Editing Assemblies in Large Design Review

You can use Edit Assembly to edit assemblies in Large Design Review mode. You can add and edit mates, and insert components when you edit an assembly.

To use this functionality, open the assembly and component files individually and then save in SOLIDWORKS 2019. Click File > Save All to save all the open files at the same time.
In the FeatureManager design tree, the following features appear for top-level assemblies:
  • Standard planes
  • Origin
  • Mates folder
  • Reference geometry, read-only
  • Sketches, read-only
  • Component Patterns, read-only
On the Large Design Review tab of CommandManager, these tools are available:
  • Insert Components
  • Mate

You can use Move with Triad. To access this tool, right-click a movable component and click Move with Triad .

You cannot insert a component by dragging it from the Task Pane or File Explorer. You cannot copy a component using CTRL + drag or CTRL + C. You cannot paste a component into the assembly.

You cannot edit an assembly in Large Design Review mode if the top-level assembly contains at least one of these features:
Belt/Chain Chamfer Circular Pattern (feature)
Extruded Cut Fillet Hole Series
Hole Wizard Linear Pattern (feature) Mirror (feature)
Revolved Cut Simple Hole Sketch Driven Pattern (feature)
Swept Cut Table Driven Pattern (feature) Weld Bead

To edit assemblies in Large Design Review mode:

  1. Click Open (Standard toolbar) or File > Open.
  2. In the dialog box, select an assembly, and then in Mode, select Large Design Review.
  3. Select Edit Assembly.
  4. Click Open.

    An eye overlay appears on the icons of all components indicating that the assembly is in Large Design Review mode.

To edit an assembly that is open in Large Design Review mode, right-click the top-level assembly, and click Edit Assembly.

Creating Mates in Large Design Review

When you edit assemblies in Large Design Review mode, you can create mates between components and use geometry types as mate references. These mates and mate references are available when you open the assembly in lightweight or resolved mode.

Supported mate types:
Angle Lock
Coincident Parallel
Concentric Perpendicular
Distance Tangent

You can use the following geometry types as mate references for any component in the assembly:

Arc edges Conical faces Cylindrical faces
Linear edges Planar faces Vertices

Temporarily Fixed Components

For existing mates or mate references that are not supported in Large Design Review mode, the mates and mate references appear as temporarily fixed .

Flexible subassemblies perform like rigid subassemblies in Large Design Review mode.