The Art of SolidWorks Part Modeling

The Art of SolidWorks Part Modeling

SOLIDWORKS part modeling is a powerful tool that can be used to design a wide range of parts, assemblies, and drawings. Several techniques are available for creating a SOLIDWORKS part model. The choice of technique will depend on the shape of the part and the desired features.

Creating a good 2D sketch is essential for producing a quality 3D model. It is also important to use the right technique for the job, as there is no one-size-fits-all approach to part modeling. Using features and components wisely can help create complex parts more easily. The SOLIDWORKS help system is a valuable resource for learning about the different part modeling techniques. By following these tips, you can create accurate, efficient, and easy-to-use SOLIDWORKS part models.

PARTS

Efficient assemblies depend on the quality of their parts. To achieve this, parts must be modeled intelligently and effectively as they are essential components of bigger assemblies. In designing parts, it is crucial to begin with a plan that prioritizes efficient modeling and properly placed reference geometry. To achieve this, it is important to establish design intent, which will aid in planning part construction by considering the key elements below:

- Origin: Where should the origin be placed? How will it affect the mating of the parts in the assembly?

- Symmetry: Is there symmetry? If so, how many planes of symmetry? Generally, the origin is on all the planes of symmetry or even less of the part and then either mirrored or patterned.

- Features: Decide which elements should get their features in the FeatureManager design tree. Will any features need in-context relationships?

- Configurations: Configurations can be used to create both the maximum (full detail) and minimum (only the detail needed to mate the part into the assembly) conditions of the part.

- Patterns: Patterns can reduce the amount of work needed to create the part and can also be used at the assembly level to add fasteners automatically.

- Views: Which view of the model will be the Front View when detailing? Will detailing require special views?

- Mating requirements: How will this part be mated in the assembly?

- Properties: What properties need to be attached to the part for accurate assembly weights, BOMs, part callouts, and the like?

- Templates: The right template can save time by having repetitive information and proper settings already entered. Consider creating specific templates for different customers.

- Document settings: Document settings will control the speed and ease of the design process. What image quality and display settings will allow us to see the design easily without slowing down?

FEATURES

To reduce the number of features, it's recommended to plan ahead before modeling. Combining features in a sensible manner is important as you may need to make changes to the model in the future.

When it comes to fillets and chamfers, it's best to place them at the end of the FeatureManager design tree and combine them into the minimum number of features possible. This has two benefits: the model rebuilds faster when adding features before fillets and chamfers, and these features can easily be grouped into folders for quick suppression and unsuppression. Use the Feature Statistics tool to identify which features are slowing down rebuild time and consider suppressing them while working on other parts of the model. Feature Freeze is another tool that can be used to keep some or all features from rebuilding, which can significantly reduce rebuild time for complex parts. By setting the Feature Freeze bar at the bottom of the FeatureManager design tree, all features can be kept from rebuilding, making configuration changes much faster.

FEATURE STATISTICS / PERFORMANCE EVALUATION

The Performance Evaluation/Feature Statistics tool is a useful resource for identifying features that take a while to rebuild. By using this tool, you can determine which features should be suppressed in a simplified configuration.

When inserting a part into an assembly only once, manually creating mates can work well. However, if the part is used multiple times, it can be more efficient to establish mate references on the reusable parts, saving a significant amount of time.

PATTERNS

Using patterns can either speed up or slow down the model rebuild time depending on how they are utilized. Feature patterns offer the benefit of being a source for other patterns at the assembly level, as in feature-driven patterns. They can also be a source for adding fasteners to an assembly through Smart Fasteners, which helps to reduce rebuild times as the pattern controls the fastener positions instead of mates.

It is best to avoid patterning on top of other patterns. Instead, create a single pattern that includes all the features. Additionally, move larger patterns to the bottom of the FeatureManager design tree. This allows other features to be built first and also enables the pattern to be suppressed without worrying about parent/child relationships.

REMODELING PARTS

At times, certain parts can experience inefficiencies as a result of added or removed features in search of the perfect final form. In order to eliminate these inefficiencies, the part in question should be recreated completely from scratch. However, making the decision to do so can be a challenge, especially when operating under tight deadlines. It is crucial to weigh the cost of remodeling the part against the potential problems that may arise due to the inefficient model. While remodeling does require a finite amount of time, it usually does not take as long as anticipated since the final model is already known. An inefficient model can fail to rebuild with even a minor change and can drastically affect rebuild times when there are multiple inefficient parts. It is important to consider if the part in question is a one-time-use component or if it will be utilized in future designs prior to opting out of recreating an efficient and reusable part.

SYMMETRY

In the world of engineering, creating a part with symmetry can prove to be an extremely useful technique that can simplify the entire assembly process. By doing so, the number and complexity of mates required are automatically reduced, making the process more manageable and efficient. What's more, symmetry proves to be particularly beneficial when parts need to be perfectly centered on each other.

Apart from this, using symmetry can also speed up the rebuild time for individual parts when mirroring bodies. Instead of having to rebuild the geometry for each feature, surfaces are patterned, making the process much faster. Overall, using symmetry is an excellent way to streamline the entire assembly process while ensuring precision and accuracy.

TEMPLATES

Using proper templates can save time in all phases of modeling. The advantages of using good templates are:

- The document properties are already set, so you can start modeling without adjusting the settings.

- Visual and physical properties such as the model and background appearance can be set beforehand, eliminating the need to change them later. The appropriate and consistent materials can be added to the part before creating the first geometry.

- Custom properties such as the company name, address, and the creator of the file can be prefilled. Other important information such as the material and weight can also be established to capture model properties.

PART ORIGINS

The location of a part's origin is typically determined by its geometry and symmetry. However, there are two exceptions to this rule. The first is when the origin is positioned in a way that allows the part to align with a layout grid without the need for mates. The second exception is when a part is created in-context and its origin is projected onto the Front plane of the new part from the assembly origin.

Positioning the origin based on the part's geometry is the most commonly used method and is recommended in best practices documents. However, aligning the part's geometry to the origin for alignment purposes is not typically done in smaller assemblies or with parts that may be used in different assemblies. This approach can be useful in larger assemblies as inserting the part at the assembly origin and fixing it reduces the number of top-level mates required. If the features of a part are correctly located on the origin, mating planes are already present. For instance, if the absolute center of a sketch for a Wide Flange Beam is placed on the origin, extruding from the midplane produces a Top plane, a Right plane, and a Front plane in the middle of the beam without any additional work.

When a part is created in the assembly, its origin may be located far away from its geometry, which is generally unacceptable. This can be fixed, or in-context relationships can be created differently to avoid the origin being off the part.

PART CONFIGURATIONS

When working with large assemblies, it's important to consider the impact of the parts' configuration on their speed and performance. While configurations can lead to increased productivity and a reduction in the number of files to manage, they can also result in larger file sizes for parts and assemblies. Ultimately, it's up to the user to decide whether the benefits of using configurations are worth the potential file size issues for their specific application.

Configurations provide a simple way to manage numerous variables within a part or assembly, and design tables take it even further. However, when a configuration is activated, the data for that configuration is created and saved in the file to prevent performance issues. As more configurations are activated, file size increases, which can slow down performance when opening or transferring files over a network. When a part is used in an assembly, only the information for the configurations used in that assembly is loaded into memory. Furthermore, saving a file using "File, Save As" will only keep the data for the active configuration, significantly reducing the file size.

To maximize assembly performance, it's recommended to use simplified configurations that can be selected when opening the assembly. By doing so, unnecessary configurations are avoided, leading to faster loading times and a smoother overall experience.

SIMPLIFIED CONFIGURATIONS

In order to optimize the performance of your assembly, it is recommended to create a simplified configuration that only includes essential information about the part. By doing so, you can significantly reduce the amount of data loaded into your computer's RAM when opening the assembly. When creating this simplified configuration, it is important to include key information such as mating surfaces and interference surfaces. Mating surfaces are crucial for proper assembly, while interference surfaces ensure that the part does not interfere with surrounding components. On the other hand, cosmetic features like fillets, chamfers, and engraving should not be included in the simplified configuration as they are not essential for the assembly. Moreover, detail features, which refer to the small details of the part design, should be avoided as they can cause graphics performance issues due to the formation of many small triangles, similar to creating a mesh in FEA. By following these guidelines, you can create a simplified configuration that will enhance the performance of your assembly.

Naming Simplified Configurations

A great way to use simplified configurations is to create an assembly configuration that opens all components in their simplified form. This can easily be done by selecting the desired configuration name for each component when opening an assembly using the Advanced option. It's important to note that only one configuration name can be selected, so it's best to have a company standard for each engineer to create a simplified configuration with the same name. Additionally, capitalization matters, so "Simple" and "simple" are considered as two different configuration names.

To simplify the process of selecting small features, the Simplify tool is available. This command allows users to select features based on their size relative to the part. Users can select individual features from the Results list and click on "Suppress", or select "All" and then "Suppress" to suppress all the features found in the Results list. A derived configuration will be created with those features suppressed.

The Simplify tool can be found in the Menu under "Tools", then "Find/Modify", then "Simplify". It can also be accessed by clicking on "Simplify" in the Tools toolbar.

FASTENERS AND TOOLBOX

There are two ways to set up the toolbox:

1. Master parts - In this setup, the toolbox retains a set of master parts. When you insert a fastener into an assembly, the toolbox creates a configuration of the master part based on the size you are using. The benefit of this is that the part files increase in size as additional configurations are created. However, in a company environment, the toolbox part files are usually kept on a network drive, which can slow down performance as the files have to be opened across the network.

2. Copied parts - In this setup, new part files are created when you insert a fastener into an assembly. The advantage of this method for large assemblies is that these files can be stored with the assembly and have only a single configuration. This creates more files, but they can be stored locally and smaller because they only need a single configuration.

Toolbox parts can display three types of threads. Since fasteners are purchased parts, there is no need to show the threads unless they are needed for display purposes. For better performance, use a simplified thread display. If the threads are needed for rendering, choose cosmetic to have a thread appearance applied to the surface.

LEVEL OF DETAIL FOR PURCHASED COMPONENTS

When incorporating purchased components into your designs, you will require models of these components that fit seamlessly into your assembly. Depending on the source of the component model, it may offer a varying degree of detail. However, you only require the simplified configuration and not more detail than that to execute your design effectively. To hasten the assembly level design, the model may be stripped of excessive detail.

LEVEL OF DETAIL

Excessive detail results in extended rebuild times. Here are some suggestions on how to eliminate detail.

- Do not model threads. Instead, model only functional threads. Modeling helical threads comes with considerable regeneration times. If you need a visual representation of the threads, you can use the option on Toolbox to show threads as a texture map.

- Adding helical threads can cause more than five times the number of triangles required to represent the surface of the bolt.

- Use the Cosmetic option in Toolbox if you need to see visual threads.

- Avoid using text for features. Do not model text unless it is part of casting or will be machined into the part. Modeling text using TrueType fonts in Windows can result in hundreds of entities, sometimes per letter. You can evaluate the impact of modeled text by opening a part with extruded text and using the Performance Evaluation tool, previously known as Feature Statistics, to list and rebuild times.

- Minimize unnecessary detail.

- Combine fillets of equal size or function.

- Avoid Lofts and Sweeps if you can create the geometry with an extrude or revolve feature. Lofts and sweeps take longer to generate.

- Do not model springs unless absolutely necessary. Sweeping along a helix creates a large file due to the complexity of the surface, just like helical threads. Instead, use a cylinder that forms the bounding shape of the spring. This can be mated and used to detect interference while solving very quickly.

- If you need more visual representation, consider adding a decal or a thread appearance.

- Fully define sketches. Leaving sketches under defined may be acceptable when you are still in the early part of the design process for a part. However, before using that part in an assembly, you should have it fully defined to avoid rebuilding errors and unintentional changes.

In summary, when using purchased components in your designs, it is vital to consider the level of detail required. Too much detail can result in extended rebuild times. Therefore, it is necessary to eliminate unnecessary detail and use alternative options such as a cylinder or a decal to represent the required features. Finally, it is crucial to fully define sketches to avoid unintentional changes and rebuilding errors.

ADDITIONAL CONSIDERATION FOR PARTS

When constructing parts, there are other important factors to consider besides the techniques mentioned above. One such factor is the level of detail required for the manufactured parts. Typically, there is a mandatory level of detail and several optional levels, which are determined by the modeling and configuration.

The default configuration, also known as the full configuration, should contain all the necessary information to manufacture the part. Additionally, rendering may require all the details of the part, which is important for marketing purposes.

To simplify configurations, it is recommended that the company establish a mandatory name for this configuration. This ensures that when an assembly is opened, all components with a simplified configuration can be opened in that configuration.

In some cases, certain features, such as fillets that create tangent edges, should be suppressed before creating a drawing. This is known as the drawing configuration.

For huge savings in computational and memory requirements, a SpeedPak configuration should be considered for all assemblies.

Finally, if the part needs to be analyzed, the person doing the analysis will create the analysis configuration. Deciding which features to suppress involves more than simply suppressing small fillets.

COMMON TOOLS

When creating parts within an assembly, sketching is similar to the process used in part mode. However, with the added advantage of being able to reference and view the geometry of surrounding parts. To achieve this, you can use Convert Entities and Offset Entities, and dimensions can be added to the geometry.

Alternatively, if you don't want to create external references for your new feature or part, you can adjust the setting in Tools, Options, External References. This will result in the converted geometry being duplicated without any constraints, and no dimensions or relations can be added to other components or assembly geometry.

Furthermore, Hole Series is a unique type of Hole Wizard hole that is created at the assembly level. It automatically creates in-context holes in the referenced components. While Hole Series is beneficial in the design process, it's important to remember that it creates an in-context feature that must be solved at the assembly level.

IN-CONTEXT MODELING

Assemblies can contain virtual or in-context parts that can be created and built within the assembly itself. These parts can also be inserted into the assembly as new parts and built using converted edges, offset edges, and standard techniques. In-context modeling is a great time-saver in the design phase of most projects as it allows for changes to be carried through in-context features in a predictable way. However, it is generally best practice to remove in-context references before parts are released to manufacturing to avoid unintended changes from occurring. In some cases, in-context relationships may be left intact and locked if the customer is known to require changes after manufacturing has begun.

While in-context features have many advantages, they can cause slower performance when solving the model and can create confusion for people working on the model later in the process. Additionally, in-context parts in an assembly can cause the part origin to be in an undesirable location. It is important to consider where the part will be used before deciding to model it in the context of an assembly. In-context features and parts are best used for "one-of-a-kind" parts that will be used only in the assembly where they are modeled. Parts that will be used in more than one assembly should not be modeled in context as the external references created by the in-context features are stored in and controlled by the assembly in which the references were established.

If a virtual or in-context part is to be reused in other assemblies, it is possible to make a copy of the part and remove all of the external references with some work. The part can also be created by borrowing geometry without creating external references.

In-context features affect performance by creating additional work when the assembly is solved. The relationship between the current feature and the entity it is referencing is maintained at the assembly level, which can slow down the assembly rebuild speed. Therefore, in addition to the other reasons for removing in-context relationships, we must consider the performance of the assembly.

CREATING IN-CONTEXT FEATURES

In SolidWorks training classes, creating in-context parts involves a specific method. When adding a new part to an assembly, you select a plane or planar face and the part is given a default name. The selected plane orients the Front reference plane of the new part while an InPlace mate is added to the assembly to maintain the position of the new part. The assembly origin is projected onto the Front plane of the new part to determine its origin location.

When building parts within an assembly, the selected plane face becomes the active sketch and the part is in Edit Part mode. Standard methods and references to other geometry in the assembly are used to create the part.

In-context features are created by referencing geometry from another part while making a feature. This creates a relationship between the referenced geometry and the feature. For example, referencing the edge of a shaft when creating a mating hole in another part creates a relationship between the two. If the diameter of the shaft is changed, the diameter of the hole will correspondingly change.

INPLACE MATES

The InPlace mates that are automatically created for in-context parts serve the purpose of preventing the part from moving. This is because the in-context part is connected to the geometry of the parts in the assembly through external references that cross between parts at the assembly level. If the location of the part is changed, it can cause undesired changes to the geometry.

To replace InPlace mates, you can use standard mate techniques to remate the part and provide a degree of freedom for movement. It is recommended to select a face that is perpendicular to the direction of motion, as this will not affect the part origin. If you delete an InPlace mate, a warning message will appear after the confirmation dialog.

The base sketch of the part located by the InPlace mate contains references to other entities in the assembly. These references may update unexpectedly after the mate is deleted because the part will no longer be positioned relative to the assembly. You will be prompted to remove these references, although no geometry will be deleted.

ERRORS

To ensure a seamless process, it is highly recommended that you deal with any rebuild and import errors as they arise. It is always easier to address a rebuilding issue as soon as it occurs, as this allows you to pinpoint exactly where the problem originated. If you choose to continue building a part with errors present, you will find that the errors will compound over time, ultimately requiring significantly more effort to resolve than if you had tackled them immediately. The same principle holds true for import errors, which should be fixed before any further edits are made to the part. Failing to do so is akin to building a house on a shaky foundation, and can lead to major complications down the line.

One tool that can be particularly helpful in identifying potential import issues is Import Diagnostics, which should be run anytime you import a new model. This tool is designed to flag any potential issues caused by geometry with errors, allowing you to address them before they can cause any major problems. However, it is important to note that once you add additional features to an imported part, Import Diagnostics will no longer be available, as it only works on an unmodified imported body.

Another useful tool is Check, which can be used at any time to locate geometry errors and undesirable geometry, such as short edges, that may cause other geometry to fail. This tool can be accessed through the CommandManager by selecting Evaluate>Check or through the Tools menu. By using Check regularly, you can ensure that your parts are always in top shape, helping you avoid any potential issues down the line.

EXTERNAL REFERENCES

In order to establish and maintain relationships between parts in the assembly, external references are utilized by in-context features. However, to prevent the breaking of these references and maintain the integrity of the part, it is necessary to manually modify the in-context references to local references. External references are considered in-context when they function properly, but out of context when they fail to update correctly.

In-context relationships are preserved in the Update Holders 3 assembly. For an in-context feature to work effectively, the assembly must be open to allow for updates. Changes can only be propagated through the assembly while it is open. If a part is out of context, opening the externally referenced document and selecting Edit In Context from the right-click menu on the out-of-context feature will put it back into context.

The Lock/Unlock and Break options temporarily or permanently stop the flow of changes. These options suppress the Update Holder, which speeds up the assembly rebuild. To create a duplicate part that is not tied to the assembly, in-context references should be removed by copying and editing the in-context part. Once in-context features are created, it is recommended to lock the external references. If changes are made that affect the in-context features, the external references can be unlocked, the assembly rebuilt, and then the external references locked again.

When the List External References dialog is active, Lock All and Break All options are available. Lock All freezes the references until they are unlocked. When the references are locked, changes will not propagate to the part. The FeatureManager design tree lists the locked references with “->*” symbols. Break All breaks all references with the controlling files. Once broken, changes will no longer propagate to the part. The FeatureManager design tree lists the broken references with “->x” symbols. Break All does not remove the external references, but simply breaks them irreversibly. Therefore, Lock All is recommended in most situations.

To permanently stop changes, it is best to use File, Save As with the Save As Copy option to copy the part and remove the references. When parts are built in-context, unexpected changes could occur if mates are removed or in-context parts are used in other assemblies. In-context references must be removed prior to out-of-context use for re-use of data and improved assembly performance.


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