If you work on a drawings of large assemblies you know it can be frustrating at times due to reduced performance. Those drawings contain several drawing sheets and each sheet contains several views of all types. Not to mention all the dimensions, notes, tables and annotations each view and sheet contains. The data for just the drawing alone becomes rather large over time and add to the drawing data the assembly model data making the total amount of data for both the drawing and assembly quite large thus reducing overall performance.
Opening a large assembly drawing and loading all that data in memory takes time especially if you open the drawing from a remote server as opposed to locally. If you are opening from a remote server then you should look into SOLIDWORKS PDM Standard or Professional which helps manage your parts, drawings and assemblies but also delivers those file to you to open and work locally.
SOLIDWORKS Product Management and Software Development staff are always looking for ways to improve performance and reliability. To address opening large assembly drawings Detailing Mode was introduced in SOLIDWORKS 2020. Detailing Mode replaces Detached Drawings. I spoke with Nikhil Kulkari, SOLIDWORKS Drawings & MBD Applications Manager Director, about Detailing Mode and how it came to be. Nikhil came up with the idea after visiting a customer that explained to him how he had to wait 30 minutes for a drawing to open in order to make a few minor edits. Nikhil thought there had to be a way to overcome this unproductive use of time waiting for the drawing to open. He thought about Detached Drawings and how they don’t require the assembly or part model to be loaded in memory thus improving performance. But, Detached Drawings isn’t the answer because you have to save as a detached drawing which is slow for large models and then you end up with 2 drawing files containing the same information which undesirable for PDM. Nikhil worked on some prototypes and came up with a method to have the drawing standalone without the need for the part or assembly model data available to perform a variety of detailing functions.
Now you’re wondering; “How’d Nikhil do that?” And your next thought is “Will I have to buy another computer to take advantage of this new found performance?” First, the good news; the answer is no you don’t have to buy a new computer. So, how does Detailing Mode work? The short answer is Detailing Mode uses precise views using twice the precision of a normal drawing view. The view data is stored in the drawing file which contributes to a file size increase but certainly worth the overhead because of the increase in performance. Other information such as hole callout information and silhouette edges are stored in the drawing file. Working behind the scenes is Robust Referencing which saves you a dramatic amount of time by eliminating the need to resolve and save to maintain final annotation and dimension associativity and avoid dangling dimensions and annotations. Robust Referencing allows you to add dimensions and callouts in Detailing Mode and when you open the drawing fully resolved those dimensions are attached to the model geometry. For instance you add a hole callout in Detailing Mode and you save and close the drawing. In the meantime the hole size changes. The next time the drawing is opened the hole callout will update to reflect the new hole size. All the benefits of associativity are maintained using Detailing Mode. Inserting Model Items is a limitation, naturally, because the model data is not loaded. Automation is better with Detailing Mode. For instance in View Only Mode you can only save as a TIF file. In Detailing Mode you can save as a pdf, tif, dxf/dwg or print the drawing making it faster than opening the drawing any other way.
In a side by side comparison opening this 2021 drawing fully resolved takes 1 minute and 30 seconds. Not bad. Using Detailing Mode it took a few seconds.
Here’s what you can do in Detailing Mode:
You must save the drawing in SOLIDWORKS 2021 before you can add or edit break, crop, or detail views to it in Detailing Mode.
- Create Dimensions and Annotations
o Exception: You cannot create dimensions or annotations that require model information such as, cosmetic threads, or links to model properties.
o You can save your changes to the existing drawing file without exiting Detailing mode. Saving in Detailing mode does not require a special save format.
• If you save the drawing in Detailing mode, and then close it and reopen it, you can continue to edit the items you created in Detailing mode.
• If you save the drawing in Resolved mode, the dimensions and annotations you created in Detailing mode are resolved and saved. Then if you close the drawing and reopen it in Detailing mode, the ability to edit the resolved dimensions and annotations is limited. You can only change their position or delete them.
- Capabilities Available in Detailing Mode
o You can create the following dimensions and annotations:
• Notes, including notes with leaders
• Weld callouts
• Linear and circular note patterns
• Geometric tolerances
• Surface finish symbols
• Datum feature symbols
• Revision symbols
• Datum target symbols
• Radial and linear dimensions, including use of the Smart Dimension tool
• Revision clouds
• Locations labels
• Ordinate dimensions
• Magnetic lines
• Angular running dimensions
o In addition, you can do the following:
• 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.
o You cannot create new drawing views.
o You cannot create centerlines, center marks, or hatching.
o You cannot use the Undo tool.
o Draft quality section views cannot be selected or exported to DXF/DWG.
o Detailing mode is not available for detached drawings.
- Break, Crop, and Detail Views in Detailing Mode
o In Detailing Mode, you can create and modify break, crop, and detail views. You can also add dimensions and annotations to the views.
- Hole Callouts in Detailing Mode
o In Detailing Mode, you can add and edit hole callouts for holes that use Hole Wizard, Advanced Hole, Hole, Extruded Cut, Swept Cut, and Revolved Cut features.
- Editing Existing Dimensions and Annotations in Detailing Mode
o In Detailing Mode, for existing dimensions and annotations created in resolved mode, you can edit additional characteristics. You can do the following:
• Edit dimension tolerance values
• Edit dimension characteristics such as line type and arrow type
• Add and remove dimensions in sets of chain and baseline dimensions
• Edit annotation note characteristics and content
As you can see Detailing Mode allows you to perform a majority of the detailing functions without the need for the model to be loaded in memory. Give it a try I’m sure you’ll be impressed or check out what else is new in SOLIDWORKS 2021 by clicking here.