Type to search

Top SOLIDWORKS MBD Tips and Tricks: Hole Callouts

CAD Concept Design

Top SOLIDWORKS MBD Tips and Tricks: Hole Callouts

For mechanical engineers and designers, holes are one of the most frequently used features in engineering design. They are often used to mount with other components or to support shafts. In model-based definition (MBD) implementations, I am often asked how to dimension and tolerance internal or external diameters in 3D in a way that is similar to 2D drawings, such as the bearing housing in Figure 1. Let’s walk through this situation and see what tools are available in SOLIDWORKS MBD to help us out.

2D_DrawingFigure 1. 2D drawing of a simplified bearing housing.

First, it’s pretty straightforward to define diameters in SOLIDWORKS MBD. Just remember to use the size dimension, rather than the location dimension. This distinction complies with the ASME Y14.5-2009 geometric dimensioning and tolerancing (GD&T) standard, whereby diameters are defined as features of size and can be quickly inspected with a functional gauge pin. With just a few clicks, we can easily drop several callouts, as shown in Figure 2.

Figure 2. Initial diameter callouts.

But it comes with several problems:

  1. Most of the callout leader lines and arrows are obscured by the model, so it’s not very easy to tell which diameter is associated with which hole, except for the selected Φ.754±.005 in green cross-highlighting its corresponding feature. This cross highlighting indication is required in ASME Y14.41-2012 as “Visual Response,” which works well for an individual query in SOLIDWORKS MBD, but lacks a clear overview of all the annotation anchors and doesn’t work on paper printouts.
  2. In the 2D drawing layout in Figure 1, a section view is nicely integrated with annotations to present both its complex internal contour and attached callouts. If we cut a section view in 3D, as shown in Figure 3, some annotations are floating because the model body part they are attached to is cut out, which makes it more misleading and confusing.

Figure 3. Floating annotations in a section view.

So how can we adjust leader styles and reorient these diameter callouts to achieve the same result in 3D as in the 2D drawing in Figure 1? Let’s again pick this highlighted Φ.754±.005 callout as an example. First, to host the to-be-reoriented annotation in an appropriate Annotation View, let’s make sure the Right Annotation View is activated as shown in Figure 4.

Figure 4. Activate the Right annotation view.

Then the following several quick clicks in Figure 5 will give us the expected style.

  1. Select Φ.754±.005 and click on the Leaders tab on its property manager;
  2. Switch from Diameter leader style to Linear leader style;
  3. Under Linear leader style, click on the Parallel To Axis button, which means the annotation plane is now parallel, not perpendicular, to the hole axis. To be more precise, they are actually coplanar in this case.

Figure 5. Three clicks to reorient a diameter callout Parallel To Axis.

Repeat this adjustment to other diameters and we will get much closer results in Figure 6.

Figure 6. All diameter callouts reoriented in a section view.

A quick note here: If we didn’t activate an appropriate host Annotation View before these adjustments, we may get placements similar to the highlighted one in Figure 7, depending on which Annotation View or orientation is active, but we can still manually reassign these callouts to a desirable Annotation View in two ways:

  • Right mouse click on a callout and click Select Annotation View from its context menu as shown in Figures 7 and 8. You may notice the annotation orientations are previewed instantly and dynamically as your mouse cursor moves through each option in the pop-up list in Figure 8.

Figure 7. Select Annotation View command in the context menu.

Figure 8. Pick an Annotation View from the pop-up list.

  • One shortcut here is to press the tilde key (˜) above the tab key on a keyboard while an annotation is selected. Then this Annotation View list will pop up for selection. This shortcut is not only faster, but can also preview annotation view results on the fly in a command to facilitate better decision before a placement. On a side note, the tilde key was chosen in this software behavior design rather than the tab key because the tab key is already used in overall design to cycle through various controls on the Property Manager, which is a standard Windows operating system behavior.

With all the above hands-on experiments, hopefully we have a better understanding of the relationship between callouts and annotation views. A natural question to ask now is if we do start with an activated Section Annotation View like the view on the left in Figure 1, can we get those diameter annotation orientations (parallel to axis) right away without the above adjustments? The answer is yes, as shown in Figure 9. With this Section View A-A activated, we can directly drop a hole callout parallel to the hole axis using the Size Dimension command.

Figure 9. Direct hole callout parallel to axis when a Section Annotation View is activated.

Now, comparing Figure 1 and Figure 6, you may notice that we still have some work to do. For example, the text orientation perpendicular to dimension lines takes substantial space to avoid overlapping, which isn’t very efficient for layout and printing. Also, there are two identical Φ.754±.005 callouts, which would be better if combined to save screen or paper space. Third, all the tolerances are .005 in., but in reality, sometimes we may want to loosen some to save manufacturing and inspection costs. Or we may need tighter tolerances on critical features. For example, holes to hold bearings or shafts in this case.

To begin, aligning texts with dimension lines is really easy. Just hold the Ctrl key to multi-select all the diameter callouts and then switch to the Leaders tab on the Property Manager. Scroll down to the bottom, check the Custom Text Position box and click on the first button, Solid Leader, Aligned Text, as shown in Figure 10, and we are all set here. By the way, when these callouts come pretty close to each other, accurately selecting one may become a bit harder. An easier way is to click on dimension witness lines or leader arrows, rather than the texts.

Figure 10. Aligned text with dimension lines for multi-selected annotations.

Next, hold the Ctrl key to multi-select these two identical Φ.754±.005 callouts, and then right click to display its context menu. Here the command Combine Dimension (Figure 11) can give us the expected 2x result, and this combined annotation can cross highlight both features. Of course, this works for more instances in a combination too. Also, to be eligible for a combination, all instances must be identical. When necessary, we can break a combination into individual pieces. Just right click and select Break Combined Dimension as shown in Figure 12.

Figure 11. Combine identical dimensions.

Figure 12. Cross highlight on both features and Break Combined Dimension.

Lastly, we can loosen several tolerances to possibly save manufacturing and inspection costs. Again we can hold the Ctrl key to multi-select the highlighted three callouts and modify their tolerances to 0.010 in. together.

Figure 13. Modify tolerances for multiple callouts together.

Another handy tool is Style. Let’s try the opposite by actually tightening these three tolerances from 0.010 in. to 0.003 in. because these holes are supporting the bearings or shaft. We can modify one first, or just pick an existing desirable annotation style, and add it as a style (Figure 14), and then apply it to other annotations (Figure 15). We can also save this style as a file and load it later, so that we can reuse it not only in this session, but also in other sessions or on other computers. This reuse of styles can save quite a few mouse clicks and typing, while maintaining better consistency.

Figure 14. Add an annotation style.

Figure 15. Apply an annotation style to multiple callouts.

Now Figure 16 presents a section view with desired diameter callouts similar to Figure 1 after following tips and tricks:

  • Reorient diameter callouts to parallel to axis
  • Change annotation views using the context menu or tilde key
  • Adjust custom text positions with multi-selection
  • Combine and break dimensions
  • Modify tolerances together with multi-selection
  • Add and load a style to multiple annotations

Figure 16. 3D section view with diameter callouts parallel to axis and cross highlighting from a combined annotation to two hole features.

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.  


You Might also Like