| Rev # | Date | Description |
|---|---|---|
| 1.0 | Oct 2020 | Document created |
| 2.0 | Oct 2023 | Added section #16 to cover 3DEXPERIENCE Platform for SOLIDWORKS |
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 SP03 and 3DEXPERIENCE SOLIDWORKS R2023x FD03. If you have questions or need assistance in understanding the content, please get in touch with your designated reseller.
Acknowledgment
This document was originally authored by TriMech Solutions and reviewed by Dassault Systèmes SolidWorks Corporation. Subsequent updates to this document were performed by Dassault Systèmes SolidWorks Corporation.
Preface
SOLIDWORKS is one of the leading 3D engineering solutions worldwide. For years, this suite of applications has allowed users to unlock the potential of their concept and helped bring innovative designs to market. To get the most out of the applications, there are best practices that you should take into consideration. The purpose of this guide is to clarify those practices and to serve as a reference for both new users and seasoned veterans.
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Units and Enforcing Standardization
When it comes to documenting designs, standardization across an organization is of the utmost importance. The goal of computer-aided design (CAD) models and drawings is to communicate the design intent of the engineer or the designer. If every individual has their own way of communicating, important details may be lost in translation. By unifying and adhering to standard practices and units and settings, there is likely to be more consistency in that communication.
Specifying Units in Document Properties
There are several ways to change the units of your document. Any document, whether it is a part, drawing or assembly, can use its own unit system. To change these units, go to Tools > Options, and click the Document Properties tab. In the document properties, select the Units category. There are four default unit systems. You can also create a custom unit system. You use different units for Length, Dual Dimension Length, Angle, Mass, Volume and others. Refer to the following image.
Help Document: Units and Dimension Standard
You can quickly access and change these options by selecting the units function on the right side of the status bar within SOLIDWORKS.
It is a best practice for organizations to standardize their designs to conform to a single unit system. This helps to avoid errors and miscommunication of the design intent. Because the unit system saves per document, this is sometimes challenging. To resolve that challenge, consider creating custom templates for each document type, with the specified units preconfigured. The next chapter of this guide covers templates in more detail.
Checking Units with Design Checker
Even when using custom templates and a standard unit system, nonstandard units might still exist within a document. To look for these inconsistencies, SOLIDWORKS provides the Design Checker tool. This tool lists any nonconforming dimensions, and can correct the unit system automatically if you choose to do so.
In addition to standardizing units, organizations might want to consider other methods to enhance communication.
Features in a SOLIDWORKS FeatureManager® Design Tree receive names based on the type of feature. Users can rename each of these features. Using more descriptive feature names allows faster modification of designs and makes it easier for other users to understand the design intent of the original author.
Users can also rename dimensions. Much like renamed features, descriptive dimension names make it easier to understand what each dimension controls. This allows for quicker changes with fewer errors.
It is also possible to add comments throughout the SOLIDWORKS FeatureManager Design Tree, or to the document itself. Similar to comments in a programmer’s code, these feature and document comments help users communicate their intent for each feature, or for the overall design of the document.
It is best to fully define sketches whenever possible. Sketches that are not fully defined appear in the SOLIDWORKS FeatureManager Design Tree preceded by (-). For example, (-) Sketch1. Over defined sketches are preceded by (+). For example, (+) Sketch2.
You should also resolve errors and warnings in features and sketches because these can lead to problems when modifying the design in the future. Such errors and warnings can hinder performance.
Templates
Building on the philosophy of standardization in CAD documentation, templates are an essential starting point for that documentation. By using shared templates, users ensure that specifications such as units and document appearance are consistent across designs, regardless of the individual author.
Creating Templates
As mentioned in the previous chapter, templates are a great way to store your specifications for unit systems. In addition, you can store any modifications to options within the document properties in a document template. This is a great way to prevent the need to make frequent changes to those settings. For drawings, templates can also save the choice of sheet format file.
It is a good practice to create custom templates for parts, drawings and assemblies. While you can use any file to create a template, it is typically best to start with a blank document.
To create a template:
Open a new document.
Change the Document Properties as required.
Click Save As.
For Save As Type, choose the respective template type from the list. You can select a part template (*.prtdot), a drawing template (*.drwdot), or an assembly template (*.asmdot).
Selecting a template file type automatically switches your save as location to the first folder in the Document Template folders in the File Locations options (Tools> Options > System Options > File Locations). You can reorganize the file locations to place the required folder at the top.
Help Document: Creating a Template
Specifying Sheet Format Files for Drawing Templates
For drawing templates, SOLIDWORKS saves a file location for the sheet format within the template. The sheet format file contains the border, zone labels and title block for the drawing. Users can either create a sheet format from scratch, modify one of the default files for the sheet format that are included with SOLIDWORKS, or create a sheet format by importing an existing DWG or DXF file that uses an existing standard for your organization.
You can link items in the title block to custom properties, which makes it easier to populate a title block with properties.
Specifying Default Templates
Users should designate one template as their default template for each SOLIDWORKS file type. To set a default template, click the Default Templates category in the System Options. This page lists the file locations for each default template for Parts, Assemblies and Drawings. To change the locations, click the ellipsis (…) for that location and select a new template from the available tabs.
Help Document: Default Templates Options
Managing Template Locations and Permissions
After creating templates, you can share the templates with multiple users. This helps ensure consistency in the document settings across the organization. One way to do this is to store the templates in a shared folder on a network drive. Users can then add that folder location to their list of Document Templates in the File Locations category of the System Options. When using this practice, the recommendation is to specify the Read-only permission for each template file. This prevents users from making inadvertent changes and breaking from company standards.
Help Document: Creating Additional Template Tabs
Storing Templates in the SOLIDWORKS PDM Vault
If a SOLIDWORKS PDM vault is in place, it might be beneficial to store the templates in the vault. This ensures that the templates are accessible by all vault users and benefit from the same version and revision history as any other file. It might also be worthwhile to create a custom workflow or workflow state for the template files because an organization probably handles these files differently than other files in the vault. It is a good practice to limit file permissions so users without administrative access cannot modify the templates without the approval of managers.
Consider applying these same guidelines for sheet format files (*.slddrt) as well.
Users can also make use of the templates specific to SOLIDWORKS PDM. This makes it possible to prepopulate the Custom Properties and Data Card of a document with variables (such as serialized part numbers) from the SOLIDWORKS PDM system.
Default Drawing Settings
When creating new drawing templates for your organization, it is important to understand some of the default settings and content contained within the standard default templates. This allows organizations to focus on modifications that might be required for their documentation, such as the title block, borders and sheet format layer of drawings.
Drawing Standards
By default, drawings in SOLIDWORKS specify a regional standard (ANSI, ISO, etc.). This standard, along with many other options, are controlled by the document properties, which can be saved in a template. This allows the use of different templates for different standards.
Editing the Sheet Format and Title Block
The default drawing template includes a single sheet, which also includes a default sheet format file. The sheet format file contains the border and title block that appear on the drawing sheet, as well as anchor points for the available tables. To edit the sheet format file, either right-click the sheet or sheet format nodes in the drawing tree, or on any blank area of the drawing sheet, and then choose Edit Sheet Format. You can also enter the sheet editing mode by going to Edit > Sheet Format.
The title block contains data pertaining to the part or assembly that appears in the drawing. You can enter this data manually or using the Note tool to add text to the title block. It can be helpful to populate these data fields automatically. After adding a note to a title block field, you can link the note to the properties by choosing the Link to Property option in the PropertyManager for that note, as shown in the next image.
Several tools are available to assist with modifying or creating sheet format files. The Title Block Fields tool allows users to select specific notes and designate them as user editable title block fields. Users can also define tooltips for each title block field. After defining these fields, a Title Block Table appears under the sheet format for that sheet in the drawing tree. To enter title block data, right-click the title block table listing, and then choose Enter Title Block Data. This command highlights the editable text fields in the title block, and displays the tooltip when a user moves the pointer over that field.
The Automatic Borders tool allows quick and easy creation of drawing borders. It sets drawing zone quantities and sizes, and adjusts the border margins. You can also clean up the title block area with a selection of items you can delete.
After creating the sheet format file, it is best to save the file to a designated file location, much like template files. Sheet format files can be associated with and used within drawing templates. It is also possible to modify existing drawings to use new sheet format files. If the sheet format file is configured for a different paper size, you can change that option also.
Help Document: Customizing Sheet Formats
Standard Views
If typically using standard views on all drawings, it might make sense to add these standard views to the drawing template. This is possible using the Predefined View tool to insert views (Insert > Drawing View > Predefined). This places a view with a designated orientation and specified properties. You can create Projected Views from these predefined views.
To specify the model orientation as trimetric, dimetric or flat pattern. Click Predefined View or Insert > Drawing View > Predefined. In the PropertyManager, under Orientation, select either Flat pattern, Trimetric or Dimetric. If you then choose to make a drawing from a part or assembly (File > Make Drawing from Part or Assembly), SOLIDWORKS creates the drawing views automatically without additional input from the user. This can speed up the process of drawing creation.
Default Display Elements
The display of your drawings and models can greatly influence how easy or difficult it is to understand your design intent. Understanding the options that determine how display elements such as lines and markup appear is crucial to ensuring that communication of your concept is clear and concise.
Display Styles and Edge Display
There are several options in the System Options that control how models in drawings are displayed (Tools > Options > System Options > Drawings > Display Style). In the default installation, SOLIDWORKS uses the Hidden Lines Removed display style option. This display style hides any edges that are not visible from the view’s perspective. The following other display styles are also available:
The Wireframe option displays all edges in the model, regardless of perspective.
The Hidden Lines Visible option displays hidden edges in a dashed line style.
The Shaded with Edges option displays colored shading on model faces, along with edges that are visible from the view’s perspective.
The Shaded option displays colored shading on model faces without any edge display.
By default, the Tangent edges option specifies as Visible. Tangent edges are the edges formed where curved faces meet with faces of differing curvature or direction. You can also specify either the Removed or Use font options, which display the edges with dashed lines. When active, the Hide ends option under Use font hides the ends of the tangent edges.
Color Settings
From the Colors category of the System Options, you can also specify the colors of various elements. You can switch icons between the Default and Classic (pre-2016) icon colors, and also switch the color of the interface between Light, Medium Light, Medium and Dark. Various color schemes are available for selection, and these are further customizable by specifying unique colors for entities such as visible model edges in drawings or reference dimensions. It is easy to return to the default colors at any time by clicking Reset Colors To Defaults.
Other Document Display Elements
You can control other display elements, such as the thickness of various types of edges, the extension length of centerlines, the section view line style, etc., on a per document or per template basis by changing the document properties. Users can choose to insert certain types of markup automatically by adjusting the Auto insert on view creation options within the Detailing section of the Document Properties.
Default Graphics Settings for Optimal Performance
A good chef would never consider using a dull knife. The performance of our tools can greatly influence the quality of our work and the time needed to create it. If a CAD system is not performing to a high standard, it can be detrimental to the design process. By choosing the right tools and understanding the settings that allow these tools to perform optimally, you can ensure that your CAD system is performing at its best.
Supported Graphics Cards
SOLIDWORKS is an advanced 3D modeling application that makes use of workstation graphics cards to improve graphical performance when working in parts and assemblies. A list of supported graphics cards is available on the SOLIDWORKS Support website:
SOLIDWORKS Hardware Certification
SOLIDWORKS does not require these graphics cards to run, however the use of a supported graphics card leads to an improved user experience. Tasks such as rotating, panning and zooming are much faster and smoother with these graphics card. In addition, the appearance of models also improves when using a supported graphics card.
To ensure that your SOLIDWORKS installation is using your supported graphics card, open the System Options and select the Performance category. Within the Performance options, clear the check box for the Use software OpenGL option. This ensures that SOLIDWORKS is using hardware acceleration to drive the on-screen graphics.
Level of Detail
If you experience a slowdown when rotating larger parts or assemblies, consider moving the Level of detail slider further to the right for less detail and faster performance. Refer to the next image. This reduces the level of detail as the part or assembly rotates, pans or zooms. This is particularly helpful with larger assemblies, because the number of graphics triangles dynamically reduce when the Level of detail is set to Less (faster) SOLIDWORKS automatically sets the Level of detail slider all the way to the right when Large Assembly Settings are active. Large Assembly Settings are activated if an assembly’s component count is higher than the threshold specified within the Assemblies category of the System Options, or when a user activates them manually from Tools > Large Assembly Settings. If you are using a high-performance graphics card, you might want to consider moving the slider further to the left, or all the way off to preserve detail during view manipulation.
Enhanced Graphics Performance
Effective with the release of SOLIDWORKS 2019, the software adds an option for Enhanced graphics performance. Refer to the following image. This option takes greater advantage of modern, high-end graphics cards, which leads to dramatic increases in graphical performance when active. When activating this option, be sure to restart SOLIDWORKS to initiate the functionality.
If you notice jagged lines within your display area, you might also consider activating the Anti-alias option. You can activate this option from the Display category of the System Options. This option helps to smooth the appearance of edges and sketch entities. It is also possible to improve the display quality of the entire graphics area by activating the Full scene anti-aliasing option. To activate this option, you must first close all SOLIDWORKS documents. Restart SOLIDWORKS for this option to take effect.
Image Quality
For some users, round edges and edges of holes might appear blocky or polygonal. To improve the quality, increase the Shaded and draft quality HLR/HLV resolution from the Image Quality category of the Document Properties. Because this option is in the Document Properties, it applies only to the current active document. Users might consider changing this setting in their templates, so all new documents inherit the setting. Be aware that an increase in resolution might come at the cost of a decrease in performance.
CAD Administrators put a lot of work into determining the best setup for your team. This involves choosing the best tools, and optimizing those tools to ensure that they integrate seamlessly into your engineering and design process. When individual users begin to make changes to their options or modify shared files like templates, they disrupt the congruity of the CAD system. Fortunately, there are you can use to prevent such pitfalls.
Locking System Options
It is generally helpful to ensure that every SOLIDWORKS user is working with the same settings. This helps to promote consistency and standardization across designs and ensures that all users are taking advantage of uniform settings that drive performance and usability. One way to enforce this is to create an administrative image for client installations. This creates an easily deployable package, with the ability to deploy multiple clients automatically. When creating an administrative image, administrators have the ability to specify system options, and to lock certain settings. When users then view their system options, the locked settings display a lock icon.
Help Document: Applying and Locking Options
Controlling Write Access to Shared Files
To prevent changes by unauthorized users, it is a best practice to secure shared files such as templates and sheet format files. To accomplish this, set the files as Read-only. If the files are managed within a vault, you can modify the user and group permissions to allow only designated users to make changes.
SOLIDWORKS Toolbox
When creating assemblies, engineers want to focus on the overall form and function of their designs. While essential for an accurate bill of materials, no one wants to create fasteners, washers and other hardware from scratch. Having a library of these types of components can streamline the assembly process and ensure that designers spend more time optimizing the overall design.
Advantages to Using the SOLIDWORKS Toolbox Library
The SOLIDWORKS Toolbox is a library of common hardware, such as nuts, bolts, screws, bearings, etc. The SOLIDIWORKS Toolbox is included with the SOLIDWORKS Professional and SOLIDWORKS Premium software versions. The Toolbox helps prevent the need to manually create numerous types of hardware that are used common in assemblies. If your organization uses many different types of fasteners and assorted hardware, having an integrated library of these components can lead to a significant amount of timesaving.
There are distinct advantages to using the integrated Toolbox. When you drag a Toolbox component from the library into an assembly, SOLIDWORKS mates the Toolbox to the geometry on which it is dropped automatically. In addition, many Toolbox components change size automatically to match the mated geometry. If there is an update to the size of the geometry, the Toolbox component size also updates to match the modification in the geometry. You can also apply Custom Properties, such as part numbers, per each size of each component within the Toolbox database. This is helpful in streamlining documentation such as bills of material.
Help Document: SOLIDWORKS Toolbox Overview
Creating Custom Non-Toolbox Hardware Libraries
The Toolbox is not necessarily suitable for everyone. If your organization uses only a small handful of different fasteners and assorted hardware components, it might make more sense to store these components in your own custom-shared library. Some manufacturers and suppliers of hardware provide 3D CAD models of their components; however, you should take care to remove excessive detail when present in these fasteners. The complexity of some of these CAD models can lead to considerable slowdown when many are present in an assembly.
Sharing and Protecting the Toolbox Library
Similar to Document Templates and other shared libraries, it is a good practice to share the SOLIDWORKS Toolbox library with users across an organization. This ensures that everyone is working with the same hardware, and that custom sizes become available to everyone whenever they are used within an assembly. The Toolbox location is specified during the SOLIDWORKS installation. Subsequent user installations can then be set to use the existing Toolbox. Administrators might also consider imposing read-only access to the Toolbox library to prevent unauthorized modification, creation or deletion of hardware components.
Help Document: Toolbox Administration Overview
Managing the Toolbox Library Within SOLIDWORKS PDM
When in use, it is a best practice to configure the SOLIDWORKS PDM software to manage the SOLIDWORKS Toolbox library. This allows the same version and revision control that applies for any file within the PDM vault, and allows administrators to limit access and permissions on the Toolbox library. Other benefits include the ability to add missing Toolbox components to the vault and the creation of references (such as Where Used or Contains) between Toolbox components and SOLIDWORKS assemblies.
SOLIDWORKS Logs
Log files are one of the most useful tools in a CAD administrator’s toolbox. They can be invaluable when it comes to troubleshooting potential issues with performance or functionality. They can also help administrators track when and how users are utilizing the software and available licenses. SOLIDWORKS provides numerous logs that detail performance, usage and utilization.
Installation Manager Log
The SOLIDWORKS Installation Manager creates these logs whenever the SOLIDWORKS software is installed or updated. These logs can be helpful in troubleshooting errors and problems with the SOLIDWORKS installation.
The installation logs are typically stored in the following location:
%SystemDrive%:\Users\%username%\AppData\Roaming\SOLIDWORKS\Installation Logs\%installed_version%
To view these files, users might need to activate the Hidden items option in Windows® File Explorer:
The installation logs in the specified directory are usually sufficient for troubleshooting installation problems. However, if you need more information, additional logs with more details are available within the \Other Logs subdirectory.
Performance Log
The SOLIDWORKS Performance Log is typically available in the following location:
%SystemDrive%:\Users\%username%\AppData\Roaming\SOLIDWORKS\SOLIDWORKS %release%
The performance log contains information about your current or last running session of SOLIDWORKS. These logs can be helpful when troubleshooting instances where SOLIDWORKS closes unexpectedly, or when you experience other behavioral problems with the application.
Journal File
The SOLIDWORKS Journal File is located within the same directory as the performance log. The journal file records all actions taken within the application. This log is helpful when recreating or investigating steps that lead to an unexpected closure.
You can gather these logs manually and forward them for technical support. Alternatively, SOLIDWORKS packages the journal file, performance log and many other files into a zip format file when using SOLIDWORKS Rx to create a Problem Capture. This provides a self-contained archive file that you can send to support when troubleshooting problems.
SolidNetWork License Manager Server Log
When using a SOLIDWORKS Network License Server for SOLIDWORKS licensing, there is a log file specific to the SolidNetWork License Manager. To access this log from the SolidNetWork License Manager Server application, click View Log. This opens the log file, which displays the license usage information. Administrators can view which licenses are checked out to which users, and on which systems. These entries are also have timestamps that allowing administrators to see the duration of each SOLIDWORKS session.
File Management
Your SOLIDWORKS files are the culmination of hours, days and sometimes years of hard work. They contain the intellectual data of your organization and are one of the most important resources. Therefore, managing this data should be subject to the utmost attention to detail, just like the designs they represent.
File Associations
SOLIDWORKS is a fully associative application. This means that assemblies and drawings reference part files. If a drawing or an assembly contains a part, and if there is a modification to that part, that modification then appears in the associated drawing or assembly. While this makes it easy to keep everything up to date with design changes, it can present some challenges when it comes to file management.
Warnings About Moving Files
Typically, users manage non-CAD files by simply organizing them into folders, and it is not uncommon to move or copy files from one folder to another. In SOLIDWORKS, this is not a recommended procedure. If a SOLIDWORKS assembly or drawing references a part file that has moved, the user receives a prompt to locate that file. In assemblies with many components, this can become disastrous if too many files are moved.
Unique File Naming
Another recommendation is to use unique file names for SOLIDWORKS documents. For example, if two assemblies are open, and they both reference unique parts that share the same file name, SOLIDWORKS cannot open the second file name instance as a unique part.
If an assembly build contains parts from multiple folders, it can sometimes be difficult to track down the locations of all those parts without opening each part individually. Fortunately, the Find References tool makes it easy to view the file locations of every part reference within the assembly (File > Find References).
Pack and Go
Pack and Go is another tool that can help manage moving and copying SOLIDWORKS drawings and assemblies. Pack and Go allows users to copy a drawing or assembly file to a folder or a zip file, along with all of the referenced part and assembly files also. Pack and Go can also include additional files, such as drawings, toolbox components and simulation results. There is also an option to add a prefix or a suffix to all files, as well as the ability to flatten the folder structure for additional simplification.
The ability to add a prefix or suffix to the file name allows users to create copies of existing parts, drawings or assemblies, with new, unique names. This preserves the original documents, and you can modify the newly copied files without affecting references to the originals.
When deciding whether to apply pack and go functionality to a zip file or a folder, you should consider the use case. If the purpose of the pack and go operation is to send the package document to a collaborator for design review or modification, use of a zip file simplifies the process by producing a single file with a smaller file size. This is also the best option for sending a drawing or assembly to a Value Added Reseller (VAR) for technical support. If you only need to copy a drawing or assembly to a new location, a folder is often the better option.
SOLIDWORKS File Utilities
The SOLIDWORKS installation includes the SOLIDWORKS File Utilities tool, which can help users with file management while updating assembly and drawing references. This tool adds options to the right-click shortcut menu within Windows File Explorer. From the SOLIDWORKS category in the shortcut menu, users can choose the Open, Pack and Go, Rename, Replace, Move or File Locations file options. When using the SOLIDWORKS file utilities to perform any of these actions, the tool also updates the file references within the associated SOLIDWORKS files.
Help Document: SOLIDWORKS File Utilities
External References
In addition to the standard file references that exist between parts, drawings and assemblies, it is also possible to create external references. These external references create dependencies between files. As an example, when a part is created in the context of an assembly, and the new part uses edges or sketches of an existing part, that new part will have a dependency created using an external reference back to the assembly and the component to which that reference was established. To determine which files have external references, you can right-click the part name at the top of the SOLIDWORKS FeatureManager Design Tree and choose External References.
If a part has an external reference that is out of context, meaning the reference file it is dependent upon is not loaded into memory, it is possible to load the file by right-clicking the feature with the external reference and choosing Edit In-Context.
Help Document: External References
Important and Recommended Document Properties
After optimizing the sheet format layer and title block for your organization, the next aspect of managing templates is to ensure that the templates use the proper document properties. These properties save into the template, and control several different characteristics, depending on the type of file or template.
The Document Properties section of the SOLIDWORKS Options is broken into numerous categories that contain many options that apply to those categories. These categories are specific to the type of document (part, drawing or assembly) that is open. It can be challenging to determine which category and option is best for your particular use case. Fortunately, after taking a closer look, it is not as daunting as it may seem at first.
Drafting Standard
The properties in the Drafting Standard category are easy to set because your region or industry typically dictates the options you select. In addition, if your organization mandates the use of all uppercase letters on notes and dimensions, etc., you should activate these options.
Annotations
This section is specific to the style for annotations. As a best practice, specify the overall annotation options to use the preferred font for your organization. You can also change leader attachments to match your company’s style. Expanding the annotations options reveals additional items that you can customize to match the preferred appearance and functionality for your organization.
Dimension Options
It is also possible to customize general dimension options. You can define a specific Font for dimensions, and you can control the decimal precision for units, tolerances, and for dual dimensions. In addition, the fractional display is customizable to match your preference. Finally, you can also specify leading and trailing zeros.
If you do not want to include parentheses on reference dimensions, make sure to turn off the Add parentheses by default option. Additionally, activating the Center between extension lines option can help improve the organization of dimension layout on drawings. It is also a good practice to activate the Show dimensions as broken in break views option, because this helps prevent confusion about break view dimensions. Expanding the Dimensions options allows users to customize settings for each specific type of dimension.
DimXpert Options
When it comes to DimXpert dimensions, it is important that the Base DimXpert standard option match the overall drafting standard of the document. Once specified, you can dive deeper into the types of tolerance, whether it is a block tolerance or a general tolerance. You can specify different tolerance types for different dimension types. To prevent redundancies in DimXpert dimensions, make sure that the Eliminate duplicates option is active in the Display Options for DimXpert dimensions.
Unit Options
In the Units category, specify the Unit system according to your dimension standard. You can also specify either the default precision, or the number of decimal places for each unit type. It is also good to specify the Decimal rounding options to an agreed standard.
Image Quality
Image Quality should be set to provide smooth edges without sacrificing view performance. If zooming, panning and rotating a model is too slow, consider moving the sliders lower for the Shaded and draft quality HLR/HLV resolution option and the Wireframe and high quality HLR/HLV resolution option.
Automatic Update of BOM and Hole Tables
To ensure that bill of materials (BOM) tables update automatically, activate the Automatic update of BOM option from the Tables > Bill of Materials section of the Document Properties. This applies to hole tables as well; therefore you should activate the Automatic update of hole table option also.
Automatic Insertion of Annotations
It can be helpful to insert certain types of annotations and markup automatically when creating or inserting a view. The Detailing section of the Document Properties allows users to change the settings to specify that items such as center marks for holes, fillets and slots are inserted automatically. In addition, you can import dimensions marked for drawing into views automatically. This prevents the need to perform this action by using the Model Items tool after inserting a view.
Using SOLIDWORKS Rx
When working with complex systems, it is important to have a tool to help with diagnostics. Auto mechanics might have an OBD II code reader that provides additional information about what is happening within the automotive system. Similarly, SOLIDWORKS Rx enables users to dive deeper into their SOLIDWORKS maintenance, performance and diagnostics.
System Maintenance Tools
SOLIDWORKS Rx is a multipurpose tool that is a component of the SOLIDWORKS installation. SOLIDWORKS Rx allows users to view diagnostic information about their system and their software installation. It also provides quick and easy access to common system maintenance tools.
Users can clean up their backup and temporary directories, for both SOLIDWORKS and Windows. It also provides quick access to the hard drive diagnostic tools built into Windows.
Problem Capture
Perhaps the most important capability of SOLIDWORKS Rx is the Problem Capture tool. This allows users to record a problem that they are having with their installation, or with a SOLIDWORKS file. They can then package this recording, along with SOLIDWORKS logs, into a self-contained zip format file. This makes it very convenient to send the requisite information to their VAR for technical support.
Reliability Report
The Reliability tab displays a report that tracks SOLIDWORKS sessions and how the method of closure. It also tracks Windows events collected before a closure. This information can be helpful in tracking unexpected closures of the SOLIDWORKS software and the log entries associated with them. This pattern information can also be helpful when troubleshooting installation or behavioral problems.
Benchmark Tool
Finally, there is a Benchmark tool, which allows users to benchmark their system performance and compare their scores with other customers. This can help determine whether a hardware upgrade is necessary, and can indicate areas where improvements are possible.
Using Performance Evaluation
While SOLIDWORKS Rx serves as a diagnostic tool that provides information about your overall SOLIDWORKS installation, the Performance Evaluation tool (Tools > Evaluate >Performance Evaluation) is invaluable for analyzing assembly performance, particularly on larger or more complex assemblies. If an assembly is performing slowly, or rebuild times are long, the tool can help determine exactly what might be causing the problem. It offers statistics about the performance of the assembly as well as the assembly’s attributes.
Open Performance
The first section details the Open Performance. This provides a full detailed list of how long it took to open each individual part and assembly file within the top-level assembly, in order from longest opening time to quickest. Clicking the Show These Files link displays a complete list of the files, configurations and the open time. You can print, copy or save the list for reference. You can also open individual files by selecting them in the list and clicking Open.
Help Document: Performance Evaluation for Assemblies
Display Performance
Display Performance indicates the number of graphics triangles contained within each part in the top-level assembly. More complex geometry or components with excessive detail contain a higher number of graphics triangles, which can significantly affect assembly performance. For components with many graphics triangles, it might be helpful to create a simplified configuration for use within the top-level assembly if the full level of detail is not required.
The Rebuild Performance section indicates how many mates are evaluated when the assembly is rebuilt, as well as a report of the last assembly rebuild.
Settings Performance
The Settings Performance indicates whether specific options are active for the open assembly. If the Verification on Rebuild option is active, Performance Evaluation flags this option in the report. While Verification on Rebuild can help ensure the integrity of components and the assembly, it influences performance. It also specifies whether the number of components is large enough to trigger Large Assembly Settings automatically, and indicates whether Large Assembly Settings are active.
Statistics
The Statistics section shows the total number of components in the assembly. The report further shows more detailed information, such as the number of unique part files, bodies, subassemblies, etc.
While there are other third-party benchmark tools available to measure general system performance, the SOLIDWORKS Benchmark Test analyzes performance specific to functionality in SOLIDWORKS. The results are useful to establish a performance baseline and allow administrators to compare performance across multiple workstations. The results also allow administrators to determine if any upgrades are required.
Be aware that when running the benchmark test, it is best to restart your computer and make sure no unnecessary applications are running. This helps ensure optimal performance and yields the best results.
Help Document: Benchmarking Your Hardware
Processor Performance
The Processor performance results indicate how the CPU will handle most common SOLIDWORKS tasks, such as rebuilding parts and assemblies. Many processes in SOLIDWORKS use a single core. Typically, a higher single core performance yields better results than higher multicore performance.
Graphics Performance
The Graphics performance results indicate how well the system will handle common viewing tasks, such as rotating, panning and zooming in parts and assemblies. Larger models and assemblies are more taxing on the graphics card during these actions, and higher graphical performance yields smoother and faster results. The graphics performance can also have a significant effect on the rendering time in SOLIDWORKS Visualize.
I/O Performance
The I/O performance score directly relates to how long it takes to save and open files on your system’s hard disk drive. This score improves significantly with the use of solid-state drives.
Rendering Performance
The benchmark test only evaluates the rendering performance if PhotoView 360™ is installed. PhotoView 360 is one of the SOLIDWORKS applications that makes use of multiple processors or cores, and therefore performance improves if they are present.
RealView Graphics Performance
The RealView Graphics Performance score is only available if your system has a supported graphics card installed. This score indicates how well your system performs in the same graphical viewing tasks from the previous section when the RealView Graphics mode is active. Both the graphics card and CPU can affect the score, but the score leans more toward the graphics card when the RealView Graphics mode is active.
Simulation Performance
The Simulation performance results are only available if SOLIDWORKS Simulation is installed. The SOLIDWORKS Simulation software also uses multiple processors, and therefore multiple processors or cores help improve performance. A solid-state drive might also improve performance because SOLIDWORKS Simulation frequently writes computation data to the disk.
CAD Admin Dashboard
The CAD Admin Dashboard is a useful tool that allows administrators to keep track of how their SOLIDWORKS licenses are used. The Cad Admin Dashboard also provides statistics that pertain to the registered systems. You can access the CAD Admin Dashboard through the SOLIDWORKS Support page or go directly to the CAD Admin Dashboard.
To access the CAD Admin Dashboard, you must be the administrator for your organization. Specifically, you must have the Security Admin role as defined in the DSx.Client Care and Order system. If you are the administrator and do not have the Security Admin role, request that your Support Partner or Reseller grant you the role.
Help Document: SOLIDWORKS CAD Admin Dashboard
User System Accounts
The CAD Admin Dashboard shows a list of all user system accounts that are registered to each SOLIDWORKS license. By clicking the plus (+) icon in the first column, administrators can view the system information at a glance. The system information includes the system brand, the installed operating system, the RAM capacity, the installed graphics card and graphics driver. Administrators can also see summaries of the Rx Benchmark tool, recent Session Details, which service pack is installed and whether the graphics driver is supported. You can filter accounts using several different parameters, and can group accounts based on the office location, user type and other criteria. It is also possible to red flag an account based on specific conditions such as an unsupported graphics driver, the Rx benchmark score or other nonconforming system options.
System Options
When you select an account, additional details become available. The System Options are broken down into categories, and administrators can view what options are set on that system. They can also select a system to serve as the baseline for the system options, and then filter any systems that differ from that baseline. This is a helpful way to ensure that everyone is using the same system options and enforce standardization.
Machine Details
The Machine Details are also available seen in greater detail. This section lists the same specifications mentioned earlier, and also indicates the processor, the computer model and the Windows Experience Index score. If you have run the Rx Benchmark, those results also appear in greater detail on the Rx Benchmark tab.
Session Details
The Session Details tab shows the start time of each recent session, as well as the total duration of the session. The sessions are color-coded to indicate sessions that terminated normally by the user, terminated by the user ending the application or terminated unexpectedly.
You can export much of the data in the CAD Admin Dashboard to the CSV or Excel® file formats. This can be helpful in keeping records of user accounts, as well as how licenses are being used.
3DEXPERIENCE Platform for SOLIDWORKS
This section describes the vital settings for customers who plan to use the 3DEXPERIENCE platform. For those who are not familiar with the benefits of using the 3DEXPERIENCE platform, consider reading the following article to learn more about its advantages. The article provides valuable insights into the essential configurations and settings required for a better 3DEXPERIENCE implementation.
Web Page: Focus on Design with Cloud Services
Familiarity with SOLIDWORKS
As you explore the 3DEXPERIENCE platform, it is essential to ensure that you have the right tools, knowledge and access in place. It is also vital to have an understanding of the SOLIDWORKS application.
Access to the 3DEXPERIENCE Platform
The first step to experiencing the power of the 3DEXPERIENCE platform is to gain access. If you do not have an account yet, contact your organization’s system administrator or your VAR. Ensuring a smooth onboarding process is helpful to setting yourself up nicely on the path to using the collaborative capabilities and advanced features of the platform.
System Requirements
Make sure that your system meets the minimum requirements to run the 3DEXPERIENCE platform effectively. Review the hardware, operating system compatibility and internet connectivity specifications on the Certified Workstations web page. It is also a good practice to use the Cloud Eligibility Tool to ensure that your hardware and software configurations meet the specifications of the platform to guarantee optimal performance and user experience.
Familiarize Yourself with 3DEXPERIENCE Terminology
The 3DEXPERIENCE platform introduces new concepts and terminology that might differ from what you are used to in SOLIDWORKS. Therefore, it is important to familiarize yourself with these new terms, such as Roles and Apps. Roles are collections of various Apps, while Apps provide the functionality. It is up to you to decide which Roles and Apps you need, so you can select what you want for now, and grow as you go. Understanding these concepts helps you navigate the platform with confidence.
To help you navigate the platform effectively, the recommendation is to invest time in the training that is available on MySolidWorks.
Hardware and Network Considerations
Platform Eligibility Checker
The Cloud Eligibility Checker is an online tool available for download to check the compatibility of their environment with the 3DEXPERIENCE platform on the cloud. Ensure that all fields in the status column are green (OK). If required, apply the guidelines that the tool suggests. For more information, see the following documentation:
SOLIDWORKS System Options
3DEXPERIENCE Integration
The 3DEXPERIENCE Integration system options make SOLIDWORKS files compatible with the 3DEXPERIENCE platform.
For migrating data to the 3DEXPERIENCE platform, it is a recommendation that you update the SOLIDWORKS settings to be upgraded to the latest configuration manager that is compatible with the 3DEXPERIENCE platform.
To update SOLIDWORKS files for compatibility with the 3DEXPERIENCE platform, click Tools > Options > System Options > 3DEXPERIENCE Integration > Update.
Note: You can only activate this option when no sessions or files are open.
The following changes occur when you update the model:
The custom properties and configurations align with the 3DEXPERIENCE platform.
The Configuration Properties and Properties Summary tabs in the Properties dialog box manage the custom and configuration-specific properties.
In the ConfigurationManager, the CAD Family tab, assemblies and parts appear as CAD family objects. Configurations appear as physical products and representations.
For SOLIDWORKS models that have multiple display states, the active display state is assigned to the physical product. When you insert a component into an assembly, the component uses the display state assigned to the physical product.
Note: After applying the option and making changes, you cannot undo the updates by deactivating the option.
For more information, see the following documentation:
In the SOLIDWORKS® 3D CAD software, what are the '3DEXPERIENCE Integration' options and what are the benefits of using them? (QA00000300960)
https://r1132100503382-eu1-3dswym.3dexperience.3ds.com/#community:52/wiki:Y639fc2yRLanqvrrN8N82g
File Locations
Design Library
The SOLIDWORKS Design Library tab in the SOLIDWORKS Task Pane provides a central location for reusable design elements such as parts, assemblies and sketches. Customers that adopt 3DEXPERIENCE can store their Design Library parts and assemblies in a collaborative space, and organize them using a bookmark structure. This is called a Connected Design Library and it appears in the Task Pane with a blue library icon.
Help Document: Connected Design Libraries
SOLIDWORKS Templates
Information about the SOLIDWORKS templates appears in section 3 of this document. However, the 3DEXPERIENCE platform presents a different approach to creating and saving the templates.
SOLIDWORKS templates are the method of enabling all users at a company to work together using consistent SOLIDWORKS settings and defined drawing standards. For existing SOLIDWORKS customers who adopt 3DEXPERIENCE, storing templates in the platform allows them to maintain that consistency of settings and standards with some added benefits.
Create Template
3DEXPERIENCE users can create templates for the 3DEXPERIENCE platform directly from SOLIDWORKS in the following way:
Open a SOLIDWORKS part, assembly, drawing or template that you want to save as a template.
Go to File > Save as Template.
Enter a Title and Description.
Save the template with one of these options:
Create As Released - Creates template in the Released state. You cannot modify a template in this state.
Create As Private - Creates the template in the Private state. You can modify a template in this state.
If a template file already exists in 3DEXPERIENCE, all Save commands open the Save Template dialog box. Silent saving is not supported for templates.
Change the Title and the Description.
Save the template modifications.
Reset the fields to the default value.
After saving the template in 3DEXPERIENCE:
MySession refreshes and shows the 3DEXPERIENCE information that relates to the template.
The template file becomes available in the New SOLIDWORKS Document dialog box from SOLIDWORKS File > New, under the 3DEXPERIENCE tab.
After saving to 3DEXPERIENCE, you can revise and modify the templates. Who can make a modification and when depends on a users’ collaborative space permissions and the maturity state of the template. You can delete templates from a collaborative space using the same methods as a physical product using either the 3DSearch, Bookmarks Editor or Collaborative Lifecycle widgets.
For more information and guidance about this topic, see the following 3DEXPERIENCE documentation:
List Other File Locations Now Supported in 2023x FD03
In earlier product versions, administrators had no way to share SOLIDWORKS resources (non-CAD files) with users using the platform tools. However, 3DEXPERIENCE customers can now upload and manage those resources as documents in the Bookmark Editor. For collaboration, a person or team can upload and bookmark the documents for all SOLIDWORKS users on the platform to share.
When adding a folder for a SOLIDWORKS file location, each SOLIDWORKS user can browse from 3DEXPERIENCE and pick the bookmark that contains the content type they want. After selecting the bookmark, the bookmark appears in the File Locations options and the content downloads to a local folder for use by SOLIDWORKS.
Go to Options > System Options > File Locations.
Select Sheet Metal Bend Table > Add Location > and choose Select From 3DEXPERIENCE.
Select the applicable bookmark. The bookmark appears in the file location for Sheet Metal Bend Table.
Be aware that the Select from 3DExperience option is only available for the file location that supports bookmarks. In earlier versions, the Design Library was the only file location that supported bookmarks. For now, the following file location options support this option:
Bend Table Template
Blocks
BOM Templates
Custom – Appearances
Custom - Decals
Custom - Scenes
Design Library
Dimension/Annotation Favorites
Drafting Standards
Hole Table Templates
Hole Wizard Favorites Database
Macros
Punch Table Templates
Revision Table Templates
Sheet Formats
Sheet Metal Bend Tables
Sheet Metal Gauge Table
Title Block Table Template
Weld Table Template
Weldment Cut List Templates
Weldment Profiles
Weldment Property File
Structure System – Connection Elements
You can also update the local content if the bookmarked content in 3DEXPERIENCE changes. The update function becomes active when you select a folder that is a bookmark path. To verify the local content with the content in the 3DEXPERIENCE platform, click Update and go to Update File Location from Bookmark.
The SOLIDWORKS MySession settings provide the ability to configure the open and save behavior on each workstation. To enhance the user experience and productivity, users should have information about these options and their significance.
When teams work together on the same project, you can activate the collaborative environment settings through MySession > Options, to avoid unexpected behavior.”
The MySession options appear on the Tools tab of the MySession Action Toolbar.
The following two graphics provide an explanation of the recommended MySession option settings.
Save Options
Saves the graphical properties that relate to an assembly. For example, hide or show state and transparent of components.
When you choose to create a new revision after saving a part, assembly or drawing, the old revision is automatically replaced with the new version in the SOLIDWORKS session. It is a recommendation to activate this option unless there is a specific reason not to.
Open Options
The assembly open mode dialogue box appears when opening an assembly from 3DSearch or the Bookmark Editor in MySession. This is a recommendation for users who work with large assemblies. The Open Mode functionality is only available for SOLIDWORKS connector.
A warning appears if multiple revisions of the same component exist in the assembly structure.
For more information about the MySession options, see to the topic “Options Dialog Box in the Tools Tab” in the 3DEXPERIENCE online documentation.
Also see the SolidPractices document: –“Best Practices for Implementing 3DEXPERIENCE for SOLIDWORKS Users”. This document describes various aspects that require consideration when SOLIDWORKS users implement the 3DEXPERIENCE platform. This guide provides important information and encourages further investigation through links to other topics and relevant SolidPractices documents.
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 DS SOLIDWORKS Corp.
