Problem

This article details the various opening modes that exist for SOLIDWORKS files, including their advantages and limitations. There are different options available depending on the file type being opened (Part, Assembly, or Drawing). This article is broken into 3 sections, one for each file type.

The file opening modes are available for all file types when opening the file via the SOLIDWORKS File > Open command, before selecting Open.

When opening a file through Windows File Explorer, we will not be given these options. By opening the file through the SOLIDWORKS Welcome page or Recent Documents, we can expand the arrows in the bottom right-hand corner to see these options.

Solution 1: Parts

Resolved mode is the standard loading method for parts, and all data is loaded. We can also select the Configuration and Display state in which to open the part and check the file's References (if any exist). By default, Part files will open in Resolved mode unless otherwise specified.

Quick View mode allows viewing the part but has many limitations. We can zoom, pan, and rotate, but cannot edit, measure, or save the file. We can only select configurations that have had the "Display data mark" added to them. We cannot select display states or see the file's references. This mode is meant for viewing the file graphically without making any modifications to the file. To switch from Quick View to Resolved mode, right-click in the graphics area and select "Edit".

Solution 2: Assemblies

Resolved mode opens the assembly with all of its data. Typically, this mode takes the longest time to open, as all components, mates, and assembly-level features are fully loaded. Resolved is also the normal state for assembly components, unless opened in another mode or manually set to another mode. Resolved components are fully loaded in memory, fully functional, and fully accessible. All of a resolved component's model data is available, so its entities can be selected, referenced, edited, used in mates, and so on.

When opening in this mode, we can also select other options, such as "Load hidden components", "Use Speedpak", and "Use Large Assembly Settings". We can also set the configuration and display state to open and see or edit the file's references.

• Load hidden components: Turning off the loading of hidden components can decrease loading time, as hidden components will not be loaded into the assembly.

• Use Speedpak: If any of the subassemblies have Speedpak configurations, these will be used. If none exist, nothing will happen. For more information on Speedpak, please see: SpeedPak - 2027 - SOLIDWORKS Design Help

• Use Large Assembly Settings: This opens the assembly using Large Assembly Settings, which is a collection of system settings meant to improve the performance of assemblies. For more information on this, please see:
  Large Assembly Settings - 2027 - SOLIDWORKS Design Help

Lightweight mode opens the assembly to load the components with graphics and geometry data. After opening, feature data can be loaded as required. Lightweight mode is faster than Resolved mode.

When an assembly is opened in Lightweight mode, components will have a blue feather displayed in the FeatureManager Design Tree.

We can toggle individual components between Lightweight and Resolved mode by right-clicking them in the FeatureManager Design Tree to select  "Set Resolved to Lightweight" or "Set Lightweight to Resolved".

To toggle all components in an assembly (whether the top-level assembly or a subassembly), right-click the assembly in the FeatureManager Design Tree and select "Set Resolved to Lightweight" or vice-versa.

In Lightweight mode, we can still perform most actions. For a full list of available actions, please see: Lightweight Components - 2027 - SOLIDWORKS Design Help

There are a few options in Tools > Options > System Options > Performance > Assembly loading that control the automatic loading of lightweight components. 

• Automatically optimize resolved mode, hide lightweight mode: This option allows SOLIDWORKS to determine which components to load in Lightweight vs. Resolved, and does not require manual input. Components loaded in lightweight in this method will not be displayed with the blue feather.
• Manually manage resolved and lightweight modes: This option allows users to set their preferences for loading components in Lightweight vs. Resolved.

We can also set the Large Assembly Settings in Tools > Options > System Options > Assemblies > Opening a large assembly to automatically load using Lightweight mode above a specified threshold of component files.

Large Design Review mode opens assemblies quickly with only graphics data. Geometry and feature data are not loaded. This mode does limit functionality, but we can turn on the checkbox for "Edit Assembly" to allow inserting components, adding and editing mates, and assembly-level patterns. If the assembly contains flexible subassemblies, we cannot use the Edit Assembly option.

When an assembly is opened in Large Design Review, components will display an eyeball in the FeatureManager Design Tree. 

When opening an assembly in Large Design Review, we will be shown a list of available actions:

In Large Design Review mode, assembly-level features, component patterns, and mates are not shown in the FeatureManager Design Tree. Components that have multiple configurations will only show the last used configuration or configurations that have the Display Data mark. Assembly features that are not propagated to the part level may not display in this mode.

Solution 3: Drawings

Resolved mode loads all information about the referenced model(s) and typically takes the longest to load drawings. 

All functions are available similarly to loading an assembly in Resolved mode; we also have the options to "Load hidden components", "Use Speedpak", "Use Large Assembly Settings", and locate or edit the file's references.

• Load hidden components (Assembly Drawing only): Turning off the loading of hidden components can decrease loading time, as hidden components will not be loaded into the drawing.

• Use Speedpak (Assembly Drawing only): If any of the subassemblies have Speedpak configurations, these will be used. If none exist, nothing will happen. For more information on Speedpak, please see: SpeedPak - 2024 - SOLIDWORKS Help

• Use Large Assembly Settings (Assembly Drawing only): This opens the (assembly drawing) using Large Assembly Settings, which is a collection of system settings meant to improve performance of assemblies. For more information on this, please see: Large Assembly Settings - 2024 - SOLIDWORKS Help

Lightweight mode loads only the graphics and geometry data when opening a drawing. After opening, feature data can be loaded as required. Lightweight mode is faster than Resolved mode. A Lightweight drawing is analogous to a Lightweight Assembly. We have the same options as for a Resolved drawing regarding hidden components, Speedpak, Large Assembly Settings, and the file's References.

When a drawing is opened as Lightweight, drawing views will have a blue feather displayed in the FeatureManager Design Tree. 

The following components will always be resolved as limitations of Lightweight mode:

• Components that contain a Weldment
• Components Model Items are imported into the drawing
• Components whose units differ from those of the drawing
• Components whose model is not updated to SOLIDWORKS 2009 or later

Here are the Lightweight Drawing Capabilities:

• Create all types of drawing views
• Attach annotations to models in views
• Dimension models in views
• Specify edge properties
• Select edges & vertices
• Set drawings of subassemblies to Lightweight or Resolved modes

Detailing mode loads the drawing without part and assembly data. This mode limits functionality but opens faster than Lightweight and Resolved modes.

Here are the Limitations of Detailing Mode:

• We cannot create new drawing views (with the exception of Standard Views from the View Palette).
• We cannot create Centerlines, Center Marks, or Hatching.
• We cannot use the Undo tool.
• Draft quality section views cannot be selected or exported to DXF / DWG.
• We cannot create dimensions or annotations that require model information, such as Hole Callouts, Cosmetic Threads, or links to model properties.

Here are the Detailing Mode Capabilities:

• We can create most Dimensions and Annotations, with the exception of those listed above. For a full list of Dimensions and Annotations available, please see: Detailing Mode - 2027 - SOLIDWORKS Design Help
• We can drag standard views (such as Front, Top, Back) from the View Palette into the drawing
• We can change the position, rotation, and labels of existing drawing views
• We can add general, revision, and hole tables only
• Save the file as a PDF or DXF, or print to PDF

For additional support, existing customers can submit a ticket or new customers can contact Hawk Ridge Systems.