySolidWorks Lessons 

This video-based training is available 24 hours per day for different topics. Characteristics include: 

• Individual learning modules that consist of lectures, videos and quizzes. 
• Included in the SOLIDWORKS subscription benefits. 

Includes online training content for 3DEXPERIENCE solutions. 3DEXPERIENCE platform users automatically get Guest access for a selection of learning paths, learning modules and certifications. The Guest access includes content that is relevant to 3DEXPERIENCE SOLIDWORKS. The learning paths and learning modules are self-paced. Additional training options are available through your SOLIDWORKS VAR. 

19) Professional Certifications for Users 

The SOLIDWORKS Certification Program is an objective-driven tool to test and validate proficiency in all SOLIDWORKS areas. It can challenge your users to specialize in areas that interest them. 

User can view all their certificates in the 3DEXPERIENCE Certification Center (Figure 43). 

Figure 43 

Each user can share this page with their manager, Human Resource department or with the CAD administrator. 

The Certification Center also allows the validation of individual certificates. If prospects include their certificate numbers on their job application, you can validate them (Figure 44). 

Figure 44 

20) Conclusion 

This document focused on the best practices for configuring the SOLIDWORKS environment for the optimal performance and consistency of your team. Depending on what other areas of SOLIDWORKS your team uses, other SolidPractices documents are availablethat complement this information. Examples: 

• Efficient Modeling 
• Efficient Drafting 
• Working with Sheet Metal Design 
• Working with Weldments 
• Managing Large Assemblies in SOLIDWORKS 
• Working with Imported 3D Data 
• Working with Imported 2D Data 

We hope that you find this document informational and useful and request that you leave a brief feedback about the topics that you want us to cover in the next revision of this document. Click here for a complete list of SolidPractices documents available from Dassault Systèmes SOLIDWORKS Corp. 

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