In the first and second parts of this guide, we worked on the hole callouts in Figure 1, such as the internal and external diameters, the custom text orientations, the distances from intersection planes, the datum attachment styles, the hole selections and the polar dimensions.
Figure 1. 2D drawing of a simplified bearing housing.
When creating the polar coordinates of the flange hole pattern in the second part of the guide, we used the SOLIDWORKS Auto Dimension Scheme. To pick the primary, secondary and tertiary datum reference features one by one, we had to move the mouse cursor back and forth between the model in the graphics area and the left-hand property manager. That could result in pretty time-consuming mouse travels. Luckily, we have several handy time savers here, but they may not be very discoverable, hence not well-known yet.
After picking the first datum feature, rather than going back to the property manager to switch to the second datum input box and then return to the model for another pick, we can simply right-click right there without any mouse cursor movement. One click not only accepts the first datum selection, but also switches the focus to the second datum input box as shown in Figure 2. You may notice a small blue Enter key icon on the right mouse button in Figure 2 indicating this shortcut. As long as the mouse cursor is over this feature, the bottom Plane 7 in this case, this right-click acceptance button is available. Simply put, we can just left-click on a feature to pick it, right-click to accept it and move on to the next feature without any mouse travel.
Figure 2. Accept a datum selection with a right-click.
What if we have moved our mouse cursor away from the first datum feature? We can still accept the datum selection using an in-context menu command as shown in Figure 3. Of course, the OK button on this in-context menu can execute the Auto Dimension Scheme on the spot.
Figure 3. Accept a datum selection via an in-context menu command.
To continue the flange hole pattern definition, let’s further specify the position tolerance as shown in Figure 1. It’s pretty straightforward to define a geometric tolerance, but one trick here is to directly drop a feature control frame onto an existing callout so that they are correctly oriented and concisely combined as shown in Figure 4. There is a presentation issue in this new combination. We will fix it later.
Figure 4. Drop a feature control frame to a callout directly.
You may notice there are some basic dimensions on the right-hand view that we haven’t touched yet. There are several reasons:
- In geometric dimensioning and tolerancing (GD&T) terms, basic dimensions define the theoretically ideal locations and sizes of features. Therefore, they don’t specify tolerance zones and generally are surrounded in box borders. Actually, 3D CAD models are theoretical and implicitly convey the feature locations and sizes already. If necessary, simple model queries can provide these dimensions. So explicit basic dimensions in the model-based definition (MBD) approach are less important than in 2D drawings. They repeat existing information just for quick visual readings.
- Beyond visual readings, many software programs such as those involved in computer-aided manufacturing (CAM) and coordinate measuring machines (CMM) can read 3D CAD models directly to automate numeric control (NC) code generation. So the implicit basic dimensions in the model are digitally consumed seamlessly, which further alleviates the need for explicit ones.
However, in order to ease the transition to the MBD processes, sometimes we need to accommodate 2D drawing conventions, even if they may not be very relevant in the MBD approach any more. Explicit basic dimensions are one example. Sometimes, the data consumers may still need, or like, to see these callouts on digital drawings or hard copy printouts. SOLIDWORKS MBD provides many automatic ways so that we don’t have to annotate each one manually. For example, we can right-click on the position tolerance in the DimXpert tree and select the “Recreate basic dim” command on its in-context menu as shown in Figure 5. One click will create all the constructive basic dimensions for this hole position geometric tolerance automatically. This command is pretty powerful, but also not very discoverable. I hope you find it helpful.
As illustrated in the first part of the guide, to save some space, we can align the dimension text with the dimension line using the Custom Text Position options on the Leaders tab of the property manager. Now, with several quick placement adjustments, these callouts are presented clearly in Figure 5.
Figure 5. Recreate basic dimensions automatically.
We can create these only for selected feature control frames using this command, or we may choose to apply this creation for all feature control frames automatically if this is a company or personal preference. Figure 6 shows a Document Property setting under DimXpert > Geometric Tolerance. By checking the box “Create basic dimensions,” we are enabling this automatic creation for this entire document. There are also Chain and Baseline styles for us to choose.
Figure 6. A document setting to create basic dimension.
Besides the above automatic creations, SOLIDWORKS MBD provides a dedicated Basic Dimension button on its command bar. So we can create all the basic dimensions in Figure 5 manually, too. It’s more flexible, but takes more time.
Now that we have created all the callouts in the 3D model following the 2D drawing in Figure 1, it’s time to review and tie up several loose ends we left earlier. Norm Crawford with Crawford Dimensional Management pointed out that the position tolerance attached to the combined counterbore callout is confusing. Is it controlling the bigger diameter, Φ.264±.005 in., or the smaller one, Φ.134±.005 in? The actual mounting feature is the smaller holes. So let’s be more specific here by breaking this combination as shown in Figure 7. Now the result in Figure 8 is much clearer visually.
Figure 7. Break the callout dimension combination.
Figure 8. A position tolerance is attached to the correct callout.
I should also mention that once the combination is broken, the position tolerance is automatically attached to the correct mounting hole callout. That is because SOLIDWORKS MBD automatically associates the feature control frame with the correct feature in Figure 4. If you remember, we just dropped it to the combined callout. We didn’t even pick a feature there.
Common engineering experiences tell us what really matters in a counterbore is the actual mounting hole. The top flat is mostly just to accommodate a bolt head. This kind of experience has been built in to the software to structure more intelligent definitions. It may seem trivial visually, but in streamlined MBD processes, this semantic association and data structure make significant differences in the 3D PMI consumption for downstream manufacturing software. CAMWorks for machining or CheckMate for inspection are two examples here: they can read the intelligent 3D PMI by SOLIDWORKS MBD to further automate the production.
We finished this case study in Figure 1 and also improved the callouts in the 3D model. We covered many useful-but-not-well-known tips and tricks such as the datum selection acceptance in the Auto Dimension Scheme, dropping a feature control frame to a callout directly and the “Recreate basic dim” command for a position tolerance. Your comments are welcome below. To learn more about how SOLIDWORKS MBD can help you with your MBD implementation, please visit its product page.
About the Author
Oboe Wu is a SOLIDWORKS MBD product manager with 20 years of experience in engineering and software. He is an advocate of model-based enterprise (MBE) and smart manufacturing.