| Rev # | Date | Description |
|---|---|---|
| 1.0 | May 2023 | New document |
Note
All SolidPractices are written as guidelines. The recommendation is to use these documents only after properly evaluating your requirements. Distribution of this document is limited to Dassault Systèmes SolidWorks employees, VARs and customers that are on active subscription. This document may not be posted on blogs or any internal or external forums without prior written authorization from Dassault Systèmes SolidWorks Corporation.
This document was updated using version SOLIDWORKS 2023 SP0.1 and 3DEXPERIENCE R2023x GA. If you have questions or need assistance in understanding the content, please get in touch with your designated reseller.
Acknowledgements
This document was authored by TriMech Solutions and reviewed by Dassault Systèmes SolidWorks Corporation.
Preface
This SolidPractices document contains recommendations for both CAD administrators and drafters related to organizing and managing the CAD environment, tools and techniques for maximizing efficiency when working with SOLIDWORKS drawings.
Because drawings link parametrically to 3D models, the drawing performance depends greatly on the optimization of those models. Many of the slowdowns that drafters report relate to the models, system settings or document properties. The Efficient Modeling SolidPractices document covers these topics and is a supplement to this document.
When developing a new product, self-taught SOLIDWORKS users who have not optimized their drafting environment estimate that they dedicate 50% of their time to creating part and assembly models and the other 50% of their time detailing those models in drawings.
Users with full training who have optimized the drafting environment can take full advantage of the parametric and associative nature of SOLIDWORKS. This enables them to use less than 10% of their time working on drawings.
The goal of this document is to help users unlock the 40% gap in productivity.
Figure 2
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Structure of a Drawing Document
There are many types of elements that relate to drawings. Therefore, to better understand the structure of a SOLIDWORKS drawing, consider the schematic in Figure 3.
The drawing file is the main container of information. When you start a new drawing from a drawing template, the new drawing inherits all the information shown in Figure 3from the drawing template automatically.
You can imagine the drawing sheet and the sheet format as two transparent layers that can contain information independent from each other. It is possible to update elements from both automatically using information that saves in sheet format templates.
Upgrade Old Templates to Maximize Efficiency
It is true that once a company creates its templates and trains its associates how to use them, almost no other effort is required to maintain these templates for a long time. Many companies established their environment 10 to 20 years ago and they still use their original templates.
To maximize user efficiency, stay up to date with the relevant enhancements that each new version of the software introduces.
Parametric Drawing Zones
For example, if your company is using drawing templates created before SOLIDWORKS 2015, you might not benefit from one of the most useful tools for parametrically labeling drawing entities by their location. In other words, drawings created from these templates do not have well-defined parametric drawing zones.
If the border on your drawing contains no zones, like the border in Figure 4, refer to section 3)b).
In cases where your border has zone information, confirm that the setup is accurate. For example, the drawing in Figure 5has zones around the border, but they produce incorrect location labels, which introduce the potential for costly production errors if a user attempts to insert such parametric labels.
To confirm that the drawing zone of your template is properly established, start a new empty drawing and add a note containing the zone information anywhere on the sheet. For example, see Figure 6.
Move the note around the sheet and observe how the zone label updates. Does it synchronize with the zones on the border? If it is not, you have two options:
Keep your existing border and adjust the zone parameters in the sheet properties to match the information on the border. See Figure 7.
Use the Automatic Border tool to recreate the border.
Automatic Border Tool
While the previous solution can save you time when editing the sheet format template, the recommendation is to use the
Automatic Border
tool to recreate the border.To determine if your sheet format has an intelligent border, expand the Sheet1 node in the FeatureManager® design tree. If the Sheet Format folder does not list a Border in the contents (Figure 8), you are using an inefficient drawing template.
To replace your old border with a parametric border, follow these steps:
Adjust the document properties for the border according to your company standards (Figure 9).
Edit the sheet format.
Figure 10
On the Sheet Format tab, click
Automatic Border
.
Optionally, select all entities from the old border (lines and notes) that you want to delete. As an alternative, you can postpone this step until you create the new border, allowing you to match the results.
Figure 12 – The result of deleting the old lines and notes
In the
Automatic Border
PropertyManager, click the) arrow.
Define the border according to your company standards. In the Figure 13, the old border still appears. This makes it possible to compare the result of customizing the new border by superimposing it over the old border. After defining the new border, use the
) arrow to return to the previous page and delete the old border per Figure 12.
Figure 13 - New border preview in orange superimposed over the old border
Click
Figure 14
Title Block
Because the title block does not offer the same degree of automation as the border, if the old template has a title block, you may be able to use that template with minimal modifications.
A good introduction about how to create and customize title blocks is available in the self-guided video lesson Sheet Formats and Templates on my.solidworks.com. Be aware that you need to log in with your 3DEXPERIENCE ID to access this lesson.
Depending on the specifics of your company, you might use some or all of the following steps:
Edit the sheet format.
Create the border. See section 3b.
Draw sketch lines to define the title block and use relations and dimensions to constrain them.
Hide all dimensions that relate to these lines:
Select one dimension.
Press Ctrl +A to select all dimensions.
Right-click the selection.
Select Hide.
Optionally, you may use Insert > Picture to insert a company logo. Resize and relocate the logo as required.
Add notes and link them to custom properties as required. For more information about how to do this, see section 4.
Optionally, you may use the Title Block Fields command to select a number of notes as title block fields. After selecting these notes, you can edit them directly from the sheet focus. You do not need to edit the sheet format to access the notes.
Table Anchors
In the sheet format, you can define thedefault anchor locationsfor several types of tables:
| General Table Anchor | Revision Table Anchor | ||
|---|---|---|---|
| Bill of Materials Anchor | Weld Table Anchor | ||
| Hole Table Anchor | Bend Table Anchor | ||
| Weldment Cut List Anchor | Punch Table Anchor |
Use of Custom Properties in Drawings
When working with drawings, custom properties are essential for maximizing efficiency. The optimal usage follows the “Single Source of Truth” principle. In other words, enter the value for a custom property once, in one place, and refer to it anywhere else.
This document uses the term custom properties to refer to all metadata within each SOLIDWORKS file, including the configuration properties. This is important to know because in 3DEXPERIENCE SOLIDWORKS, all properties are configuration properties.
There are multiple ways to create custom properties and modify the property values, including but not limited to:
SOLIDWORKS PDM data cards – This is the method that SOLIDWORKS PDM users prefer.
PLM attributes – This is the method that 3DEXPERIENCE users prefer.
Property tabs – This is the method that non-PDM users prefer.
Title block fields
Design tables
To determine at what level to locate a custom property, consider the associativity between parts and assemblies of various levels and drawings.
It is possible to link to custom properties that exist in other files if those files are lower in the file reference chain, not higher.
In drawings, you can extract the values of custom properties from multiple entities like:
Notes
Tables
Balloons
Labels
Custom Properties in Notes
You can use theLink to Propertyfunction in the Note PropertyManager to parametrically include custom properties in notes.
You can extract the property value from:
Current document (drawing)
Model referred by the current drawing view
Model referred by the drawing view specified in the sheet properties
Selected components
Component to which the annotation is attached
For example, the note in Figure 21 includes the Description property value of the component to which the note is attached.
Custom Properties in the Bill of Materials
You can select any property from any component of the assembly as a column header.
You can also use the values of custom properties in BOM formulas, including as decision criteria.
In the column E of Figure 23, if the value of the property Source is MANUFACTURED (case sensitive), then the cell links to the value of the property Material, otherwise the value of the property is Vendor.
Custom Properties in Balloons
Balloons can refer custom properties. Figure 24 depicts a good example of using an efficient process to quickly document the sourcing of the assembly components. In this case, the Auto Balloon tool was used to populate all the notes with the Source property values attached to each component.
Table Templates
To save time and foster consistency within your team, customize templates and save them in a shared templates location for frequently used tables. SOLIDWORKS allows saving templates for the following types of tables:
| Table | File Name Extension |
|---|---|
| General Table | .sldtbt |
| Bend Table | .sldbndtbt |
| Bill of Materials | .sldbomtbt |
| Hole Table | .sldholtbt |
| Punch Table | .sldpuntbt |
| Revision Table | .sldrevtbt |
| Weldment Cut List | .sldwldtbt |
| Weld Table | .sldwldtbt |
| Title Block Table | .sldtbt |
To create and save a table template, follow these steps:
Create and customize a table according to your company standards.
Right-click anywhere in the table and select Save As.
Select Template as the file type then browse to the shared folder and save the file.
When users insert a new table, they typically click the Open table template icon to browse to the location of the template that they want to use.
Use Batch Processing Tools for Repetitive Tasks
One of the most wasteful ways to use a drafters time is to ask them to perform repetitive clerical tasks. This usually happens at the beginning or end of a project. For example:
After duplicating all the files of an existing job to use to start a new job, open each drawing and change the sheet format in all sheets.
Print all drawings during the release process.
Save all drawings in the PDF format.
Save all drawings for sheet metal parts in the DXF format.
Fortunately, you can perform such tasks efficiently using batch processing programs such as the SOLIDWORKS Task Scheduler.
Starting SOLIDWORKS Task Scheduler for SOLIDWORKS Desktop
If you have a SOLIDWORKS 3D CAD installation (the traditional desktop version), you can run the SOLIDWORKS Task Scheduler directly from a Windows® Search (Figure 28).
Starting Task Scheduler for 3DEXPERIENCE SOLIDWORKS
If you are using 3DEXPERIENCE SOLIDWORKS, start the SOLIDWORKS application first. The Task Scheduler is available from the Tools > SOLIDWORKS Applications menu (Figure 29).
Example: Saving all Drawings from a Folder in PDF Format
To save all drawing files from one or more folders, follow these steps:
Start an Export Files task.
Select the Adobe Portable Document Format (*.pdf) file type.
Click Options and then adjust the export settings.
Specify the start time and then click Finish.
Other Batch Processing Programs
Task Scheduler has acceptable functionality. However, if you want capabilities beyond those that SOLIDWORKS Task Scheduler offers, look for a batch processor that could also:
Open drawings in detailing mode for export purposes. For example, you could print or save hundreds of large drawings to the PDF format in minutes instead of hours or days, if you open drawings in this mode.
Automatically extract file references. For example, you could select a top-level assembly and have the software collect a list of drawings for all the assembly components to print or save to the PDF format.
Run multiple tasks sequentially.
Process restarts in case of errors.
Force SOLIDWORKS to restart after processing a specific number of files.
Automatically:
Run tasks as a specified user or as the active user. For more information, see the Knowledge Base article QA00000113316.
Check out files that require updates from the PDM vault before processing.
Process the files.
Check files back in to the PDM vault and add a comment on your behalf if the file is checked out during the process.
Running PDM Tasks Triggered by Workflows
In SOLIDWORKS PDM Professional, you can use PDM Tasks to automatically run tasks like saving drawings to PDF or DXF after file approval. In addition, it is possible to distribute the running such tasks on multiple workstations, which can significantly reduce the time required for completion.
Be aware that SOLIDWORKS PDM Standard has limited functionality, being able to only save files to PDF.
The recommendation is that you consult your Value Added Reseller (VAR) to ensure that the implementation of such tasks maximizes the efficiency of your team.
Drawing Opening Modes (Match the Task with the Mode)
When users complain that a certain drawing is large or slow, they usually refer to these three major symptoms:
Long opening time
Lag when performing various tasks after the opening a drawing
Long saving times
For existing drawings, you can greatly mitigate such symptoms by asking a critical question:
Why do I need to open this drawing?
The answer to this question allows you to match any task with the most efficient mode of opening a drawing.
| Task | Fastest Opening Mode | Assembly Opens in Background | Requires Saving Model Data in the File |
|---|---|---|---|
| Review the Drawing | Detailing | No | Yes |
| Selective Sheet Loading | Detailing | No | Yes |
| Detailing | No | Yes | |
| Save to PDF | Detailing | No | Yes |
| Add/ Edit/ Delete Annotations | Detailing | No | Yes |
| Delete Tables | Detailing | No | Yes |
| Add/ Edit/ Delete Revisions | Detailing | No | Yes |
| Add/ Move / Rename/ Delete Sheets | Detailing | No | Yes |
| Move/ Delete/ Hide/ Show Drawing Views | Detailing | No | Yes |
| Add Detail Views | Detailing | No | Yes |
| Break Views Existing Views | Detailing | No | Yes |
| Add Saved Standard Views | Detailing | No | Yes |
| Add/ Edit/ Delete Markups | Detailing | No | Yes |
| Any other tasks | Lightweight or Resolved | Yes | No |
There is a simple fact that explains the recommendations in Table 3; “A drawing opens faster if the minimal amount of data is loaded in the RAM.”
Most users open drawings by double-clicking the file name in Windows File Explorer or from the SOLIDWORKS PDM add-in. That action causes a drawing to open in either Lightweight mode or Resolved mode, depending on the system options. Both of the modes require that the assembly first opens in the RAM.
As shown in Figure 33, opening the assembly starts multiple computation phases. All of these phases are time consuming.
For most tasks in Table 3, the information required already exists in the drawing. For example, if the drawing is in a released state, opening its assembly is even counterproductive because it can potentially trigger an update of the drawing views.
The following sections examine each of the opening modes.
Detailing Mode
If the Save model data option is active in the Document Properties >
Performance
options (Figure 34), more information saves in the drawing file for each drawing entity. This allows the drawing to open for detailing operations without loading the model into RAM.
Figure 34
The only file that is required for working in this mode is the drawing file. This opens interesting opportunities for collaboration with third-party associates.
Functionality
When a drawing opens in Detailing mode, the operational speed is optimal. There is no lag when switching sheets, zooming in or out or when panning or selecting entities.
An impressive number of tools are available to:
Edit file properties
Edit document properties including the drafting standard
Add, edit or delete layers
Add, move or delete sheets
Edit sheet properties including the sheet format
Add standard views from the View Palette (if they were saved in the drawing file)
Add detail views of existing views
Break or crop existing views
Add empty views
Provide access to most detailing tools. As the software evolves, more tools become available. It is a recommendation to review the tools that become available with each new release.
AddHoletables andRevisiontables
Add, edit or delete markups
Use the Design Checker to ensure that a drawing complies with the company standards.
Example of a collaboration scenario using the Detailing mode
Imagine that a company contracts the detailing of its drawings to a third-party provider. They follow this process:
An employee of the company creates a new drawing that contains only the model, BOM and the projected and section views required to start the drafting process. The drawing contains no additional dimensions or notes.
The employee shares the drawing with a contractor.
The contractor opens the drawing in Detailing mode and adds:
Detail views
Break views
Crop views
Dimensions
Notes
Balloons
The contractor sends the completed drawing back to the company employee.
The company employee opens the drawing in Resolved mode and then rebuilds and saves the model.
The job is complete.
Advantages:
The company transfers a minimal amount of data, limiting the exposure of sensitive intellectual property to the third-party provider.
Minimizes the time required for the contractor to open, edit and save files.
Use cases
There are multiple use cases for opening a drawing in Detailing mode (Table 3). To perform them, you can use the following techniques:
Switch sheets: Select the sheet tabs at the bottom of the SOLIDWORKS window. Because the amount of data that loads in RAM is minimal and there is nothing to compute, the shift from one sheet to the next happens immediately.
Zoom and pan inside a sheet: Viewport manipulations are very fast (more than 60 frames per second). There is no lag in operation.
Print: If the drawing is in an approved state (read-only), opening it in Detailing mode is the best way to ensure that what prints corresponds to what was approved.
Read and edit file properties: Only the properties of the current file are accessible in this mode. You cannot access the properties of the referred models because the model does not load.
Controlling Drawing Updates in Lightweight or Resolved Modes
When a drawing opens in Lightweight or Resolved mode, the models referred by the drawing loaded into the RAM. When SOLIDWORKS recognizes that one of the models was modified, the program may perform an update of the drawing. This can be a time-consuming operation with drawings of complex models.
To maximize drafting efficiency, it is critical to control the updating of drawing views.
Updates During the Drawing Load Phase
To avoid an automatic update when opening a drawing, clear the check box for the Allow auto-update when opening drawings option in System Options > Drawings >
Performance
.With this option inactive, if there is a modification to the model, you receive a warning. To postpone the update, click No.
After the drawing loads, sheets and drawing views that are out-of-date are highlighted in the FeatureManager design tree, on the status bar and in the graphics area.
At this point, you can decide which drawing views or sheets require an immediate update.
Updating all views from a sheet
To update individual sheets, right-click the sheet and select Update Sheet.
In the example shown in Figure 43, the user postponed the upgrade of the Sections sheet because of work being performed on the current sheet.
Updating individual drawing views
To update one or more drawing views, preselect the views and click the Update View command. In this way, you can postpone unnecessary updates and save time.
Updates After Editing a Model
Sometimes, a simple roundtrip between the drawing view and the model can generate a drawing update. To prevent automatic updates from happening, turn off the Automatic view update option for the active document. While this option is a document setting, it appears in the FeatureManager design tree and not in the settings area. To turn this option off, clear the check box as shown Figure 45.
Control Updates of Individual Views
Some drawing views take more time to update than others. You can use the Performance Evaluation tool to generate a report that contains the rebuild times for both sheet and drawing view levels.
For example, in Figure 46, Section View H-H takes the most time to update. You can exclude this view from automatic updates by activating the Exclude from automatic update option in the PropertyManager of the view.
Excluding complex views from automatic updates allows you to work efficiently when making frequent modifications to assemblies and drawings.
The good news is that saving the drawing triggers the update of all views. Therefore, the drawing is up to date after saving.
View Palette and its Potential Impact on Update Time
If a drawing refers to a complex model with many saved orientation views, rebuilding the
View Palette
can increase the opening and update times significantly.To troubleshoot this problem, use the Performance Evaluation tool and review the Rebuild View Palette time. If the time for this task is not acceptable, deactivate the automatic rebuild of the View Palette.
Types of Drawing Views - Impact on Performance
To study the impact of the drawing view type on performance, the following experiment was performed.
Selected an assembly that contain over 10,000 components.
Ensured that the assembly is not fully rebuilt.
Ensured that the assembly file was set to read-only to trigger the update of the drawing on opening.
Created several drawings containing:
Primary views (model and projected)
Secondary views (section, detail)
Tertiary views (crop)
Opened the drawings in Resolved mode and measured:
Open Time
Update Time
The results are reported in Table 4.
| Views | Model | Projected | Section | Detail | Crop | Open Times | Update Times | Graphics Display Times |
|---|---|---|---|---|---|---|---|---|
| 5 | 5 | 0 | 0 | 0 | 0 | 29.7 | 0.2 | 19.6 |
| 5 | 1 | 4 | 0 | 0 | 0 | 30.1 | 0.3 | 19.6 |
| 11 | 5 | 0 | 0 | 5 | 1 | 39.4 | 0.5 | 25.9 |
| 9 | 1 | 4 | 4 | 0 | 0 | 126.3 | 47.4 | 39.1 |
| 13 | 1 | 4 | 4 | 4 | 0 | 145.1 | 47.7 | 50.5 |
Conclusions:
The Model, Projected, Detail and Crop views have the least impact on performance.
Section views have a major impact on performance.
Good to know:
The Detailed and Crop views are fast because they require a simple generation process:
Copy the parent view.
Scale the copy (if required).
Mask the area outside the sketched shape defining the detail or crop view.
The Section and Broken-out Section view are slow because they require a complex generation process:
Create a configuration of the model referenced in the parent view.
Perform a physical extrude-cut through the new configuration using the sketch line.
Display the resulting model on the drawing.
In addition, data for the new model configuration that corresponds to each section view saves to the drawing file. This increases the file size significantly.
Configurations versus Display States - Impact on Drawing Performance
As discussed in section 5i of the SolidPractices document: Best Practices for Managing Large Assemblies and Drawings, overusing the configurations affects the performance of large assemblies. In cases where the geometry and properties do not change, the recommendation is to use display states instead.
These recommendations are especially relevant when representing such assemblies in drawings. The performance impact on a drawing is magnified by the number of configurations referred in its various drawing views. Take a moment to revisit the drawing opening and rebuilding process in Figure 33 – Update all Configurations of the Assembly Referenced by the Drawing.
Consider a case where a user wants to document the assembly process by creating a configuration for each step of the process. See Figure 49.
There are 15 total steps. Consider the consequences.
Consequences of Working in the Assembly Environment
Each of the 15 configurations generates separate assemblies. At this time, the user needs to decide whether to save the body data for each configuration or not. Table 5 describes the consequences of this decision.
| Configuration Data | Pros | Cons |
|---|---|---|
| Saved | Quick switch between configurations | Larger File Size |
| Not Saved | Smaller File Size | Assembly needs to be rebuilt when switching configurations |
A higher-level assembly that requires two or more configurations of a subassembly corresponds to the number of body data sets that update and load into RAM.
Consequences of Working in the Drawing Environment
At the drawing level, the potential problems of using configurations increase by an order of magnitude.
For example, if the configuration data of the nonactive configuration is not saved in the assembly file, the following processes must occur when the drawing opens:
Rebuild 14 of the 15 configurations required by the drawing views in Figure 49. The active configuration always saves in the assembly file.
At this time, 15 assemblies load simultaneously into RAM.
Because 14 configurations rebuild during the loading phase, the application updates the 14 drawing views.
In practice, such a drawing would open many times slower than the drawing of an assembly that captures the same information using the display states of a unique configuration. In this case, only one assembly would open in RAM. This would require no configuration rebuild and no drawing view update.
The following procedure was performed as a test:
Select an assembly with more than 10,000 components.
Add 5 configurations and 5 display states.
Create 3 drawings, each containing 5 drawing views:
The first drawing uses the same configuration and display state in all drawing views. This is the baseline.
The second drawing uses a different configuration for each drawing view.
The third drawing uses a different display state for each drawing view.
Open each drawing and use the Performance Evaluation tool to report the times recorded in Table 6.
Configurations | Display States | Open Time | Drawing Views Update Times | Graphics Display Times |
|---|---|---|---|---|
| 1 | 1 | 25.2 | 0.3 | 15.6 |
| 1 | 5 | 24.8 | 2.5 | 22.2 |
| 5 | 1 | 69.9 | 0.3 | 21.5 |
These findings confirm the recommendations to minimize the use of configurations in drawings.
Diagnostic Tools
When you analyze existing drawings to determine if the overuse of configurations might be affecting performance, take advantage of the following diagnostic tools.
Drawing Open Progress indicator
When a drawing opens, each individual set of configuration data that loads into the RAM appears as a Group in the Drawing Open Progress indicator.
For example, if you know that the drawing for Figure 50 refers only one assembly file, it means that at least 30 drawing views show either a different configuration or a section view. As mentioned in section 10), each section view generates a supplementary configuration in the RAM.
Performance Evaluation tool
The Evaluate > Performance Evaluation tool in a drawing has two areas that could show (Figure 51):
Assembly Performance: Displays the number of assembly loads into RAM.
Different Configurations: Displays drawing views that refer to different model configurations.
Hiding Reference Drawing Views to Improve Performance
When placing drawing views outside the border to use only as reference for creating secondary views, the recommendation is to hide them, which reduces the Graphics Display Time value in the Performance Evaluation tool.
In the examples shown in Figure 52 and Figure 53, hiding the two reference views decreases the graphics display time by 20%. The time savings vary with the number and complexity of the hidden views.
Mirror Existing Drawing Views
If your company procedures permit, in situations where you need to create 2D drawings for pairs of symmetrical products (left and right hand) from only one 3D model, you can use the Mirror drawing view options to save time.
In Figure 54, the only views that require mirroring are the independent views: two Model views and one Relative to Model view.
As shown in Figure 55, all derived views are mirrored automatically according to the options specified for the parent view.
Views represented with the Shaded or
Shaded With Edges
display styles cannot be mirrored.Draft Quality versus High Quality Views
You can specify the display style for drawing views as
Draft quality
orHigh quality
.A bit of history:
When the first versions of SOLIDWORKS became available, the most advanced CPUs available had no more than two cores. Converting 3D model edges into drawing lines require complex computations, therefore, it was critical to save time processing the lines to a state that is “good enough” to allow the user to start detailing the drawing.
Draft Quality Views
The easiest solution involves taking advantage of the fact that the mesh of graphics-triangles that approximate the ideal shape of the model was already computed in the part or assembly model. Extracting the drawing lines from that mesh is a relatively fast operation that creates Draft quality drawing views.
The quality of the drawing lines in such views is not ideal. Saving time in processing such views comes with consequences such as:
Dimensions are approximate.
Requires a large amount of data, which results in larger file sizes and longer saving times.
When printing or saving the drawing to the PDF format, the output has a “raster” quality (Figure 58).
Saving to the DXF format can generate missing or incorrect data.
The processing of such views occurs sequentially.
Draft quality
drawing viewHigh Quality Views
With advancements in CPU design, more cores became available to the SOLIDWORKS users. This allows for extracting more precise drawing lines from the mathematical representation of the model shape (body data) by dedicating a separate core for each drawing view, and therefore allowing multicore processing.
With modern hardware, there is no longer any benefit to defining views as Draft quality.
On the basis of running tests, drawings that contain
High quality
drawing views:Have smaller file sizes
Open and save faster
Update faster
Generate prints or PDF files with “vector” quality output
Generate correct DXF files
Allow for quick and precise operations in Detailing mode (section 7a)
Figure 59 - "Vector" quality in PDF output of a
High quality
drawing viewSpecial Considerations for Shaded and Shaded with Edges Views
Any display style that includes the word shaded requires the extraction of information from the graphics-triangles mesh. For example, information about the colors of the faces. You can only represent the shaded views, especially those not containing edges, in
Draft quality
mode.Therefore, the recommendation is to use caution when using shaded views. If opening or saving a drawing takes a long time, test to determine if the drawing settings affect performance. To do that, define all drawing views as Hidden Lines Removed and
High quality
and save a copy of the drawing. If the performance improves, it means that the shaded views were causing the slowdown.Efficient Dimensioning
One of the most time-consuming activities when detailing drawings is applying dimensions. Using the same “Single Source of Truth” principle described in section 4, the most efficient drafters avoid duplicating work by taking advantage of the dimensions in the model.
It is true that the dimensions used to define sketches and features in the model might not always be relevant for detailing the manufacturing operations in the model, especially when the modeling technique does not follow the manufacturing process. With that understanding, you can add the Reference and DimXpert dimensions to the model and assign them to Annotation views for importation into the drawing views.
The other major benefit of using such techniques is an increase of efficiency at the team level. Senior designers can add all the dimensions required for detailing and include them in Annotation views or 3D views. This helps ensure that a junior member of the team can use them to quickly create accurate drawings that contain all required dimensions and tolerances.
Annotation Views
Annotation views are useful to collect relevant product and manufacturing information (PMI). PMI includes entities like the dimensions and annotations in a model (part or assembly), and assigns them to a specific orientation.
Creating Annotation views
SOLIDWORKS creates some annotation views automatically, when a user adds dimensions or annotations parallel to a standard drawing view. A user can add others manually and the user can add, remove or move dimensions between existing annotation views.
As a starting point in learning more about using annotation views, you can view the self-paced Annotation Views video training lesson on my.solidworks.com.
After defining annotation views in the model, you can use the views toautomatically populatethe drawing views with PMI.
Updating the PMI on drawings after revising Annotation views
When adding, editing or removing dimensions and annotations from the model annotation views, it is easy to update the corresponding drawing views.
After modifying the annotation views, the first perform a Rebuild of the drawing or Refresh of the view palette runs the Annotation Update command. While this command is active, previously hidden annotations and modified annotations appear as gray in the existing drawing views. Right-click the annotations to display them.
Be aware that you can access hidden dimensions anytime using the Hide/Show Annotations command.
Another way to run the Annotation Update command is by following the two steps from Figure 62:
Click the Sheet tab.
Click the PropertyManager tab.
3D Views
3D views are the best tools to capture multiple settings such as the following and save them under one name:
Orientation
Annotation views
Configuration
Display State
To create 3D views, you must have a license for the SOLIDWORKS MBD application. Be aware that at this time, SOLIDWORKS MBD is not available to users of 3DEXPERIENCE SOLIDWORKS.
After creating a 3D view, the view is accessible to all SOLIDWORKS users, regardless of the type of license.
You can learn more about 3D views on my.solidworks.com.
You can insert 3D views in 2D drawings as drawing views by dragging the views from theView Paletteto the drawing sheet as shown inFigure 64.
Model Items
You can use the Model Items command to perform further customizations when inserting model dimensions and annotations in the drawing views. For maximum efficiency, consider using Annotation views first and
Model Items
second. TheModel Items
functionality includes:Adding dimensions for selected features
Adding annotations that annotation views do not recognize, such as:
Pattern instance counts
Caterpillar
End treatments
Smart Dimensions
Efficient drafters useSmart Dimensionsonly for adding the remaining dimensions that are not easy to capture as model items.
Efficiency and Consistency Enhancing Tools for Dimensioning
When customizing dimensions, speed and consistency are critical. Consider the following tools:
Drafting standards
Drafting standards are the best tools to ensure consistency of the default settings for your team. The standards are easy to customize and you can save them in external files and apply them quickly to modify existing drawings.
Styles
Styles make it possible to capture all settings of an entity, such as dimensions or annotations for:
Reuse in the same drawing
Save in external files to:
Share with team members
Load and apply on other drawings
Ideally, it is best to use styles when dimensions or annotations deviate from the drafting standard.
Dimension Palette
The Dimension Palette is a productivity enhancer that you can incorporate in the “Stay in the Flow” modeling workflow described in section 3 of the Efficient Modeling SolidPractices document.
Simply select one or more dimensions and an expandable button appears next to the cursor. It provides shortcuts to some of the most commonly used dimension properties as well as additional settings for arranging and aligning dimensions.
Tables
The topic of tables in drawings is vast. This document attempts to briefly cover as much as possible. For maximizing efficiency, the best practices for customizing the environment and ensuring a unique source of truth described throughout this document also apply to working with tables.
Use table templates as per your company standards.
As much as possible, use the parametric metadata from the models to populate table cells.
For more information about tables, watch the video lessons available from my.solidworks.com, including:
Bill of Materials
Custom Properties in BOM Tables
General Tables and Hole Tables
Design Library
One of the best ways to eliminate duplicate work and foster consistency in your team is to save the most frequently used drawing elements in adesign library. For example:
Annotation styles
Notes
Blocks
Symbols
An easy way to configure and interact with these libraries is from theDesign Librarytabin theTask Pane.
The Design Library provides a central location for reusable elements including annotations. In Figure 68, the gray
Design Library
folder is located on the local computer or on the network. The blue Annotations folder is a 3DEXPERIENCE bookmark.Design Library | Subfolders populated by SOLIDWORKS with reusable items such as parts, blocks and annotations. You can add folders and content. | |
|---|---|---|
Connected Design Library(3DEXPERIENCE users only) | Provides access to content from the 3DEXPERIENCE platform by means of the Task Pane. For more information, see Connected Design Libraries. |
To add bookmarks in the Design Library, use theSystem Optionsshown in Figure 69.
Conclusion
SOLIDWORKS offers a huge number of options, tools and techniques for creating, editing and viewing 2D drawings. For most companies, creating and documenting efficient drafting procedures requires a lot of research and discipline.
It is hoped that the information in this document can help reduce the amount of time that you need to develop and adopt procedures to maximize your drafting efficiency.
We hope that you find this document informational and useful and request that you leave a brief feedback about the topics that you want us to cover in the next revision of this document. Click here for a complete list of SolidPractices documents available from DS SOLIDWORKS Corp.
