Improving Workflow With Exploded Flat View in SOLIDWORKS

By Laura Weismantel on May 30, 2018

In many industries, quick manufacturing turnaround is an important element of the design process. When sending an assembly with multiple 2D flat components to a cutting machine, organizing and outputting these profiles can be tedious. If your workflow involves exporting these profiles as part of one drawing, the traditional technique is to create a view of each component, which can later be exported to a 2D format. For a faster alternative, keep reading! 

Creating an “Exploded” Flat View

A faster way to manage this is to create an Exploded Flat View of the components in your assembly environment and then add this single view (containing all profiles) to the drawing. The biggest challenge here is aligning all flat components to the same orientation, despite their assembled position. Because of this, the traditional Explode View command is not an easy solution.

Instead, we’ll manually move these components to a “flattened” orientation using configurations. This process is made very simple by utilizing multiple made mode–a extremely convenient and underutilized mate setting. To do this, follow these four steps:

1_Configuration-PropertiesStep 1. Create a new configuration of the assembly. Consider using a derived configuration, if configurations are already in use for a different purpose. The properties for both the parent configuration and the derived configuration should have new features, mates, and components suppressed automatically.

Step 2. With the new derived configuration active, suppress all positioning mates of the components you need the flattened view of. It’s also convenient to organize these mates into a folder so they can easily be suppressed and unsuppressed as needed. At this point, every component should be completely unconstrained and free to move, except for any fixed components.

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multiple mate modeStep 3. Create a mate between every components’ Front plane and the front plane of the main assembly. This can be done very quickly using multiple mate mode. You chose one common mate assembly, the front plane assembly in this case, and mate as many other entities as you want. To enable multiple mate mode, select the paperclip icon (pictured right) while in the mate command.

Step 4. This step is optional. Use multiple mate mode to create parallel (NOT coincident) mates between the top plane of the main assembly and the top planes of all individual components. This will help align everything to be perfectly horizontal.

At this point, a front view orientation of the assembly should enable you to easily drag and position all components, creating a nice 2D layout. This can be inserted onto a drawing and exported to DXF. Duplicate components can be hidden and the remaining components can be ballooned to indicate quantity or item numbers if they are referenced in a cut list.

Note: You may find the need to flip the orientation on some of the coincident or parallel mates to get them aligned correctly. 


Once all the “flattening” mates have been created, it is recommended to organize the mates into folders, classifying whether or not they are used to position or flatten the components. Also, in SOLIDWORKS 2018 folders in the feature tree are colored to indicate the state of components inside, such as hidden, showing or suppressed.

If you want to dig deeper into SOLIDWORKS techniques like this one, sign up for a 3D CAD training course!