How to use SOLIDWORKS envelopes

Envelopes are a special kind of part or assembly.

It’s a reference model that does not affect your assembly mass.

You can also select all components within an envelope.

In this post I’ll show you how to use them.

When do you need envelopes?

When you are designing a part, you have to make sure it fits into the rest of the assembly. How do you do that right now?

Do you edit the part in the context of the assembly? That slows down your whole PC.

Do you temporarily add the housing to your subassembly? Doing so will add the housing twice.

You can use envelopes as a permanent reference within an assembly, without messing with the mass or having the part showing up in your drawings.

How to turn a part into an envelope

Every existing part or assembly can be used as an envelope.

You can even use virtual components.

Say you are designing this assembly (from the CSWA certification test) and you want to fit it inside a pre-existing housing.

By the way, you are entitled to two free exam vouchers a year when your company is on a SOLIDWORKS subscription! SOLIDWORKS will send you a code via SMS  when you visit Certification Offers for Subscription Service Customers so you can earn official certifications.

SolidWorks certificate CSWA CSWP CWSE

To turn a model into an envelope:

  1. Open an assembly
  2. Right click a component (part or assembly) in the feature tree and select Properties.
  3. Set it as an envelope part in the bottom right corner.
SolidWorks turn a part or assembly into an envelope

Turning a part or assembly into an envelope

Properties of an envelope

Beside its paper-holding capabilities, an envelop model has the following properties:

  • You can mate other parts to it
  • The mass of the envelope will not count toward the assembly mass.
  • SOLIDWORKS shows the envelope part as blue and translucent by default.
  • The icon in the feature tree gets an extra envelope
  • Be up to 100% faster when making drawings
  • Never use a wrong template again
  • Create a new drawing with one click
  • The envelope does not show in drawing views by default.
  • The checkbox “Exclude from bill of materials” is checked automatically and cannot be turned off. This means that the envelope model will never appear in a BOM.
    • This is why working with envelopes is way better than copying parts into multiple assemblies and then suppressing or deleting them when the design is done.

You can change the default color in the settings by going to Colors > Color scheme settings > Envelope Components.

envelope icon feature tree

How to show envelopes in a drawing view

Envelopes are hidden in drawing views by default.

To show them, right click a view and select Show Envelope.

solidworks show envelope in drawing view

Hide all envelopes in an assembly

Of course you can still hide, show and suppress in all of the usual ways.

If you like to hide all envelope models though, right click the top assembly in the feature tree and click Hide All Envelopes. The name says it all.

hide all envelopes in assembly

How to select all components within an envelope

You can create a model with a certain shape and volume that should contain a machine or parts of it.

You can then use this envelope to do advanced selections. I like the sound of that. There are two methods:

Method 1: via the feature tree

When you right click a envelope and select Envelope, you get the options Select Using Envelop and Show/Hide Using Envelope. I’ve combined both forms in the second image below.

select all parts within an envelope

hide or show all parts within an envelope

You can now select, hide or show all models that fall within or outside of the envelope. Pretty neat, right?

Method 2: Advanced Select

I must say I have never used the advanced selection tool before, so I might just start now.

Have you ever really noticed this pointer in the main menu?

SOLIDWORKS advanced select

We’re going to open the last one. This window gives you very advanced ways of creating selections.

I’m certain I will use this feature in the future to select parts based on their mass.

solidworks advanced select components within envelopes

Summarizing

When you use the envelope feature, you are creating a good reference for the rest of your assembly.

Without accidentally having a part within your assembly twice. The component does also add no mass and never shows up in the BOM.

The selection methods make it a very useful feature for collaborating as well, because everyone can be given their own envelope to stay in.

In my last project, defined bounding boxes could have saved us a lot of trouble because we were constantly interfering with each other’s space.

So do you think you will use envelopes in the future? If you are a lead engineer, you can set the path for your colleagues to do so.

Want to learn more?

Check out our mega article on balloons or the posts about Origin mates or virtual parts.

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