How robust are your SolidWorks CAD models?
Why is 'robustness' of CAD important?
Unstable models can create frustrating rebuild errors and fail the moment you begin editing core established features in the tree. These frustrations are escalated by the time and cost implications to projects and deadlines due to agonisingly rebuilding the model tree step by step. Developing larger projects through concept, prototyping and production with a lack of parametric consideration can accumulate to days and potentially weeks of wasted time rebuilding CAD models. In this article we intend to share some useful tips for building a robust CAD model and also to ensure working file handovers run smoothly.
Planning your model: The foundation of efficient and stable CAD
We can’t stress enough how important planning the modelling process is, especially for large complex models where design constraints are not always clear from the beginning. Taking up to an hour to plan your modelling approach can help streamline your workflow, increase stability and often saves hours of frustration when updating designs. Here is your checklist to run through next time you plan a SolidWorks model.
Have a hand sketch reference
The process of modelling even the simplest parts can be streamlined by putting pen to paper and generating a quick sketch. Use this sketch as a reference and try to fill in any key dimensions before you enter CAD. For quick 3D printed jigs, it's best to take note of all the measurements of the product in a hand sketch before modelling rather than interrupting the modelling process to take out the callipers.
For more complex fluid forms, designing as you drive in SolidWorks can be dangerous and sometimes your creativity can be limited by your skills using the software. The best approach is to have a clear direction as to the form you want to achieve before starting your model. Often if a form is well defined in hand sketches, they can be scanned in and inserted as a reference within your model as a ‘sketch picture’.
Choosing your origin
Choosing the most logical origin position can dramatically simplify your model complexity.
- For designs with clear lines of symmetry, the origin should pass through this line of symmetry so one of the defined planes can be used for mirroring features/sketches.
- Consider which face on your design should be the front face of the model. This is usually determined by how you hold the product or interact with it.
- For non-symmetrical models, try to position the origin in a functional area with some consideration on how the planes may be used later in the model tree.
How will it be manufactured?
How the part is manufactured can also help determine your modelling approach. If you are creating a master model part with some sheet metal components, it's best to model the sheet metal using standard features and converting them to sheet metal components when they are exported into their separate part files. Alternatively, if you are modelling a single body sheet metal part, strongly consider using the Sheet Metal features from the offset. For moulded parts, it's worth considering matching one of the 3 core planes to the direction of pull for your draft.
The key features
There's nearly always more than one approach to creating a part. Simplicity and consideration are always at the heart of good practice in SolidWorks. It’s important to think about the key forms in your design and the most efficient features to create these. You can then plan where certain sketches and planes are needed to constrain these features. Often people jump into surface modelling when solid features such as sweeps and lofts can achieve the same complex geometry but more robust and in fewer steps.
Think about your sketches
Keep your sketches simple. Try to think beyond the fillets in your design. Avoid adding sketch fillets where the fillet feature can perform the same action towards the end of the model tree. Master sketches can be useful for laying out key interactions between components on the same plane. This is where one sketch is used for multiple features and therefore the interactions of these parts can be easily controlled. Sometimes when these sketches are absorbed by other features their purpose can be overlooked, therefore this sketch must be identified in the model tree.
Consider if there is anywhere in your model that could benefit from this approach. Not fully defining your sketches in SolidWorks is undeniably an engineering sin! Splines seem to be a key feature many users under define. Measured dimensions are best for defining splines but they can also be easily manipulated into the desired form and then constrained with a ‘fixed’ relationship. To make sure undefined sketches are never the cause of your unstable model, tick the ‘Use fully define sketches’ box in SystemOptions>Sketch. This should be enforced across all SolidWorks users.
Also, consider what part of the model you dimension your sketch to. Understand when it’s best to dimension sketches to planes, axis, other master sketches, absorbed sketches, model points and edges. It’s rarely a good idea to dimension your sketch against a fillet!
Think parametrically
It's important to think parametrically so your model is easy to update and rework. Define the key relationships within your model geometry and plan how these relationships are easily adjusted. If there are areas in your model that rely on the same dimensions but have not fully been defined, for example, material thickness using the shell feature, then consider adding this parameter as a global variable. Global variables become even more useful if you plan to create multiple variations of the product using separate configurations.
Underused features and quick tips to increase your model stability
Through our use at IDC, we have found some interesting tools which can help check and ensure the stability of models.
Verification on rebuild
Have you ever returned to a very complex model, only for rebuild errors to appear on your tree where there were none previously? When first modelling the part, SolidWorks identified the geometry of the feature as being sound, and therefore there were no errors. However, when recalculating the rebuilding of the model, it can pick up an error that has been missed previously.
Once this rare event has happened, it can be very difficult to return to the source and correct it without affecting the majority of the model tree. To avoid a complete breakdown, some models have to be frozen before a certain point to keep stability and prevent breaking on rebuild. The key to successfully avoiding unstable geometry is pre-empting the areas in the model tree that create complex geometry and therefore require extra attention to stability. You can then apply the ‘Verification on rebuild’ performance option.
When SolidWorks generates any part geometry, it considers how that feature is being generated at the specific mathematical location within the model. It doesn’t consider the other faces outside of the feature scope. However, when 'verification on rebuild' is activated, from this point on in your model tree, SolidWorks considers how the feature affects all other geometric features within the model. If any dodgy geometry has been detected, SolidWorks will prevent the feature from being generated and will immediately produce an error for review.
Evaluate > Check Entity
If you are concerned that you have already modelled something with an invalid geometry, you can always use the ‘Check Entity’ tool in the evaluation tab. This will highlight any inconsistent geometry features in your model, even if you don’t have any rebuild errors. However, this is an evaluation tool and therefore will not help solve your original mistake.
Solving sketches
When you’ve updated features in your tree and it’s common for warnings to appear on some of your sketches relating to the updated feature. It's not always easy to see why sketches have become over defined. Normally, there are two approaches to quickly solving these relationships.
- Right-clicking on the workspace and selecting ‘display entities’. Here you can filter and delete the dangling and over defined relationships. It’s then a matter of redefining these relationships manually.
- Sketch Expert is a powerful yet often overlooked tool taught on the SolidWorks Essentials course. The program can automatically Diagnose the sketch and produce various solutions by removing conflicting dimensions and relations. It’s then a matter of cycling through these variations to select the desired outcome.
Sharing CAD and maintaining a solid transfer of knowledge
Whether you’re working in a team internally or externally, inheriting a CAD model from another user can often be an insight into their way of thinking. Working on these designs without prior knowledge of the thought process can be dangerous to the integrity of the model, causing frustrations, increasing costs and draining resources. Below are some key points to consider to maintain CAD efficiency when sharing your files.
Fundamentals for digestible CAD models
Name your key features, sketches, equations and use named folders to structure the core sections of your model. Folders are especially useful when navigating larger and more complex models. However, avoid adding folders within folders. SolidWorks has a tough time rebuilding and recognising features buried deep in layers of folders.
Although they are rarely used, adding Comments to some features explaining your logic can help prevent any ambiguity regarding why they are there or how they are generated. You can add images, screenshots of the model and timestamps to every comment, but be warned, SolidWorks by default does not show the Comment indicator beside each feature. To make sure you don’t miss any, right-click on the tree and select TreeDisplay>ShowCommentIndicator.
The Design Binder
The visibility of this tool in SolidWorks is off by default, and so it is often missed by users. To show the Design Binder go to Tools>Options>System Options>FeatureManager>DesignBinder>Show.
You now have access to an embedded document you can edit and use to track your rationale and create a guide as to how to manipulate your model. This is particularly useful where you need to record equations, relative OEM part information and configuration features that are essential to your design. The Design Binder also lets you embed or link other relevant documents such as OEM part, material Datasheets and Design Guides.
Inheriting a model: Where to start?
In an ideal world, CAD handovers should come with a meeting where the creator talks through the model step by step. When models are dropped on your lap without a proper handover process in place, the logical thing to do is to determine how the previous user modelled it.
- Knowledge Transfer - Inspect the model for comments, equations, configurations, and any information transferred through the Design Binder. When you open the equations tab, each equation will show exactly what features it relates to.
- Folders and Features - Note the naming and order of the folders and features in the model tree. The model has been built in this specific order for a reason.
- Rollback – Run through the model step by step and try to identify where the dependencies and logic of the creator. Most people use the Rollback bar on the model tree for this process, but users often overlook the Part Review feature, which makes the process more streamlined. Instead of dragging and dropping the Rollback bar for every feature, the Part Review tool allows you to cycle through by clicking just one button. This tool also highlights any comments associated with each sketch or feature, ensuring they are not missed as you review the part. Viewing all the sketches in the model unabsorbed by features can be a useful way to review the modelling process. To do this, simply right click the model at the top of the tree Tree Display>ShowFlatTreeView.
Compare your updates and check for errors
When parts from your assembly need to be edited and updated, if you don’t have a full understanding of the master model with some complex dependencies, it can sometimes be easy to make small unintentional changes missed by the naked eye. Use the Compare tool to compare the geometry of previously issued parts to your client/manufacturer before up-issuing your part. This tool can help highlight any geometry that differs from your previous models and ensure any unintentional mistakes are caught before it’s too late.
We hope this post highlights some features you may find useful in your own developments. We'd love to hear which parts caught your attention or were most interesting!
At IDC, all of our design engineers progress through the SolidWorks certifications to become more proficient. If SolidWorks training or certification is something you'd like to learn more about for your team - we suggest speaking with the guys over at SolidSolutions. You can take a look at the available courses HERE.
About the Author
Kevin O'Malley is a Product Design Engineer with experience developing medical devices and consumer products. He became a certified SolidWorks Expert at IDC after completing a Master's Degree in Product Design Engineering from the University of Glasgow and Glasgow School of Art.
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