Advanced Assemblies: What are Envelopes in SOLIDWORKS and when to use them?

How to Create Envelopes in SOLIDWORKS

Envelopes can be created in-context within an assembly or from inserted SOLIDWORKS parts or subassemblies.

Envelopes can be created when inserting parts or assemblies into an assembly. Before placing a component, select the ‘Envelope’ tick box in the Insert Component property manager.

’In-context’ components that have already been inserted into an assembly can also be converted into envelopes.

Right-click on the desired component and access the Component Properties from the right-click menu.

Within the Component Properties window, check the box for ‘Envelope’ to convert the component into a weightless envelope component.

Here it’s important to note that the option to ‘Exclude from bill of materials’ is checked by default and cannot be turned off for envelope components.

These envelope components are excluded from mass properties and other evaluation tools as they are ‘for reference only’. However, they can be used to mate to, dimension from, and position other elements.

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Referencing Top-Level Components with the Envelope Publisher

The Envelope Publisher allows us to create envelopes within subassemblies from the top-level assembly.

That way, we can build reference components into subassemblies like this kitchen unit and improve performance while making design changes.

We want to maintain the sink and plumbing components as references but exclude their mass and material properties from the unit assembly. As this is a top-level assembly, we can use the Envelope Publisher tool to create envelopes from our top-level assembly.

The Envelope Publisher feature which is found under Tools > Envelope Publisher.

Once in the property manager, we can select the components to include in the envelope and then any destination sub-assemblies they will be added to.

1. 1. Envelope Components are those that will comprise the final envelope. Add these to the blue ‘Components to use as envelopes’ box by selecting them from the viewport or the FeatureManager Tree.For our example, these will be any components that do not comprise the unit – the sink and tap components.
   2. Destination Subassemblies are any sub-assemblies that the envelope will be added to.Again, select these from the viewport or the FeatureManager Tree to add them to the purple ‘Destination Subassemblies’ box. In our case, this is the under-sink unit.

The Envelope Publisher property manager and the final selections.
1. Click ‘Add group’ when all selections have been made.

Additional envelopes can be created by repeating the selection process. For this example, we just need the one envelope so instead we’ll hit the green tick to confirm the command.

On confirming the command, we can open any of the selected destination sub-assemblies and see our new envelope.

Envelopes vs Interference Detection in SOLIDWORKS

A common misconception is that SOLIDWORKS envelopes can be used for determining component interferences.

However, as they are excluded from mass calculations, envelope components cannot be used within the Interference Detection tool and therefore actually hinder any interference evaluation.

The under-sink cabinet with our shelf modification.

Take the model of the kitchen unit above. While we could technically achieve the shelf modification illustrated while using envelopes as reference components, we would not necessarily be alerted to interfering geometry.

It is therefore best practice to return the component(s) to a non-envelope state by right-clicking on the component, going to Component Properties, and deselecting the ‘Envelope’ checkbox from the Properties window.

This will return the component to its normal state and allow it to be used in interference detection calculations, in this case checking whether someone would have adequate space to move around in the fitted kitchen.

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How to Change the Appearance of Envelopes in SOLIDWORKS

Changing the appearance of envelopes can help to differentiate between envelope and component geometry as well as improve clarity in drawing views.

The default appearance for envelopes in SOLIDWORKS is a transparent, light blue colour and is visible in parent assemblies as well as any ‘destination’ subassemblies.

The colour of envelopes can be altered under System Options > Colors > Envelope components in the colour scheme settings list. Click ‘Edit…’ to choose a new colour for envelope components.

Similarly, on the same System Options > Colors tab, the transparency can be modified using the dropdown at the bottom of the window.

Individual envelopes can be shown and hidden like any other SOLIDWORKS component from the FeatureManager Tree. To hide or show all envelopes, right click the top-level assembly name in the feature tree and select ‘Hide All Envelopes’.