Crossing the Chasm: 3-D Model Based Definition in SolidWorks
While there is compelling evidence suggesting that commercial enterprises can benefit from implementing and reusing 3-D model based drafting practices, transitioning away from 2-D drawings isn't like flipping a switch; it takes careful planning and, often, reconsideration of fundamental 3-D CAD modeling practices. This article will demonstrate how apply 3-D MBD practices within SolidWorks 2013.
3-D MBD in SolidWorks 2013
SolidWorks has a suite of tools that enable design engineers and modelers to add 3-D dimensions, tolerances and other annotations within the 3-D environment. Once these annotations have been created, they can be reused in associative 3-D PDF TDP documents, eDrawings, or in traditional 2-D drawings. But before diving deeply into how to use these tools, it is valuable to understand a few fundamental MBD concepts.
The most important concept to consider is how the various classes of model-based information are organized (or can be organized) within the context of a SolidWorks part or assembly file. As with 2-D drawings, which feature a collection of model views and view-specific annotations, the primary collector for this information is the 3-D view, otherwise known as Annotation Views in SolidWorks.
It is also important to realize that annotating a model in 3-D is different than doing so in 2-D. In addition to dimensioning and tolerancing and Annotation View organization schemes, consider re-reading ASME Y14.5 and ASME Y14.41. SolidWorks' DimXpert was designed to create 3-D dimensioning and tolerancing schemes that conform to these standards.
Like a drawing view, the Annotation View is an orientation (Front, Top, Left, Right, etc) and a set of annotations that "belong" to that view. In SolidWorks, Annotation Views are the direct replacement for 2-D views that can be created within a drawing. Since the concept of "page" is only relevant for a drawing, consider defining an Annotation View naming scheme to help identify the content within each Annotation View. A well-formulated naming scheme will enable users to distinguish at a glance the relative importance or viewing order of an Annotation View, its orientation, specific features that have been annotated, if it's a section view, and the classification or type of annotation in the view. The US Army developed a view naming convention that encapsulates this information in a short form; here are a couple examples:
- MBD0_TITLE_BLOCK: This is an "MBD" view, which should be viewed first, which contains the title block for the model.
- MBD5D_MOUNT_SLOTS: This is an MBD view, which is the "5Dth" view, which contains annotations for mount slot features.
- MBDA0_TITLE_BLOCK: This is an MBD view for an assembly (the "A" after "MBD"), which should be viewed first, which contains a title block for the model.
Title Blocks, BOMs, and Notes
Title block information and other notes can be presented in a few different ways within SolidWorks. One method is to use the Insert->Tables->Title Block Table...command. Regardless of how the data is presented to the viewer, defining this information as individual Custom Properties or Configuration Specific Properties is considered a best practice. The benefit of defining Custom or Configuration Specific Properties is that these can be defined once in a central location and referenced or presented in many forms.
Some types of information typically found in title blocks or in drawing notes are best represented as a 3-D Note object in SolidWorks. SolidWorks' Custom Properties cannot include flag symbols, GD&T symbols, or common symbols (like Surface Finish) so this type of information is better represented in a leadered or unleadered 3-D note that is assigned to a specific view.
BOM tables are typically featured in assembly drawings, and these same tables can be included within the 3-D SolidWorks environment. As with title blocks, BOM tables can be created by using Insert->Tables->Bill of Materials...
It is not possible to assign title block tables or BOM tables to specific Annotation Views in the current release of SolidWorks. (This will not be the case in an upcoming release). However, these tables can be temporarily hidden so they aren't in the way when annotating the model.
SolidWorks MBD Environment Configuration
To create 3-D MBD effectively in SolidWorks, various system, document, and feature level configuration is required (these settings apply to SolidWorks 2012 and above).
Recommended System Options
- Display dimensions flat to screen: DISABLED
Display notes flat to screen: ENABLED
- Please Note: Setting this option to ENABLED appears to be the best option when working at the assembly level, where balloon notes and other flag notes are common. On the part level, setting this option to DISABLED may be a better choice when using leadered and unleadered note objects.
- Please note: In SolidWorks 2012 and 2013 there is an issue where it is possible to inadvertently pick note objects that do not belong to the currently active view. For this reason, it may be helpful to add note objects "last"—after the creation of other 3-D dimensions, GTOLs, weld symbols, etc.
Hide/Show tree items
- Design Binder: Show
- Annotations: Show
- Tables: Show
- Hide/Show tree items
- View transitions: DISABLED
Recommended Document Options
- Overall drafting standard: ANSI
- Center between extension lines
- Cosmetic threads: DISABLED
- Feature dimensions: DISABLED
- Shaded cosmetic threads: DISABLED
- Display all types: DISABLED
Always display text at same size: ENABLED
- Please note: Please feel free to disable this as necessary, and select the appropriate scaling option. In some cases, disabling this option may provide more predictable behavior of annotation size, but may also require more font size management for individual annotations.
- Display items only in the view in which they are created: DISABLED
- Display assembly annotations: ENABLED
- Use assembly setting for all components: DISABLED
- Hide dangling dimensions and annotations: DISABLED
- Display filter
Geometric Tolerance: ENABLED/DISABLED
- Create basic dimensions (Chain/Baseline)
- Please note: This feature is primarily related to using DimXpert Auto Dimension Scheme and controls what types of dimensions are created when using this feature.
- Please note: enabling or disabling this does not preclude the creation of basic dimensions manually from features that have a position tolerance.
- To create a basic dimension from a feature with a geometric position tolerance, right-click on the position annotation in the DimXpertManager feature tree (when Tree Display is set to "Show annotation based tree") and select "Recreate basic dim" as shown below:
- Geometric Tolerance: ENABLED/DISABLED
Recommended Annotation View Settings
Right click on the Annotations folder in the SolidWorks FeatureManager and select "Details..."
- Configure as required, but be sure that Reference dimensions and DimXpert dimensions are ENABLED
- Please note: As discussed above in the Document options, set Text scale and set Always display text at same size to ENABLED/DISABLED to best meet your requirements
- Display items only in the view in which they are created: DISABLED
- Display annotations: ENABLED
- Please note: when working with assemblies, set Use assembly settings for all components to DISABLED
- Display filter:
Right click on the Annotations folder and configure the right click menu as shown below.
- Display Annotations: ENABLED
- Show Feature Dimensions: ENABLED OR DISABLED per your requirements
- Show Reference Dimensions: ENABLED
- Show DimXpert Annotations: ENABLED
- Automatically Place into Annotation Views: DISABLED
- Enable Annotation View Visibility: ENABLED
Create 3-D Dimensions, Tolerances, and other Annotations
In SolidWorks, 3-D model-based dimensions, tolerances, and other annotations can be created using several different tools and workflows. As mentioned previously, there are two "toolboxes" in SolidWorks for creating 3-D MBD:
- "RefDims" (and other annotation types within the Annotations toolbar)
Regardless of which dimensioning, tolerancing, or annotating tool is used, it is important to note that DimXpert and RefDims (or other annotation types within the Annotations toolbar) can be used together to communicate design intent clearly and effectively. In fact, DimXpert is only a dimensioning and tolerancing tool, and does not provide annotation types for notes, weld symbols, surface properties, etc. To create these types of annotations, use the tools in the Annotations toolbar.
3-D annotations can be created within existing Annotation Views or within Annotation Views that are created "on-the-fly" as the 3-D annotation is created. While both techniques are effective, the preferred method is to place 3-D annotations into Annotation Views that have been created prior to the creation of the annotation, since this provides direct control over placement of the annotation.
Before creating a 3-D dimension, tolerance, or annotation, create an Annotation View with the appropriate orientation. After creating the Annotation View, be sure to select the view and select "Activate and Reorient" from the right-click menu. (If the Annotation View is already "active" the right-click menu will display an "Orient" command).
To enable or disable creation of Annotation Views automatically when adding 3-D dimensions and tolerances:
- In the FeatureManger tab, right-click on the Annotations icon and select "Automatically Place into Annotation Views."
- As mentioned above, the preferred configuration is to disable this feature. However in some scenarios enabling this can be helpful, especially if a feature sketch plane doesn’t align with a standard view.
DimXpert can create 3-D dimensions and tolerances automatically or manually. The DimXpert Auto Dimension Scheme function provides an automated dimensioning and tolerancing solver that can dramatically reduce the time and effort required to dimension a part. While it is possible to click the Auto Dimension Scheme button, and then click OK button (green check sign), the Auto Dimension Scheme feature is far more effective if it is constrained before calculating the resulting solution.
Constraining DimXpert's Auto Dimension Scheme feature can be accomplished in several ways:
In the Settings panel:
- Select Prismatic or Turned depending on the type of model
- Select Plus Minus or Geometric Tolerance type
In the Datum Selection panel:
Designate a Primary Datum by selecting a face, group of faces, or a feature within the model
- Use the Create Compound Plane option in the DimXpert Feature Selector to define a datum plane across multiple coplanar faces
- Designate a Primary Datum by selecting a face, group of faces, or a feature within the model
In the Scope and Feature Filter panels
- For large, feature rich models, the preferred method is to click "Selected Features" in the Scope panel, then manually select features within the 3-D model. Doing so will constrain DimXpert to create dimensions and tolerances for the selected features only.
- An effective alternative is to select "All features" in the Scope panel, and then selectively enable feature types in the Feature Filters panel.
- These techniques are especially effective for models than contain numerous, complex fillets or chamfers.
- After constraining the DimXpert Auto Dimension Scheme function as described above, click the OK button (green check sign) to execute the auto dimensioning function.
- The Auto Dimension Scheme function can be used on the same part multiple times to create sets of dimensions and tolerances that have been constrained to specific datums, selections or feature types.
If there are too many 3-D dimensions and tolerances in a single Annotation View, create a new Annotation View based upon the same orientation. Select annotations to be moved, then right-click and select Change Annotation View ([active view name]) -> [name of new view with same orientation].
- When moving annotations between views be sure that the two views share the same orientation.
- When selecting dimensions and tolerances to move to another Annotation View, be sure to select both the dimension and the tolerance (the entire feature control frame) before using the Change Annotation View command.
After SolidWorks has completed the Auto Dimensioning process, expand the Annotations folder in the SolidWorks FeatureManager, control-click each Annotation View (including the "Unassigned Items" object, then select "Hide" from the right-click menu. Hiding Annotation Views in this manner will hide 3-D annotations that do not belong to the active Annotation View.
After running Auto Dimension Scheme, Activate and Reorient each Annotation View and adjust the location/placement of each annotation as desired.
Click the Show Tolerance Status button to see which features are under or over constrained for size and location. The Show Tolerance Status feature provides visual clues (yellow or green face color) to indicate whether a feature is properly constrained. Face coloring can also be used to show which model features have yet to be annotated. Please note that the status of a feature will not be affected by the use of RefDims. In other words, RefDims have no affect on the DimXpert solution.
DimXpert dimensions and tolerances can also be added manually using the Location Dimension, Size Dimension, Datum, Geometric Tolerance, and Pattern Feature controls within he DimXpert toolbar.
Please note: Datums to be referenced in DimXpert geometric tolerances must be created prior to creating the geometric tolerance.
Please note: DimXpert Datum tags must be unique; it is not possible to create more than one DimXpert datum tag with the same label. If a datum tag should be visible in more than one Annotation View, create a DimXpert Datum tag in one Annotation View, then create a another Datum tag using the Datum Feature button in the Annotation toolbar. Since there can be only one DimXpert dimension for any specific feature, this technique can also be used to create multiple dimensions of the same feature within different Annotation Views.
For more information about using DimXpert please consult the SolidWorks Help document. In particular, see the following DimXpert Help sections:
- DimXpert for Parts
- Using the Feature Selector
- Changing Annotation Planes
- Combining Dimensions
- DimXpert Tools
RefDims and other 3-D Annotations
The 2nd "toolbox" for creating 3-D dimensions, tolerances, weld symbols, surface profiles, and other annotations is accessed via the SolidWorks Annotation Toolbar. To access the Annotation toolbar, select View->Toolbars->Annotation.
As noted previously, before creating a dimension, tolerance, or other annotation, be sure to create an Annotation View first, then Activate (and Orient) the view.
To create a Reference dimension:
- Click the button labeled "Smart Dimension" located at the top of the Annotation toolbar. Next, be sure to select "Reference dimension" from the Dimension panel.
Click on a planar face, edge, point, or reference geometry to create a dimension.
- Currently, it is not possible to move the annotation plane of a Reference dimension after it has been created.
To create Geometric tolerances:
- Geometric tolerances can be created by clicking the Geometric Tolerance icon in the Annotation toolbar. Unlike DimXpert geometric tolerances, there is no requirement that datums exist prior to adding them to the geometric tolerance symbol (feature control frame).
- Geometric tolerances can be leadered or unleadered. To attach a geometric tolerance to a dimension, click the Geometric Tolerance button in the Annotation toolbar, then click on an existing dimension. Enter the symbol, tolerance, and datum references as required.
To create Notes:
- To create a 3-D Note annotation, click the Note button in the Annotation toolbar.
- Notes can be linked to existing Custom or Configuration Specific properties, or can contain formatted text copied from another source or entered by hand.
- To create a Note with multiple leaderlines, select a set of faces, edges, or points on the model, then click the Note button.
- To create a Note without a leaderline, deselect faces, edges, or points in the model.
- Create a leaderline for an existing Note by selecting the note, then selecting the appropriate button in the Leader panel within the Note properties.
- This technique is handy if leadered, flat to screen notes are required.
Recommended Annotation Process
To ensure that annotations are created within specific desired Annotation Views, follow this procedure:
- To create an Annotation View manually, right click on the Annotations folder and select Insert Annotation View
- Before manually adding a DimXpert annotation, Reference dimension, or other 3-D note, ALWAYS right click on a specific Annotation View and select Activate and Reorient
- ALWAYS add an annotation to the "active" Annotation View
Try to avoid:
- Adding 3-D annotations "on the fly" without activating and orienting an Annotation View first
- Moving annotations from one Annotation View orientation to another Annotation View with a different orientation (for example, moving an annotation from TOP to LEFT)
To ensure that annotations within a specific activated Annotation View are visible, follow this procedure (only needs to be done once, for example after running DimXpert Auto Dimension Scheme):
- CTL-CLICK each Annotation View in the Annotations folder
- Right click and select Hide from the right click menu
If you need to move an annotation to another Annotation view, follow this process:
- Move the annotation to another view with same orientation. (Create the new annotation view first)
- If the dimension has a GTOL, select the GTOL first, then the dimension, then right click and select Change Annotation View... to move. This ensures both are moved to the new annotation view
- If a GTOL doesn’t appear in an Annotation View, find the GTOL, then right click and look for the Change Annotation View... command. The Annotation View that the GTOL belongs to should appear in parentheses
The evolution to 3-D MBD and away from 2-D drawings is inevitable, and new 3-D MBD publishing solutions are enabling a wide range of "model-based applications" for model based enterprises. While a transition to a model-based practice can't be accomplished overnight, a growing number of large manufacturers are proving that while the path may not be well worn, at least it is clear—and that the benefits of model-based engineering are real.
The internet, and the rise of "instant gratification" social media tools like Facebook, YouTube, and Twitter did not exist during the last great CAD revolution (2-D to 3-D), and a mass-market transition to 3-D MBD practices will happen quickly once it catches fire. With a growing number of CAD users becoming familiar—if not adept—at using 3-D MBD tools in applications like CATIA, CREO, NX, and SolidWorks, the ability to find help online and draw upon the experience of others will only hasten this transition.