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 you are opening (Part, Assembly, or Drawing). This article is broken into 3 sections, one for each file type.
This is not a troubleshooting guide. If you have any technical issues with SOLIDWORKS please contact Hawk Ridge Systems technical support.
Contents
Selecting the Opening Mode (All File Types)
Selecting the Opening Mode (All File Types):
The file opening modes are available for all file types when opening the file via the
SOLIDWORKS File > Open command, before selecting Open.
If you open a file through Windows File Explorer you will not be given these options. By opening the file through the SOLIDWORKS Welcome page or Recent Documents, you can expand the arrows in the bottom right-hand corner to see these options.
Parts
Resolved
This is the standard loading method for parts, and all data is loaded. You can also select the Configuration and Display state in which you want 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
Quick View mode allows you to view the part but has many limitations. You can zoom, pan, and rotate, but cannot edit, measure, or save the file. You can only select configurations that have had the "Display data mark" added to them. You cannot select display states. You cannot 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 > Edit.
Assemblies
Resolved
Opening an assembly in Resolved mode loads 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.
You can also select other options, such as Load hidden components, Use Speedpak, and Use Large Assembly Settings. You can also set the configuration and display state you want 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 - 2024 - SOLIDWORKS 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 - 2024 - SOLIDWORKS Help
Lightweight
Opening an assembly in Lightweight mode opens 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 Lightweight, components will have a blue feather displayed in the FeatureManager Design Tree:
You can toggle individual components between Lightweight and Resolved mode by right-clicking them in the FeatureManager Design Tree > Set Resolved to Lightweight or Set Lightweight to Resolved.
If you wish to toggle all components in an assembly (whether the top level assembly or a subassembly), right click the assembly in the FeatureManager Design Tree > Set Resolved to Lightweight or vice-versa.
In Lightweight mode, you can still perform most actions. For a full list of available actions, please see: Lightweight Components - 2024 - SOLIDWORKS 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 Lightweight vs. Resolved, and does not require manual input. Components loaded lightweight in this method will not be displayed with the blue feather.
- Manually manage resolved and lightweight modes: this option allows you to set your preferences for loading components Lightweight vs. Resolved.
You 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
Opening an assembly in Large Design Review mode opens it quickly with only graphics data. Geometry and feature data is not loaded. This mode does limit functionality, but you can turn on the checkbox for Edit Assembly to allow inserting components, adding and editing mates, and assembly level patterns. If your assembly contains flexible subassemblies, you 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 the assembly in Large Design Review, you 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.
Drawings
Resolved
Opening a drawing in Resolved mode loads all information about the referenced model(s) and typically takes the longest to load. All functions are available. Similar to loading an assembly in Resolved mode, you also have the options to Load hidden components, Use Speedpak, Use Large Assembly Settings, and locate or edit the file's references.
[Assembly drawing only]: Load hidden components: Turning off the loading of hidden components can decrease loading time, as hidden components will not be loaded into the drawing.
[Assembly drawing only]: 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 - 2024 - SOLIDWORKS Help
[Assembly drawing only]: Use Large Assembly Settings: 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
Opening a drawing in Lightweight mode loads only the graphics and geometry data. 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. You have the same options as for a Resolved drawing regarding hidden components, Speedpak, Large Assembly Settings, and the file's References. See Resolved (above) for details on these options.
When a drawing is opened Lightweight, drawing views will have a blue feather displayed in the FeatureManager Design Tree:
Lightweight Drawing Limitations
These will be loaded Resolved. This includes any component...
- that contains a Weldment part
- whose Model Items are imported into the drawing
- whose units differ from those of the drawing
- whose model is not updated to SOLIDWORKS 2009 or later
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
Opening a drawing in Detailing mode loads the drawing without part and assembly data. This mode limits functionality but opens faster than Lightweight and Resolved modes.
Limitations of Detailing Mode:
- You cannot create new drawing views (with the exception of Standard Views from the View Palette).
- You cannot create Centerlines, Center Marks, or Hatching.
- You cannot use the Undo tool.
- Draft quality section views cannot be selected or exported to DXF / DWG.
- You cannot create dimensions or annotations that require model information, such as Hole Callouts, Cosmetic Threads, or links to model properties.
Capabilities Available in Detailing Mode:
- You 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 - 2024 - SOLIDWORKS Help
- You can drag standard views (such as Front, Top, Back) from the View Palette into the drawing.
- You can change the position, rotation, and labels of existing drawing views.
- Add general, revision, and hole tables. You cannot add other table types.
- Save the file as a PDF or DXF, or print to PDF.
- There are other capabilities available, please see Detailing Mode - 2024 - SOLIDWORKS Help for a full list.
If you have any questions or would like further assistance, please contact our support team via our web portal: Hawk Ridge Systems Support, email us at support@hawkridgesys.com, or call us at 877-266-4469 (US) or 866-587-6803 (Canada).
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