I am often asked how to reuse sketch dimensions in model-based definition (MBD) workflows. The advantages seem obvious. Some manufacturers establish internal policies to define sketch dimensions and tolerances. Reusing them in 3D can save the annotating time and effort. It also helps eliminate discrepancies between sketch dimensions and annotations by other annotating tools, such as DimXpert and reference dimensions.
However, as I explained in a previous article, reusing sketch dimensions is derived from a 3D-drawing approach, therefore it can’t realize the full potential of model-based workflows. In this article, let’s start with 3D drawing use cases and review several SOLIDWORKS techniques to serve the various need.
To begin with, as shown in Figure 1, you can check the line to Show Feature Dimensions as pointed by the green arrow. Here, Feature Dimensions include both sketch dimensions and feature dimensions. In my opinion, the categorization and naming are a bit confusing and could certainly be improved.
The other way to control the display settings all together is the dialog as shown in Figure 2. You can invoke this dialog by clicking on the Details command line on top of the context menu, as shown in Figure 1.
Now with all the annotations and dimensions selected, Figure 3 shows the graphics area.
By default, sketch dimensions, such as the 45-degree close to the shaft shoulder, and reference annotations, such as the NOTES at the top of the image, are in black. Feature dimensions are in blue, and DimXpert annotations are in green. Lastly, reference dimensions are in grey, such as the seal grove annotations R0.20 and R1 on the left.
Now with everything shown, you may find the viewport very busy and hard to digest. Let’s take the thread example on the right side and organize its annotations for easier consumptions.
First, zoom into the helixcoil feature to show its thread characteristics. As you can see, the annotations overlap on top of each other. Some are even buried in the model.
To clean up the display, let’s hide the reference dimensions, DimXpert annotations and reference annotations by unchecking their line items as shown in Figure 5.
Next, you can selectively hide sketch and feature dimensions to focus on the helix coil. For example, Figure 6 shows that I selected the 50 mm feature dimension of an angled hole length. You can make it invisible by clicking Hide on its context menu.
Figure 7 shows that I’m trying to select the 8.40 mm shoulder width sketch dimension. However, because the Instant3D feature is turned on by default, a single-click selection activated this annotation for editing because sketch dimensions are driving, not driven dimensions. In this case, turn off the Instant3D feature to avoid unintended modifications.
Next, repeat the step as shown in Figure 6 to hide irrelevant annotations. You will find a much cleaner view as shown in Figure 7. One point worth noting is that I didn’t find a way to select multiple annotations and hide them together, so I had to hide them one by one. It’d be great if multiple sketch and feature dimensions could be hidden together.
Now, you may find the text size too big for this detailed view. The software provides a quick setting to always display text at the same size, as shown in Figure 9.
Once you are happy with the current display, remember to capture it as a 3D View so that you can quickly retrieve it later. Figure 10 shows a 3D View named as Thread_FeatureDim with a thumbnail at the bottom.
It’s nice to see that the setting, “Always display text at the same size,” is specific to the 3D Views. We had it checked in the 3D View “Thread_FeatureDim.” You can also uncheck it and have it remembered in another 3D View. For example, in a zoomed-out overview, as shown in Figure 11, you may want a bigger text scale specific to this view.
By the way, if the text size looks too big in Figure 8, but too small in Figure 9, you can also adjust the text font sizes individually as shown in Figure 12.
The good news here is that you can hold the control key to select multiple annotations and adjust their fonts together. Go to the Other tab on the property manager and clear the “Document font” checkbox to overwrite it. Then click on the Font button to modify the font.
By the way, if you need to add tolerances to certain sketch dimensions, you can modify them directly in 3D without having to edit the sketch. Figure 13 shows that a 2 mm distance is selected, and its tolerance is set to symmetric on the property manager.
Now that we have fine-tuned the sketch dimensions, tolerances and display, you can export the model to STEP 242 or 3D PDF files. The sketch dimensions are supported in the neutral formats. Figure 14 shows an imported STEP 242 file in SOLIDWORKS MBD. You may notice the annotations and views preserved in the export and brought in again by the import.
I hope that this article is helpful. It is important to point out that reusing sketch dimensions is just to serve the 3D drawing needs at the initial phase of MBD implementation. This practice doesn’t support geometric dimensioning and tolerancing (GD&T) definitions. The sketch dimensions are the constructing elements of features, so they are not fully aware of the manufacturing features. Therefore sketch dimensions can’t effectively support the manufacturing automations based on semantic 3D annotations. First identify short-term and long-term goals and use cases of your MBD implementations, then you can choose the 3D annotation strategies accordingly.
If you have any comments or questions, please feel free to leave them in the comments area below. To learn more about how SOLIDWORKS MBD can help implement your model-based enterprises, please visit its product page.
About the Author
Oboe Wu is a SOLIDWORKS product manager with 20 years of experience in engineering and software. He is an advocate of model-based enterprise and smart manufacturing.