Written by Jared Spaniol, Elite Application Engineer
When working with assemblies in SOLIDWORKS there are always a few common questions that come up like where to start, what should my base component be, how can I reference other components, what is top-down or bottom-up modeling, which method should be used etc. In this webinar preview I’m going to tackle these questions and more.
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First, where do you start as far as modeling the assembly itself? The first component added to an assembly is typically the most logical base component such as a frame. All the other components would be mounted to this base component. For example, if you’re modeling a vehicle you would start with the frame which is where you would start the actual assembly process opposed to say, bringing in the wheels first. The wheels, axles, body, engine, and so forth all mount to the frame.
Second, let me explain the two main modeling strategies that are typically accepted in the 3D CAD world. Assemblies can be created using a bottom-up or a top-down strategy. The easiest way to remember the difference is bottom-up means utilizing components that are already modeled and pre-defined. These bottom-up components will be added to an assembly and mated in place. Think of LEGOs, you’re combining the pre-built blocks into place to build something. This is starting from the bottom and building up with parts that are independent of each other, meaning they are not related and have their own relationships and dimensions in each individual part. The disadvantage of this process is you must know the components’ dimensions beforehand and have confidence they will all fit together, or you end up adjusting on the fly to make sure they fit once assembled. This process can be easily started with the insert component command shown in Figure 1. Then continue with the typical mating of components to each other or the base component to constrain the appropriate degrees of freedom.
Figure 1: Insert components with Bottom-Up Strategy
The top-down strategy means that you’ll be modeling parts within the context, or “in-context” of the parts that already exist in the assembly. You’ll be building relationships and dimensions off other components that are now external to the parts being assembled. The advantage with this method is multiple parts and features can be updated simultaneously. For example, if you have a plate with some holes mounted to another component they can be built separately with bottom-up and mated together, but you must know the locations of the holes in both components and make sure they line up when assembled. With the top-down strategy you can reference the location of the holes in the mounting plate to the other component and if the hole location or size changes in one component the change will propagate in the other component ensuring the holes always stay lined up.
Modeling in-context is quite simple once you understand the workflow. It starts the same way you would normally begin working in an assembly. Instead of insert part, use the new part command to begin creating a new part in an assembly. This can be found in the insert menu>component flyout>new part or new assembly (See Figure 2). One thing to note when creating the new part within the assembly is that there is a setting in the system options that controls if the part is saved internal to the assembly or saved as an external part. This setting can be found in Options>System Options>Assemblies>Save new components to external files. If you want the new components to be automatically saved externally make sure this box is checked. This can also be done later by RMB clicking on the component and selecting the “save part in external file” option.
Figure 2: Insert components with Top-Down Strategy
Once the new part command is started SOLIDWORKS will ask where you want to place the part. Select a face or plane to place your part, this establishes an “in place” mate. Now you can begin modeling the part and using features or sketches of existing components to define the new part. The easiest way to do this is with the convert entities and/or offset entities commands. These commands will allow you to easily take advantage of the existing geometry and create simple relationships. These relationships are now defined external to the part. There is a symbols key that defines the state of the external references shown here in Figure 3. It is beneficial to know what these mean when looking at the feature manager design tree.
Figure 3: State of External References
All the external references can be listed, broken or locked. Use the RMB to select the part and then choose the external reference option from the drop down which will open the dialogue shown in Figure 4. Within this dialogue you can see the status, what entity is being referenced, and the type. There is also a filter by status bar so the type of references can be filtered if there is a long list here. There is an option to “Lock all” or “Break all” within this dialogue as well. If the “lock all” is selected this freezes all the references in place so they don’t change when referenced components change. This option can easily be reversed by unlocking the references. The “break all” button breaks all the references and this change cannot be undone which SOLIDWORKS will warn you about before proceeding.
Figure 4: External Reference Example
The final question to be answered is which method is preferred and this will be determined by the end goals of the user. There are a few guiding questions to help with this selection process. Ask if this is a part that will be used in other models and if so, then top-down modeling might not be the best option since the part will have external references and could change unintentionally. The references can be broken and re-defined with the typical methods of defining a sketch, but that is extra steps for the user. Keep in mind that top-down models take longer to rebuild because they can contain many external references to solve. It is also a good practice to add features that won’t contain external references in the part file opened outside the assembly which will simplify things for the user.
Both methods have a place and it is good to know both directions so the user can choose the best option for their specific case. Be flexible with these strategies, use them in combination, and don’t limit yourself to one or the other.
If you found this information helpful, want to learn more, or have questions: Join the upcoming Webinar on April 24 at noon est. Register Here