Increasing SOLIDWORKS Performance with Modeling Methodology

Before we can discuss model performance, we need to first define what criteria we will use for defining performance. Is performance based on load times and rebuild times? Is performance based on the ease of modifying our models? Or perhaps we define performance on consistent modeling practices. In actuality, we need to take all these criteria into account when we talk about model performance.


Part Templates

The starting point for modeling performance is the part template. At minimum, the part template should capture the units that we will use for our projects, but templates can also define what materials we will work with. We can even have templates that contain a basic layout sketch or feature, which all our parts are derived from. Well-defined templates can enforce standardization and reduce design time. Templates can also help also reduce the learning curve for new employees by clearly defining company standards.

The part template can and should also contain custom and configuration-specific properties, which will be referenced by downstream documents, such as drawings as well data management applications. To ensure that the input of these properties is consistent, we can use SOLIDWORKS’ Property Tab Builder to create templates for entering our properties.

Property Tab Builder. (All images courtesy of the author.)

Once these properties are created, they can be linked to notes in a title block, general notes or a bill of materials.



Now that we have a template that will ensure consistency in our models, we will look at how our sketches can also increase model performance. In the SOLIDWORKS Essentials training manual, at the end of the second lesson, there is a list of sketching best practices, which was my humble contribution to that manual. I will cover some of those practices in this article.

Complex sketches are more prone to rebuild errors and harder to edit and can prevent the use of configurations. When we create our first feature, we may be tempted to incorporate as much detail as possible, with the intent of saving time. But in reality, we could be adding time to the overall project.

Often, more time is spent on editing our design than was spent in creating it. While actual figures may vary, a conservative estimate would be that 15 percent of the total design time is spent on the original design, while the rest is spent on making changes. I have always found that creating a simple first sketch\feature, which captures the overall shape or key element of a model, lends itself best to later edits. Often these first sketches consist of a simple profile.

When creating your sketches, try to capture your design intent with sketch relations or equations. A good design has only one key dimension that will update all related sketch entities or model features. The more dimensions that need to be edited in order to complete a model update, the greater the chance that one will be forgotten. This can lead to costly manufacturing errors.

Take advantage of symmetry. Dynamic mirror and mirror entities can reduce modeling times and maintain design intent. Centering the first sketch of model about the origin can facilitate the application of symmetry.

Sketch centered on origin.

Rebuild errors can significantly increase rebuild times. Just because the software allows you to save a model with rebuild errors doesn’t mean you should. Tools such as Check Sketch for Feature and SketchXpert are great tools for dealing with sketch errors.

Use fully defined sketches. Fully defined sketches can prevent accidental model changes when under-defined sketch geometry is unintentionally moved. Fully defined sketches may even increase model performance, but I have not come across any definitive proof of this recently. Perhaps this was true at the advent of SOLIDWORKS, when computers were far less powerful. Nevertheless, preventing accidental model changes should be enough reason to use fully defined sketches. The Fully Define Sketch tool can be useful in accomplishing this goal.

Fully Define Sketch dialog box.



The order in which features are created can impact the ease of editing models. Boss extrudes should be done first, as a downstream boss extrude may result in the preceding cut extrude being filled.

Boss-Extrude backfilling a proceeding Cut-Extrude.

Fillets and chamfers, while important to the manufactured product, may not be required to create downstream features. Fillets and chamfers can significantly impact rebuild times. Consider creating these features last. Also consider creating a configuration where these features are suppressed. This configuration can be used when the model is being edited.

As with sketches, taking advantage of symmetry can also help maintain design intent. Instead of blind extrudes, consider midplane extrusions as the first feature in your model.

Boss-Extrude end condition.

Consider using feature end conditions, such as Up To Surface, Offset From Surface and Up To Next, as a means to maintain your design intent. Proper use of model end conditions is key to creating efficient models.

Avoid excessive detail. Is that text feature required, or can you get away with a decal or a simple sketch? The geometry generated by extruded text can significantly increase rebuild times. Model threads can have an even larger impact on performance. Consider using cosmetic threads instead.

Cosmetic Thread dialog box.

Again, deal with rebuild errors as they occur. The What’s Wrong dialog box can provide help in fixing rebuild errors.

What’s Wrong dialog box.

The FeatureXpert can provide alternative solutions that will eliminate rebuild errors.

FeatureXpert option in the What’s Wrong dialog box.

Often the level of detail required for an assembly is much less then what is required for a model. For example, consider a gear. The amount of detail that is required to manufacture a gear is likely much more then what is needed in an assembly. In an assembly, we often only need to consider the volume of the gear.

Left: Fully detailed gear from the Toolbox. Right: Simplified gear.

Reducing the amount of detail will increase assembly performance. The same concept can also be applied to configurations used for drawings.

If you work with imported geometry, checking for import errors can prevent downstream feature failure and increase performance. Whenever a model is imported into the software, Import Diagnostics should be executed on the model. This is done by right clicking on an imported body or surface.

Import Diagnostics dialog box.

This tool is not available once you create a new feature in that model. Therefore, it is very important to run this tool before any further work is done. Faulty faces can prevent creation of features that reference them or cause these features to have rebuild errors. I have seen numerous cases in which users have lost hours of design time because of faulty faces. Once a faulty face impacts a design, often the only recourse is to delete all the features and then restart the design by first running Import Diagnostics.

Inserting an existing part into a new model can be an efficient way of starting a new design. This is often referred to as using the Master Model approach. Keep in mind that you are creating references to external models, which need to be maintained by solid file management practices.

In this article, I covered key aspects to creating efficient models. Following these practices as well as developing a consistent methodology to creating your models will increase efficiency. Remember, modeling is not a one-off task. Models will be modified, and they will be referenced by other documents. Spending time at the beginning of a design will inevitably save you more time over the course of the project.

About the Author


Joe Medeiros is a senior applications engineer at Javelin Technologies, a SOLIDWORKS reseller servicing customers throughout Canada. Medeiros has been involved with SOLIDWORKS since 1996. He regularly blogs about the product and has won awards for his blogging.

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