What’s New in SOLIDWORKS 2020 – Detailing Mode
Detailing Mode allows a user to load a drawing without having to load the referenced components. This can be useful when detailing drawings of large assemblies or if the drawing only needs to be provided to someone else.
Detailing Mode is similar to Detached Drawings, but unlike a detached Drawing, a drawing does not need to first be saved in Detailing Mode. Instead, the drawing is opened in Detailing Mode, similar to how assemblies can be opened in Large Design Review mode. In the Open dialogue box, when a drawing is selected, there are a number of modes to choose from, including Detailing Mode. A slider indicates the relative performance impact of each mode.
While not new for SOLIDWORKS 2020, Select Sheets has been moved conveniently close—to right beside the Mode selector. Previously, it was to the far-right of the Open dialogue box and easy to miss. I also like that Selected Sheets is displayed only for multiple-sheet drawings. This keeps the user interface focused.
Select Sheets allows users to decide which sheets will be loaded to work on. This can decrease open times and increase drawing performance. Once the drawing is opened, additional sheets can be loaded to work on as well.
If Lightweight or Resolved Mode is selected, the Use Speedpak option is available. Also, if Lightweight or Resolved Mode is selected, drawing References (components referenced by the drawing) can be modified.
After clicking Open, a dialogue box will list what can be done in Detailing Mode. This dialogue box can be dismissed.
When the drawing is opened, the top menu bar will indicate that the drawing is in Detailing Mode by displaying “Detailing” in brackets.
Opening a drawing in Detailing Mode when the referenced components have changed will produce a dialog warning the user that components may need to be updated, and gives the option to load the model.
This will only occur if the referenced components can be located by the search routines used by SOLIDWORKS. If the referenced components have been moved using tools other than the ones supplied by SOLIDWORKS, or if the referenced components are unavailable, then the user will be prompted to browse for the missing components or supress the missing components.
If there have been changes to the referenced components and the user chooses to continue loading the drawing in Detailing Mode, the changes to the referenced components will not propagate to the drawing. The drawing will be loaded as it was last saved.
When there is an indication that the drawing needs updating, the drawings Feature Manager will indicate the drawing needs to be rebuilt.
The affected drawing views will display with a hashed border.
Right-clicking on the drawing will give the option Resolve Drawing. Resolving the drawing will load the reference components and update the drawing. The option to resolve the drawing is also available from most tabs of the Command Manager.
The user can also choose to update an individual sheet or view by right-clicking on the sheet or view. This can be done from the drawing area or Feature Manager. Updating individual sheets or views can reduce load times, compared to loading all sheets and views.
I would like to have the option to unload the referenced components and switch back to Detailing Mode without having to reopen the drawing, similar to how hidden components can be unloaded in an assembly. Perhaps this will be available in a future release.
Once opened in Detailing Mode, there are many operations that can be completed in a drawing. The caveat is that these operations do not require loading the referenced components. These include adding Annotations such as Model Items (i.e. dimensions), Auto Balloon, Hole Callout, Center Marks, Center Lines, Area Hatch and Revision Symbols.
While Tables are available, BOMs and most other tables are not. Only the General Table and Revision Table can be added in Detailing Mode.
Like an eDrawing, the drawing can be marked up. Unlike an eDrawing, the Measure tool is not available.
Additional Drawing Views can not be added in Detailing Mode from the View Palette, but views can be copied and pasted. This includes copying and pasting between sheets. Sheets can also be added to a drawing while in Detailing Mode.
While most drawing views cannot be added from Insert > Drawing View, I do like that Empty views can be added.
This allows a user to define the position and Properties of drawing views before loading a large assembly.
I would like to have the ability to add Detail views, as can be done in Detached Drawings. I suspect that this will possible in a future release of SOLIDWORKS.
Dimensions can be added using the Smart Dimension tool, but DimXpert annotations can’t be loaded. Hopefully in a future release, SOLIDWORKS drawings in Detailing Mode will be able to load DimXpert annotations. That being said, a drawing can be loaded in Resolved Mode, the DimXpert annotations added, then the drawing saved and reopened in Detailing Mode for further detailing.
Model dimensions that were added in Resolved Mode, however, cannot be edited other than repositioning them or deleting them.
As with a Resolved drawings, notes can be attached to a view or sheet. The note can be linked to a Property but not to Model properties.
If changes are required to the title block or drawing border, the sheet format can be edited. As with other notes, notes in the sheet format cannot be linked to Model properties.
Below is a full list of what can be done in Detailing Mode as listed in the What’s New SOLIDWORKS 2020 guide, including the ones already covered in this article:
- Notes, including notes with leaders
- Weld callouts
- Linear and circular note patterns
- Geometric tolerances
- Surface finish symbols
- Datum feature symbols
- Datum target symbols
- Revision symbols
- Revision clouds
- Radial and linear dimensions, including use of the Smart Dimension tool
- Locations labels
- Ordinate dimensions
- Magnetic lines
- Angular running dimensions
- Change the position, rotation, and labels of drawing views.
- Copy or cut drawing views and paste them onto the same or other sheets within the same drawing.
- Within annotations, add links to the displayed values of dimensions and other linkable annotations.
- Insert sketch blocks.
- Add general and revision tables. You cannot add other table types.
- Select displayed geometry, such as model edges and sketches. Use Select Other to find other selectable items. You cannot select model faces in any drawing views.
- Save the file as a PDF/DXF file, or print as a PDF.
The limitations when working in Detailing Mode, as listed in the What’s New SOLIDWORKS 2020 guide, are:
- You cannot create new drawing views.
- You cannot create center lines, center marks or hatching.
- You cannot use the Undo tool.
- Draft quality section views cannot be selected or exported to DXF/DWG.
- Detailing mode is not available for detached drawings.
The limitation of not being able to perform an Undo is hopefully something that will be changed soon.
In regard to Detached Drawings, as noted, Detailing mode is not available for Detached Drawings. When a Detached Drawing is selected in the Open dialogue box, there is no option to load the drawing in Detailing Mode.
While in Detailing mode, a drawing cannot be saved as a Detached Drawing. This should not be a problem as Detailing Mode and Detached Drawings basically do the same thing. I do hope, though, that SOLIDWORKS does port some of the functionality from Detached Drawings, such as the ability to create Detail views.
In summary, drawings do not need to be saved in Detailing Mode, as is the case of Detached Drawings. Like Detached Drawings, Detailing Mode can offer improved performance while detailing drawings of large assemblies. Like both Detached Drawings and eDrawings, Detached Mode allows drawings to be shared without having toinclude the referenced components.
While there are a few more things that I would like to see in Detailing Mode, this new functionality in SOLIDWORKS 2020 shows great promise. I look forward to seeing Detailing Mode evolve.
About the Author
Joe Medeiros is a senior applications engineer at Javelin Technologies, a premier SOLIDWORKS reseller servicing customers throughout Canada, and offers SOLIDWORKS customers expertise in implementing and using SOLIDWORKS solutions.
He has been involved in many aspects of the SOLIDWORKS product family since 1996. As an award-winning blogger, he regularly writes about SOLIDWORKS solutions.