Revision History

Note

All SolidPractices are written as guidelines. You recommend using 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 SP0.1 and 3DEXPERIENCE R2023x GA. If you have questions or need assistance in understanding the content, please get in touch with your designated reseller.

Acknowledgments

This document was authored by TriMech Solutions reviewed by DS SOLIDWORKS.

Preface

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

• Hardware specifications
• Software configurations
• User knowledge and modeling procedures

This SolidPractices document focuses on modeling procedures. It includes recommendations for CAD designers relative to the tools and techniques for maximizing efficiency when creating 3D part and assembly models.

Your Feedback Requested

We would like to hear your feedback and suggestions for new topics. After reviewing this document, please take a few minutes to fill out a brief survey. Your feedback will help us create the content that directly addresses your challenges.

Design Intent

Some people say that they “design in SOLIDWORKS”. However, the product design is often already complete before they begin creating the model. Therefore, it is important to differentiate between two fundamental activities: designing and modeling; and observe how each can influence the other.

While you can create the design independently of the CAD tool, the process of generating the actual shape and properties of the final product involves performing the activity of modeling in SOLIDWORKS.

A good example is if the design of a product is already documented in a printed 2D drawing and a SOLIDWORKS user must recreate the product as a 3D model. Because SOLIDWORKS is a user-friendly design software, it offers many different methods to achieve the same result. However, this can also create challenges when a change in design occurs.

Depending on how the 3D model was built, a revision of the model can happen in a matter of seconds by modifying a small number of parameters. It can also take days if the model requires extensive editing. To minimize the editing effort, it is critical for the user to foresee the possible changes in design and build the 3D model accordingly by taking advantage of the parametric capabilities of the software.

The most efficient users know how to Model for Change, a concept otherwise known as Design Intent. The Design Intent is the plan of how the model should behave after the change.

The following sections of this document describe several tools and techniques for capturing the design intent including:

• Sketch relations
• Sketch dimensions
• Start and end conditions for features
• Pattern settings
• Equations
• Mating schemes
• Base part technique (aka Skeleton sketch)
• Envelope Publisher
• Configurations

Example of Observing the Design Intent

The two parts in Figure 1 are identical. Both were created based on Revision 0 of the same design. Even the features in the FeatureManager® design tree (FeatureManager) are identical, but the design intent is different.

command. Therefore, the holes are always located ½” from the edges of the plate.

On the right, the location of the hole centers depends on multiple dimensions including:

• The right edge of the plate
• The bottom edge of the plate
• The horizontal distance between holes
• The vertical distance between holes

Now imagine that there is a revision to the design and in Revision 1, the height of the part increases from 4” to 5”. When changing only the height dimension, the result is as depicted in Figure 2.

In summary, it is critical for all users who work on the same project to be aware of what the design intent is for each specific product or family of products to maximize their efficiency when:

• Iterating the design during the conceptual phase
• Editing the model during revisions
• Configuring the model

Users who attend the SOLIDWORKS training courses have a major advantage in this area compared to self-trained users.

Tailoring the User Interface for Maximum Performance

SOLIDWORKS makes sure that the tools users require are available in multiple places within the user interface (UI). This allows users to exercise their own personal preferences on which parts of the UI to use for accessing the tools. You can access the same tool or action from:

• Top menus
• Context (right-click) menus
• Individual toolbars
• CommandManager
• Keyboard shortcuts
• Context toolbars
• Shortcut bar (press the s-key)
• Mouse gestures
• Cursor feedback
• Breadcrumbs
• Command search

Most users like icons and they use the individual toolbars and the CommandManager extensively. This gets the job done, but has two major disadvantages:

• Unproductive time spent moving the cursor from the model to the edges of the monitor and back thousands of times daily.
• Repeatedly looking away from the model to hunt for icons.

The second consideration is the most damaging, not only to the users’ productivity, but also to their wellbeing. Every time the focus switches from the model to the sides of the screen, users get distracted. Depending on how long the interruption lasts, this affects the users’ flow of thoughts to the point that they may put more effort into remembering the next steps in the design or modeling process.

In this section, the recommendation is to use an efficient workflow that combines several tools and techniques for staying “in the flow” when modeling.

The result is working as much as possible in the graphics area while refraining from accessing the CommandManager or the FeatureManager. When users master such a workflow, their attention is 100% focused on the model and their next steps in the design process.

To help illustrate the difference between the traditional technique and the “in-the-flow” method, consider the following example. Two users have an assignment to model the part from Figure 3 and they record their mouse movements on the screen. They were asked to work at their normal speed.

method, which takes advantage of the tools that appear on-demand near the cursor, which allows them to keep their eyes on the model (Figure 5).

• It is possible to reduce mouse movement by 75%. While the first user’s mouse travels 2.8 km during one day of work, the second user moves the mouse only 0.9 km.
• During one workday, the second user saves almost an entire hour (56 minutes), which could have been used to perform design activities instead of modeling.
• The first user is repeatedly distracted by having to hunt for icons. In time, the fatigue caused by these micro-distractions accumulates and the user loses focus.

workflow is quick, highly visual and effective. The good news is that you can modify the workflow as you prefer. Some users prefer to remember a large number of keyboard shortcuts. Others spend a lot of time training their hand to master 48 mouse gestures. Instead of trying to remember keyboard shortcuts or mouse gestures, some users prefer using icons in the UI to access functions.

This section describes a balanced method that is easy to learn and takes advantage of a limited set of tools and techniques:

• Context toolbars
• Shortcut toolbar
• Cursor feedback
• A limited number of keyboard shortcuts
• A limited number of mouse gestures
• Breadcrumbs

Breaking old habits is hard. The best way to master this method is by practicing the use of these tools in the order described below, by including the use of one new tool every day. In less than a week you will be modeling in-the flow.

Preselect Entities and use Context Toolbars

To show context toolbars on selection, go to Tools > Customize and activate the option shown in Figure 7.

In the context toolbar, the SOLIDWORKS application displays the commands available that you can apply to the selected entities.

For example, if you want to start a new sketch on an existing model face, simply click the model face and a toolbar appears next to the cursor. The Sketch icon is less than 1 cm away from your cursor. Figure 8 demonstrates the differences in the content of the context toolbars for:

• Parts
• Sketches
• Sheet metal
• Assemblies

Pay attention to your workflows and identify the icons you use the most. Once you identify a repetitive command, add the icon for that command to the context toolbar.

The good news is that you can customize these toolbars. To start the customization process, right-click a context toolbar and then click Customize.

dialog box (Figure 10). Aside from the grey icons, everything else is customizable. field (Figure 11).

The shortcut toolbar also appears near the cursor when you press theskey (if you use the default keyboard shortcuts).

To start customizing the shortcut toolbar presss, right-click the toolbar, and then clickCustomize.

• Part
• Assembly
• Drawing
• Sketch

• Make the toolbar as square as possible to minimize mouse movement.
• Use individual icons (not flyout buttons) for commands that you use the most often. For example, Line and Centerline (blue border).
• Move the most commonly used icons near the top left corner (red border).
• Add icons for Point, Mirror Entities, Bosses and Cuts (orange border).

Once you input the settings for a command, do not move the mouse but look for the cursor’s feedback. If you see the icon of a mouse next to the cursor, pay attention to what activities you can complete by pressing the right mouse button. Users can save a tremendous amount of time when performing repetitive tasks by simply right-clicking to complete the command.

Right-Click Context Menu

The right-click menu is also context-sensitive. If you preselect an entity, the menu appears below the context toolbar. Otherwise, it appears near the cursor.

Figure 15 shows three use cases* for the mouse:

• To define the end-conditions for a Boss-Extrude feature.
• To control the termination of chains or the auto transition between lines and arcs in the sketch environment.
• To apply the Copy with Mates command on preselected components.

*Images in sequence from left to right.

You can optimize your focus on the model by pressing D (default keyboard shortcuts) to bring the confirmation corner or the breadcrumbs next to your cursor.

Figure 16 shows the confirmation corners next to the cursor for:

• Sketch
• Feature
• Edit component

For light users of the Mouse Gestures options, use 2 Gestures (Horizontal) wheels to program the OK and Escape keys on the left and right directions.

Practice Advice

After customizing the tools mentioned in this section, for practicing purposes you can temporarily hide the CommandManager (F9) and the FeatureManager (F10). F9 and F10 are keyboard shortcuts that toggle on and off the visibility of these two UI features.

Best Practices for Sketching

It is incorrect to state that there is a good way and a bad way to use sketches, because use cases are best determined by the type of product, job and workflow that is specific to each company or each design team. That is why SOLIDWORKS offers so much freedom in how you create and use sketches.

Typical Use Cases for Sketches

It is beyond the scope of this article to cover all the possible use cases for sketches. In any part or assembly model, you can use 2D and 3D sketches to perform one or more tasks, including:

• Establishing design intent
• Defining 3D features
• Using as reference geometry
• Converting 2D DWG to 3D SLDPRT files
• Adding mates in assemblies
• Using as reference for detailing drawings

How Sketches Are Solved

To solve a sketch, the software creates a system of equations that account for all entities, relations and dimensions in the sketch, and solves them all simultaneously. That explains why adding one more element in the sketch increases the complexity of the equations exponentially.

2D versus 3D Sketches

While 2D and 3D sketches seem to share most tools (such as the line icon), internally, they use distinct solving engines.

A 2D sketch deals with two translational axes and one rotational axis.

A 3D sketch has three translational axes and three rotational axes, which increases the number of variables multifold. In addition, having an extra direction in the three-dimensional space adds several orders of magnitudes to the complexity of the matrix, as described in section 4b. This explains why, from a pure performance point of view, 2D sketches are preferable whenever possible.

12 Simple Rules for Efficient Sketching

Because this article primarily applies to using SOLIDWORKS at the team level, it is critical to emphasize three factors that can affect the efficiency of the team:

• Clarity
• Modularity
• Fast editing capabilities (including design intent changes)

From this perspective, when using sketches for the two main purposes (defining design intent and building 3D features), consider the following best practices.

1. Use simple sketches

As mentioned in section 4b, increasing elements in the sketch directly affects the solving performance of the sketch.

Therefore, the recommendation is to use simple sketches, which improves performance and has the following advantages:

• Easy to understand by other users
• Promote modularity
• Easy to document
• Minimize the occurrence of errors
• Easy to troubleshoot
• Easy to edit
• Easy to configure

1. Make use of the origin and the major planes

The origin and the three major planes are powerful reference geometry items. The main use cases include:

• Prefer sketching on the major planes to minimize the length of the chain of references (parent-child relationships) for your sketch.
• If there is any symmetry in your model, use the origin or the major planes as references.
• For base part (aka skeleton sketch or skeleton part) workflows, referring everything to the origin enables the creation of assemblies with no mates (fixes all components on the origin of the assembly).

1. Fully define sketches

Models that contain under-defined sketches are very dangerous. Uncontrolled and unexpected changes in the model geometry can occur when editing references. In addition, it is a bigger effort to check the validity of the final product because the checker can no longer verify that the designer followed the design intent. Ideally, it is best to use the minimal number of relations and dimensions to define a sketch. While it is true that SOLIDWORKS allows adding more than the required relations, without warnings or errors, doing so causes an increase in the sketch complexity. As mentioned earlier, a complex sketch takes longer to solve and is harder to revise and more cumbersome to troubleshoot.

1. Order of operations

When creating new sketches, the best workflow follows this order:

• Create the sketch geometry.
• If symmetry exists, use the Mirror Entities tool to save time and automatically apply symmetric relations.
• Add other sketch relations.

1. Finish by adding dimensions to fully define the sketch

Start by adding or editing the dimensions with the smallest value. Doing so prevents geometry overlap when editing dimensions.

Add relations as you sketch by taking advantage of inferencing lines. SOLIDWORKS can create relations automatically as you draw new sketch entities, allowing you to stay in the flow. For example, in Figure 18, a line starts from the left side of the circle. As the cursor moves over the circle, dotted inferencing lines appear, allowing you to apply one of these relations to the line and its endpoint automatically:

• Tangent line - circle
• Tangent line - circle and coincident line endpoint - circle
• Coincident line - center of circle
• Coincident line - center of circle and coincident line endpoint - center of circle

Example: In Figure 19, using the equidistant relation allows you to define a Hole Wizard sketch by one dimension. In this case, you do not dimension the distance between instances of the hole because that is not your concern. Your design intent is to ensure only that the holes have equal spacing.

A fully defined sketch is one in which the position of all entities is unambiguous. If you are unsure what relations or dimensions are required to fully define a sketch, drag the under defined entities to see how the geometry could change.

1. Fix errors as they occur

Many different workflows can produce errors and warnings in sketches because of actions taken by the current user or somebody else. Examples include:

• The current user:
  • Adds relations or dimensions that over define the current sketch.
  • Modifies sketches or features in the current model that serve as references in the current sketch, thus over defining the sketch.
• A different user edits other files that affect the current sketch. Example:
  • Features, sketches or mates in other models (parts or assemblies) that have references in the current model (external references).

It is critical that you fix such errors as soon as possible. When errors exist in the model:

• It takes longer to solve sketches.
• The resulting geometry may not be correct.
• More errors can occur in dependents (sketches and features).

Especially when the current user generates the error, it is critical to solve the sketch before saving and closing the file. The authors of the errors are the most qualified to fix them because they know what actions generate the errors. Fixing such errors at this time is a fast and painless process.

To enhance the troubleshooting process and speed up the error fixing, become familiar with tools like:

• Check Sketch for Feature Usage – When errors or warnings are not in the current sketch, but in the features based on it. Is the sketch geometry appropriate for dependent features?
• SketchXpert – Use to identify the reasons for over definition of a sketch.

1. Use the Shaded Sketch Contours setting to:

• Select all sketch entities bordering the shaded region with one click to instantly perform actions like:
  • Move entities in bulk with no distortion by dragging the shaded area.
  • Run the Offset Entities command.

• Troubleshoot open contours (Figure 21).

tool to preserve references to features and mates

When you want to delete one sketch entity and replace it with another, you often need to create a new set of references. If you use the Replace Entity command instead, the new entity inherits references from the old entity and you do not need to recreate them. During the replacement, you can also change inherited references and add new references.

, Offset, Silhouette Entities or Intersection Curve

When using sketch tools that refer model geometry, consider using the largest entities possible for the task, in this order:

• Body
• Face
• Edge

Selecting bodies or faces generates the most robust type of relations in that sketch. Even if you remove some of the edges of the referenced body or face or add some in the future, the sketch entities update without errors (Figure 23 and Figure 24).

Best Practices for Modeling in the Part Environment

Similar to sketches, there is no good way or bad way to model parts. With that said, here are some tips to help you work more quickly.

Structure the FeatureManager for Maximum Productivity

A well-documented FeatureManager design tree allows users to save time:

• Understanding the design intent
• Editing the model
• Configuring the model
• Finding features and sketches
• Selecting entities

SOLIDWORKS has extensive capabilities for configuring the FeatureManager at the part level:

1. Learn how to switch between the classic and flat tree views

When performing edits, it is easier to see the sketches in their historical location in the tree instead of being absorbed by their features. This is very useful when the model is interrogated or replied using tools like the Rollback Bar or the Part Reviewer.

You can use the right-click context-sensitive menu (example in Figure 25), or press CTRL + T as a shortcut that switches between the classic tree view and the flat tree view.

1. Name the features that you access repeatedly

Naming features makes finding them easier, especially when using the filter at the top of the tree. In addition, you can increase the modeling consistency at the team-level by establishing naming conventions for the most important features. Capture the standardization of the naming in written procedures and communicate the standards to every designer in the company.

1. Add frequently accessed entities to the Favorites older

Adding frequently accessed entities to the Favorites folder is a convenient way to locate them quickly for editing or reference.

When accessed from the Comments folder, you can edit features, configurations and more.

” in the SOLIDWORKS online Help.

1. Use Selection Sets

Selections sets are the perfect tools for quickly selecting multiple entities in bulk based on user criteria.

Imagine that you need to be able to hide and show a set of reference sketches or reference surface bodies quickly, as shown in Figure 30.

To help understand the difference between Features and Bodies, consider a real-life manufacturing process.

The features are analogous with a set of instructions. Consider a piece of paper containing this information:

• Start with a 2” thick plate.
• Cut an 8” by 12” piece.
• Punch center marks for 4 holes, 1” away from each corner.
• Drill and ream 4 x Ø ½” through holes.

These are similar to the Features in a SOLIDWORKS model.

As a machinist follows the process, each instruction creates or modifies one or more bodies.

To summarize:

• Features are instructions (information).
• Bodies are the geometric and topological result of applying the instructions in a chronological order.

This explains the differences in what happens when a deleting a feature versus a body.

Simple versus Complex Features

In SOLIDWORKS, you can use different techniques to create the same geometry.

When considering the impact on efficiency when creating features, there are several important considerations:

• Modularity
• Robustness
• Rebuild time

1. Modularity

Using simple features increases the length of the FeatureManager but has two major advantages:

• The model is easier to modify if the design intent changes significantly.
  • For example, when the rounds are modeled as sketch fillets, there is no simple way to turn them into chamfers. You would have to edit the sketch, delete or replace all arcs with lines, and add extra relations and dimensions.
  • If instead you model the rounds as fillet features, you can quickly:
    • Suppress them
    • Delete them
    • Convert them to chamfers

1. Robustness

Simple features are more resilient when performing edits. If a simple feature fails, it is much easier to troubleshoot than a complex feature.

For example, it is possible to achieve the final geometry of the model in Figure 32 with only one complex Mutual Trim feature.

Place features that generate complex topology or geometry at the end of the tree.

Figure 34 depicts the creation of a complex pattern before creating other simpler features.

Feature	Rebuild Time Figure 66	Rebuild Time Figure 35	Time Saving
Complex Pattern	14.42	14.19	1.6%
Simple Pattern	0.38	0.11	71.1%
Counterbore Holes	0.13	0.02	84.6%
Chamfer	0.20	0.00	100%
Overall	15.13	14.31	5.42%

Hole Wizard versus Cut-Extrude Features

When you have the choice between two features that produce the same geometry, choose the feature that is specialized for the job. For example, use the

Hole Wizard

feature for cutting round holes or slots. Advantages:

• Allows for quick change of hole type and parameters
• Follows a standard
• Incorporates a sketch pattern
• Can be used as input for Pattern Driven Component Pattern
• Has more parametric dimensions and annotations available for detailing drawings
• Easy to use because it requires only position input

Patterns

When you become familiar with the advanced options for patterns, you can use them not only for duplicating features or bodies, but also for generating geometry that otherwise requires a large number of features or complex sketches.

Here are only three examples that emphasize how you can use patterns to communicate the design intent efficiently.

1. Up to reference option

This is a great way to replace complex equations for distributing features on a given space and it is the perfect tool for resizing library parts by editing only one dimension.

For example, in Figure 36, if the length of the plate changes, the cutouts relocate, while maintaining an equidistant dimension between them.

When you want to copy one feature while observing all relations and dimensions inside the sketch that defines it, the Vary Sketch option can help you achieve that. Select one dimension to define the direction:

• Linear dimension for linear patterns
• Angular dimension for circular patterns

The pattern in Figure 37 has the same effect as creating 5 different Cut-Extrude features with the same sketch relations and dimensions. The only difference between these 5 features is the original 0.500” sketch dimension, which is indexed by 2” for each instance.

This option allows:

• Incrementing spacing between instances
• Incrementing sketch dimensions
• Editing spacing and dimensions for individual instances

When downloading files, especially fasteners, from your suppliers, perform these three tasks before saving the files in your library:

1. Suppress or delete unnecessary cosmetic features (usually threads)

If your use case does not require a specific detail, eliminate that detail. Such features require unnecessary computation resources to generate the body data and, especially, the graphics data. Once created, the graphics data requires storage and manipulation by the video card, which causes additional slowdowns. Imagine the difference in performance between an assembly containing 1000 of the screws shown in Figure 39 with or without the threads and knurls.

The user who creates a document specifies the image quality. High image quality results in a large file size and slower performance. After a certain point, increasing the image quality yields negligible difference. Adjust the image quality to your company standards by moving the resolution sliders in the Document Properties - Image Quality dialog box as shown in Figure 40.

1. Delete all equations

Some suppliers insert complex equations in their models, mostly for their own use. Because you most likely download one file per product, you do not require those equations. Deleting the equations eliminates the possibility of the application evaluating them during rebuild. This saves you valuable time.

Tools for Troubleshooting

In the process of revising existing models, errors or warnings could appear in the FeatureManager. Train users to use diagnostic tools to find and eliminate the causes for such errors. Insist on establishing the practice of checking in to the vault only models with no errors.

The “SOLIDWORKS Essentials” training covers the diagnostic and repair tools extensively. This article provides examples of how such tools work together.

1. Rebuild versus Forced Rebuild

The Rebuild (CTRL + B) command rebuilds only features that change. This is your main tool when rebuilding parts.

The Forced Rebuild (CTRL + Q) command rebuilds all features. Use this command only for troubleshooting. Otherwise, you may waste time by repeatedly rebuilding features that do not changes.

1. Always troubleshoot from the top of the tree down

Because SOLIDWORKS features have a chronologic hierarchy, fixing errors in parent components many times solves problems in the children. As shown in section 5ai, you can use the Flat Tree View to reveal the complete history of the model (sort tree entities in a chronological order).

1. Rollback Bar

When repairing models with errors, the rollback bar shifts to the feature with the first error.

Remember that you can access the Rollback command from the context toolbar.

Click a part name in the FeatureManager to reveal a list of errors and warnings. Clicking any entity in that list advances you directly to that feature in the tree.

The best way to filter errors and warnings inside sketches is the Display/Delete Relations tool.

You can activate the SketchXpert tool by clicking the Over Defined notification on the status bar.

PropertyManager, click Diagnose and cycle through all possible constraining schemes in the sketch.

When relations dangle, select the dangling entity (not the relation) and a red dot appears next to it. Drag the red dot on the reference entity to reattach the relation or dimension.

When working with parts that have long feature trees and long rebuild times, it could be beneficial to use the freeze bar temporarily. This forces SOLIDWORKS to stop rebuilding all features above the freeze bar.

It is a recommendation to use the freeze bar wisely. You might have heard that freezing all part components makes assemblies open faster because no rebuilding happens at the part level.

Part components do not rebuild when an assembly is open, unless body data is missing or obsolete. When that happens, you want the part to rebuild.

While it is possible to lock or unlock external references in bulk from the main assembly, you must unfreeze frozen features file by file.

Maximize Efficiency when Fixing Imported Geometry Errors

For fixing errors with imported geometry, start by reading the SolidPractices document "Working with Imported 3D Data", which is available for subscription clients on my.solidworks.com.

From the efficiency point of view, the following considerations are critical:

1. Attempt to solve all topological errors

When topological errors exist in the model, the performance of SOLIDWORKS suffers, especially in drawings. Often, drawing views that refer to components with such errors are not solvable as high quality. This impacts the:

• File size
• Saving time
• Loading time
• Update time
• Printout quality
• PDF, DWG or DXF saving time
• PDF, DWG or DXF quality

1. Do not add new features until performing a diagnostics test to identify import errors

Whenever SOLIDWORKS imports a fil, it imports in the form of surfaces and solids, which consist of faces, edges and vertices. To repair any topological errors in an imported file, it is important to run the Import Diagnostics tool. The Import Diagnostics tool is available only before adding new features. Identify and resolve geometric errors before adding new features or use the part in an assembly.

1. Check tool

To save time when troubleshooting parts that have multiple imported geometry features, it is important to single out the features that have topological errors. The fastest way to achieve this is to use the Check tool. This tool works for both parts and assemblies.

After selecting a feature with errors in the Check tool, close the tool, right-click in the empty graphics area and select Invert Selection.

Right-click again in the empty graphics area and select Suppress. This suppresses all imported features, other than the feature that has the error.

You can now run the Import Diagnostics tool. The result becomes available within seconds, depending on how much you simplified the model.

At this point, either follow the steps from the SolidPractices "Working with Imported 3D Data", or the techniques learned from the Surface Modeling course or the Mold Design Using SOLIDWORKS course to eliminate the errors.

After repairing one feature, unsuppress the rest and repeat the steps above until the entire model is free from topological errors.

Part Level Configurations

Using the configuration functionality of SOLIDWORKS is a business decision, not a design decision.

Some companies consider that form, fit and function are the critical factors for assigning part numbers. For example, each size variation requires a separate part or assembly file. In this case, it is best to limit the usage of configurations only to generate detailed and simplified representations for use in part drawings or as components of complex assemblies.

If your company standards allow the use of configurations for creating components with different form, fit or function, it is important to train users to master the tools dedicated to creating and editing configurations:

• “Configuration and Display States” lessons on my.solidworks.com
• SOLIDWORKS Essentials training course

From the efficiency point of view, the following considerations are relevant:

1. Do not delete configuration data if it will be used in assemblies or drawings

When body data is missing, SOLIDWORKS must rebuild the part, which in turn triggers an update at the assembly or drawing level.

While the part file size increases as more data saves in the file, the savings in time that results from not having to compute body data is more important.

To maintain the body data, make sure that the Purge cached configuration data option (System Options >

Performance

) is not active.

For individual parts, ensure that all configurations used in large assemblies or drawings display a checkmark next to their name. To add the checkmark, cycle through the configurations that the assembly or drawing require.

If you require to save the body data for all configurations in the model, press CTRL + SHIFT + Q to rebuild them all.

1. Avoid multiple dimension drivers

SOLIDWORKS allows multiple tools to drive dimension values, For example:

• SOLIDWORKS equations
• Equations in Microsoft® Excel® design tables
• Equations in custom properties
• External references

If multiple drivers exist in the same part, it is possible to experience repeat rebuild cycles when performing edits. In the worst cases, the part never rebuilds completely, which drastically affects the performance of any large assembly or drawing where referred.

1. Use configuration tables

SOLIDWORKS configuration tables (version 2022 and later) are light and fast. At the part level, you can use them to:

• Create new configurations
• Configure dimensions
• Configure features
• Configure properties

• Assembly Modeling Methods

• There are multiple factors that determine how an assembly is modeled. This section mentions only a few:

  • Your company’s position in the supply chain.
    • Supplier
    • Client
    • Both
  • Type of product
  • Type of production:
    • Job production (one-off or custom)
    • Batch production
    • Mass production
  • Development maturity:
    • Ideation
    • Conceptual design
    • Product development
    • Maintenance and continuous improvement

  • Number of variables for configuring the product

    The combination of these factors determines if your team will use one of these modeling methods:

  • Bottom-up
  • Top-down*
    • Permanent
    • Temporary

  Note: * Top-down assemblies can contain components built using the bottom-up method.

  The main difference between these methods if any external references exist is how the SOLIDWORKS application manages the references at the assembly level.

  	Bottom-up	Permanent Top-Down	Temporary Top-Down
  External References	None	Yes. Permanent	Yes, during development and editing. Locked when Released for Production
  Production Type	Mass	One-off	Batch or Custom
  Development	Mature product	Conceptual phase	Continuous Improvement
  Pros	Robust (minimize the occurrence of errors)	Fast Revisions	Offers a good balance between speed and security
  Cons	Slow Revisions	Slow rebuild time if the flow of external references is not unidirectional. Possible loss of references with edits.	Require strict adherence to the company modeling procedures

  The success in applying any of these methods depends on:

  • The existence of good modeling procedures in the company
  • The degree of adherence to these procedures by all users on the team

  Simplified Flow Chart – Assembly Open Process

  Understanding how information flows when an assembly opens or updates is the key to understanding the effect of a users’ modeling decisions on their productivity.

  To do that, this section connects the dots between the assembly tree structure (Figure 55) and the Open and Update assembly workflows (Figure 57 to Figure 59).

  

  Assembly open process

  To understand the recommendations from this section, it is important to consider how SOLIDWORKS processes information when opening assemblies (Figure 56).

  You can divide the process for opening an assembly in Resolved mode into five phases (Figure 56):

  1. Load components with a preview in the graphics window
  2. Update information related to out-of-date components
  3. Solve mates
  4. Compute in-context and assembly features
  5. Compute graphics data

  

  Depending on the difference between the information saved in the assembly and the information saved in the assembly components, you can bypass or repeat some of these phases. Consider the following possibilities.

  1. Clean assembly

  If none of the assembly components have changes since last opening the assembly, the open process jumps from Phase 1 to Phase 5.

  
  1. Typical assembly

  Typically, one or more components have changed since the assembly was last open. In this case, all phases are performed only once.

  

  In this case, SOLIDWORKS evaluates all tree entities from Figure 55 only once.

  Even if you have not revised any components, something inside them might still cause the program to report them as out of date. Examples:

  • Configurations that are out of date
  • Components whose rollback state differs from the one last saved in the assembly
  • Components with cosmetic threads in pre-SOLIDWORKS 2019 format
  • Components with sheet metal features in pre-SOLIDWORKS 2013 format
  • Components with multiple drivers for dimensions, such as equations
  • Components that can take advantage of software improvements
  1. Assemblies with mates attached to entities that change during the rebuild phase

  The last case is when there are mates for entities that depend on tree items below the Mates folder in Figure 55.

  Because the rebuild progresses from the top of the assembly tree to the bottom, the software evaluates mates once. Then, the in-context and assembly features modify the location or orientation of some of the mated entities, which invalidates the first solution of the assembly mates. A second computation of the mates becomes necessary (Figure 59).

  Beyond the second computation, you can avoid an infinite loop by adding a rebuild light to indicate that a feature or component requires update. Then, the open process continues to the last phase.

  

  When opening assemblies in Resolved mode, the subassemblies also follow the same process. Imagine how many extra loops such a process might require if the subassemblies have components that are identified as changed.

  To minimize opening times, ensure that you:

  • Include body data and configuration data in the component files.
  • Follow best practices in creating mates.
  • Avoid creating external references that affect mated entities at the top level of the assembly.
  • Make external references unidirectional.

  These practices are explained later in this section.

  Assembly Open Modes

  To help understand the main open modes for an assembly, consider the simplified structure of a resolved assembly (Figure 60).

  

  Mode	Feature Data	Body Data	Mate Data	Graphics Data
  Large Design Review	Not loaded	Not loaded	Not loaded	Yes
  Large Design Review (Editing)	Not loaded	Not loaded	Top Components Only	Yes
  Lightweight	Planes and Axes	All	Top Components Only	Recomputed
  Resolved	All	All	All	Recomputed

  1. Large Design Review mode

  For users of large assemblies, it is imperative to master the use of Large Design Review (LDR) mode, with which they can quickly accomplish many of their most frequent tasks.

  Tasks include:

  • Update component graphics data
  • Highlight or isolate modified components
  • Visual examination of the assembly
  • Reviewing different configurations of the assembly (with Display Data mark).
  • Using the assembly as a graphical directory for finding specific components
  • Reading the description and configuration of components
  • Hiding, showing or isolating components
  • Performing graphics-only section views
  • Getting various types of measurements such as distances, lengths, diameters and areas.
  • Performing Static and Dynamic Interference checks
  • Checking hole alignment
  • Performing walk-throughs
  • Creating snapshots
  • Access performance evaluation (Limited)
  • Using the Selective Open dialog box to:
    • Perform quick revisions
    • Perform quick validation studies on a limited set of components:
      • Interference detection
      • Clearance verification
      • Collision detection
      • Hole alignment

  For more information about LDR, see the topic "Large Design Review" in the SOLIDWORKS online Help.

  1. Large Design Review – Editing mode (LDR-E)

  If you require quick editing of an assembly, you can edit it in LDR mode. An interesting use case is when collaborating with a third-party contractor without sending them a complete Pack and Go or Copy Tree file set:

  • The contractor receives only the assembly file.
  • The contractor opens the assembly in LDR-E mode.
  • Adds and mates new components.
  • Deletes or edits other components and mates.
  • Creates linear or circular patterns of components.
  • Saves the assembly and returns the assembly in email, along with any new components.
  • The original user receives and uses the updated assembly.

  For more information about the capabilities and limitations of the LDR-E mode, see the topic "Editing Assemblies in Large Design Review" in the SOLIDWORKS online Help.

  

  The Lightweight mode offers the best balance between speed and capabilities when working with large assemblies. Because this mode loads only a subset of data, the opening, update and rebuild times are minimized.

  It is worth knowing that in situations when the body data is missing from components, the Lightweight mode could require a secondary component read and rebuild. In extreme conditions, this extra computation could make loading the assembly in Lightweight mode more time-consuming than when opening it in Resolved mode.

  1. Resolved mode

  Modern workstations can handle most assemblies that open in Resolved mode. Because this mode loads all data from all components, it is also the perfect mode for:

  • Updating assemblies created using top-down modeling techniques
  • Troubleshooting performance issues
  1. Automatically optimize resolved mode

  Starting with SOLIDWORKS 2023, SOLIDWORKS can assign the optimal opening mode for each component. The application loads most components in Lightweight mode and resolves as needed programmatically. From the perspective of the user, all components appear as resolved. To have SOLIDWORKS assign the optimal opening mode, activate the option Automatically optimize resolved mode, hide lightweight mode from System Options > Performance.

  FeatureManager Design Tree Customization in Assemblies

  Most best practice suggestions described in section 5a for customizing the FeatureManager design tree in parts apply in the assembly environment as well, with these additions:

  1. Enhanced tree filter

  The filter in the assembly FeatureManager offers extra options (Figure 62):

  • Isolate selected components in the graphics area
  • Include hidden and suppressed components in the filtering
  • Filter based on the values of custom properties values (Figure 63)
  

  From the efficiency point of view, the fastest response when filtering is when the Filter Graphics View and Look in Custom Properties options are not active.

  1. Tree display (assemblies)

  The tree display options for assemblies have several differences as compared to the options available for parts (Figure 64).

  

  Decluttering the FeatureManager design tree is critical for maximizing efficiency when working with assemblies. To do that, master the following options:

  1. Do not show Configuration or Display state if only one exists

  

  * The names and description elements with an asterisk (*) in Figure 65 are specific to 3DEXPERIENCE SOLIDWORKS.

  1. “View Mates and Dependencies” versus “View Features”

  Tree Display	Component Features	Mates	Best Use in Modeling
  View Features	Listed	In Folder	Top-Down
  View Mates and Dependencies	In Folder	Listed	Bottom-Up

  - See what you need depending on your modeling technique

  1. Group Components Instances

  To shorten the length of the FeatureManager design tree, you can use the Tree Display > Group Component Instances option to collect instances of the same components from the top-level assembly in groups (Figure 67).

  

  1.  

     

  - Great for selecting instances of the same components in bulk

  1. Group Mates by Status

  To declutter the Mates folder, right-click the folder and then select Group Mates > By Status.

  
  • Solved
  • Errors
  • Over Defined
  • Suppressed
  • Suppressed (Missing)
  

  Efficient Assembly Structure

  When considering the assembly structure, the keyword is modularity. A modular assembly (containing a small number of top-level components) has major advantages. When compared with a linear structure (containing many top-level components), a modular assembly:

  • Opens faster. If there were no edits to subassemblies since the last time the top-level assembly was saved, the program does not recompute any mates or assembly features at the subassembly level. Fewer unnecessary computations = faster opening time
  • Computes the mating scheme faster. The program evaluates only the top-level mates during loading or when using the assembly as a flexible subassembly in a higher-level assembly.
  • Offers improved control for assembly features and in-context references.
  • Is easier to configure.
  • Is easier for other users to understand the design intent.
  • Is easier to troubleshoot and fix errors.

  

  Efficient Mating Schemes

  The locations and orientations of all components are written in the assembly file. When an assembly opens, if all components are unchanged, they are placed in their known positions and no mate computation is required (Figure 57).

  When components are identified as changed (Figure 59), if mates are present, they are computed.

  1. How mates compute internally

  Computing mates is a multistep process. Consider a simple assembly built using the bottom-up method that contains no flexible assemblies. The steps in the process are:

  1. Parse the Mates folder to identify which mates are redundant for defining the location and orientation of all components.
  2. Create a mate group for solving the mating scheme without including the redundant mates.
  3. Solve the mate group and verify its validity.
  4. If errors occur, repeat the process by selecting a different set of non-redundant mates.

  To help understand this section, perform a simple experiment. Start a new assembly and insert 3 instances of a cube. For one full minute, keep applying coincident, parallel, perpendicular or width mates between the three components. How many of such mates did you manage to apply?

  For example, the assembly in Figure 72 contains 18 mates. However, only 6 are needed to fully define the cubes. What about the other 12?

  

  SOLIDWORKS is known for its user-friendly experience and mating is no exception. As long as mates are not contradicting each other, you do not receive any warnings about mate redundancy.

  Allowing this freedom to users comes with a price, especially if mates are contradicting each other, over defining the assembly.

  As per the Dassault Systèmes Knowledge Base article QA00000117302, performance could fall dramatically if over definition occurs. In this situation, there is no valid solution to the mate parsing process. Therefore, the program selects the least "bad" solution. To derive this least bad solution, the program considers all possible mating schemes. In large mating schemes with errors, the parsing process could take a considerable amount of time.

  The main takeaway: Fix the mates errors as soon as possible!

  1. Best practices for applying mates
  • Do not apply any mates (using the Base Part, AKA Skeleton Part method).

  An assembly without mates has shorter opening and rebuild times. An upcoming SolidPractices document about the Base Part methodology discusses this technique.

  • Prefer simple standard mates

  When possible, apply simple mates like:

  • Parallel
  • Coincident
  • Perpendicular
  • Distance
  • Concentric
  • Do not create circular mating schemes

  

  • Reduce the length of the chain of dependencies between mated components

  The assembly in Figure 74 has a daisy chain mating scheme.

  The purple component is fixed. To know the location of the blue component, SOLIDWORKS needs to know the location of all the other components.

  

  The assembly in Figure 75 has an efficient one-step mate dependency scheme.

  The purple component is fixed. All the other components mate directly to it.

  

  Using the Multiple mate mode option is one of the most efficient ways to apply numerous mates to a common reference, while observing the one-step dependency principle.

  Corollary: First, mate major components directly to each other and then mate fasteners to the major components. In Figure 76, the plunger in the left assembly has a 6-step dependency in its mate chain, while the assembly on the right has only 3.

  The other major advantage is the fact that when fasteners are suppressed in the right assembly, the major components remain properly mated.

  • Mate to the most robust entities in the model. For a bottom-up assembly, consider this order:
    • Top-level assembly origin or major planes (front, top, right)
    • Component origins or major planes
    • Coordinate systems and axes
    • Faces
    • Edges
    • Vertices
    • Sketches (depending on the complexity of the project)

  As mentioned earlier, to maximize efficiency it is important to declutter the graphics area by hiding all planes, axes and sketches by default. Fortunately, there are two excellent tools to reveal reference geometry temporarily:

  • Press Q to show primary and reference planes, coordinates and origins (default keyboard shortcut).

  To apply mates, follow these steps:

  1. Hover over a component and press Q. The planes, coordinate systems and origin of that component become visible.

  Note: When hovering over empty space, the planes, coordinate systems and origin of the top-level assembly become visible.

  1. Select an entity, such as a plane.
  2. Hover over another component and press Q. The planes, coordinate systems and origin of that component become visible.
  3. While pressing CTRL, select an entity from the second component.
  4. Apply a mate between the two entities (ideally using the Quick Mates toolbar).
  5. After applying the mate, click anywhere to hide the entities used in the mate.
  • Add a keyboard shortcut or a context toolbar icon to show or hide primary planes.
  
  • Select a Reference entity to create robust Angle or Angle Limit mates

  To prevent angle mates flipping alignment on rebuilds, specify a quadrant as a reference for defining the mate by using the Reference entity field (Figure 78).

  

  As described in section 3, to maximize your efficiency it is important to focus on the model as you work. You can achieve this by working as much as possible with context toolbars, keyboard shortcuts and mouse gestures. That frees you from the need to move your attention from the model to other areas of the screen such as the PropertyManager, CommandManager or the FeatureManager.

  Following are some of the best tools to declutter the graphics area, select entities to mate and to apply and edit mates.

  1. Quick Mates toolbar

  Enable the Quick Mates toolbar by activating the Show quick mates option in the Customize dialog box (Figure 79).

  toolbar appears, proposing a list of mates that is relevant to your selection. In addition, depending on the number and the type of entities that you preselect, pressing the mate icon (paperclip) can activate MultiMate mode.

  If preselecting more than two faces, the following rules apply:

  Total Pre-selected Entities	Number of Planar Entities	Number of Circular, Cylindrical or Conical Entities	Default Mate(s) (mate icon must be pressed)
  3	3	0	Symmetric Mate
  3	2	1	Width Mate
  4	4	0	Width Mate
  Minimum 3	0	3 or More	Multi Mate mode
  Minimum 5	5 or More	0	Multi Mate mode

  

  1. Quickly select obscured faces
  2. Select Other tool: Right-click to hide faces, Left-click to select.
  3. Temporarily hide faces when the Mate command is active by selecting them while holding the ALT key.
  4. X-Ray using the magnifying glass tool. For best results:
     1. Press G to start the magnifying glass.
     2. Spin the mouse wheel to specify a 1 to 1 zoom factor.
     3. Press and hold the ALT key and spin the wheel to define the depth of a section view parallel to the screen.
     4. Press and hold the CTRL key to select multiple entities.
     5. To exit the tool, perform one of these actions:
        • Select an entity without pressing CTRL.
        • Press G.
        • Press the Esc key.

  

  1. Component preview window

  The Component Preview window is perfect for displaying any component in its own window, whose viewport you can manipulate independently from the main viewport (Figure 83 and Figure 84).

  
  • Visible
  • Wireframe
  • Transparent
  • Hidden
  

  The Isolate tool is the ultimate tool for decluttering the graphics area, especially when applying mates. Anything that was not preselected is hidden temporarily or displays as:

  • Wireframe
  • Transparent (Figure 86)
  

  When mate errors occur in assemblies, efficient users know how to use special tools to quickly troubleshoot the mating scheme, identify the cause and fix the problem.

  1. Auto Repair

  When the ID of mated entities change (usually as the result of editing a mated part component), warnings like the one in Figure 88 become attached to the affected mates.

  

  To begin the repair, right-click one mate and select Auto Repair.

  folder and selecting Auto Repair.

  To save time when troubleshooting errors in a large mating scheme, it is important to select mates that have errors or warnings quickly. A fast way to do that is to:

  1. Click the assembly name. A list of warning and errors appears.
  2. Click any item in this list (Figure 91). Each item is a hyperlink to the actual mate.
  

  Following is a great technique for decluttering the graphics:

  1. Preselect one or more mates.
  2. Start the Isolate tool.

  The components involved in the selected mates are now isolated in the graphics area, making it easier to troubleshoot.

  

  When you want to focus only on the components that have mate errors, it is important to have an ability instantly isolate only those components.

  Click Over Defined in the status bar (Figure 94) to reveal the View Mate Errors window while hiding components that have no mate errors.

  Select one or multiple mates in the list to display their callouts with shortcuts. In Figure 94, the orange box shows shortcuts, left to right, for the following:

  • Flipping the mate alignment
  • Forcing the mate solving
  • Editing the mate
  • Suppressing the mate

  Right-click the callout to display additional functionality:

  • Deleting the mate
  • Configuring the mate
  

  One of the best ways to improve efficiency when troubleshooting mates is to group them by status (Figure 95).

  
  • Solved (no errors)
  • Have errors
  • Are over defined
  • Are suppressed
  • Belong to suppressed or missing components (Figure 96)
  

  When multiple conflicts exist between mates, it is important to be able to resolve the problem by analyzing the mating scheme and grouping the errors and warnings in subsets of mates that are in direct conflict.

  The MateXpert tool does exactly that. You can access this tool by right-clicking the Mates folder.

  When the tool starts, click Diagnose (Figure 97).

  

  To minimize the time of instantly selecting multiple components based on user-defined criteria, learn how to use the multiple bulk-selection tools available in the assembly environment.

  One way to access most of these options is by using theSelectflyout button from the standard toolbar or from the shortcut toolbar (press “s”).

  The recommendation is to assign keyboard shortcuts for some of the most useful options. A good example is the Select Identical Components command, which allows the selection of all instances of a component, regardless of where they are nest inside the various subassemblies.

  
  1. Start the Advanced Selection tool.
  2. Define the criterion of selection. For example, select all Purchased components.
  3. Name your search and save it.
  menu by choosing the Add to Favorites option.
• to share the custom selection with your team in an external file, which other users can import when needed.

• Figure 105 shows the end-result.

  

  TheManaging Large Assemblies in SOLIDWORKSSolidPractices document covers most of the diagnostic tools for troubleshooting assembly performance Shortcuts to relevant Help topics follow:

  • Assembly Open Process Indicator
  • Performance Evaluation
  • Assembly Visualization
  • File Explorer Feedback

  Conclusion

  This document focused on best practices for efficient modeling specific to the core functionality of SOLIDWORKS. Depending on the areas of SOLIDWORKS that you use, you can complement this information with other SolidPractices documents. Examples include:

  • 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 DS SOLIDWORKS Corp.