Three Key Points to Bear in Mind When Reusing Sketch Dimensions in Model-Based Workflows

At SOLIDWORKS World 2018, several customers asked about how to reuse sketch dimensions in model-based workflows, so I shared some techniques in this article. The idea is similar to inheriting model items from 3D models to 2D drawings. However, in this post, I thought it would be important to clarify the pros and cons of reusing sketch dimensions, especially the key areas to watch for in your model-based definition (MBD) implementations.

The previous article talked about several obvious benefits. For example, it can help save the 3D annotating time and effort by exposing the existing sketch annotations. This approach can also help avoid the potential inconsistencies between sketch annotations and other annotations in tools such as DimXpert and Reference Dimensions. Therefore, this practice may be able to give you a head start toward the 3D drawing direction.

However, MBD is way beyond 3D drawings. Now let’s look into the areas that you may need to be aware of when reusing sketch dimensions.

  1. Sketch Dimensions Are Not Aware of the Features

To build a feature in SOLIDWORKS, typically you start with a sketch in which you can add sketch dimensions and tolerances. Then you can extrude, cut or revolve, along with many other tools to turn a sketch into a 3D feature. But it’s important to realize that a sketch is just a constructing element of a feature in the early phase. It doesn’t know what a final feature will end up with. Therefore, sketch dimensions can’t convey the full meaning of features. Figure 1 shows one instance in which the sketch dimensions are exposed in 3D to define a countersink hole.

Figure 1. Sketch dimensions are exposed in 3D to define a countersink hole.

It may seem fine, especially from the 2D drawing convention perspective. Many users have got used to this type of presentation and corresponding interpretations. The 90 degrees probably refers to the countersink angle. The 20mm diameter defines the countersink opening and 14mm diameter defines the hole. Also you may guess this definition is applicable to a series of identical holes along the border, although you may not be sure how many instances it covers without a careful manual count.

By the way, there are likely to be many sketch dimensions once you show them in 3D. So please control their visibilities carefully by hiding unwanted ones and organizing them with annotation views. Otherwise, the view may look busy and even overwhelming. Figure 2 shows one example.

Figure 2. A busy display with multiple sketch dimensions visible at the same time.

As a comparison to Figure 1, Figure 3 shows a different way in which all the instances of a countersink hole pattern are defined in one combined callout.

Figure 3. A countersink hole pattern is defined by DimXpert.

Here the 30X clearly indicates the instance count. The V-shape symbol tells that it is a countersink. Plus, selecting the callout highlights the entire pattern that has been defined by the callout. The DimXpert annotation is added after the pattern has been constructed, so it can convey the pattern definition more comprehensively. The comparison between Figure 1 and Figure 3 illustrates a difference between 3D drawings and MBD.

  1. Sketch Dimensions Can’t Necessarily Guide How a Feature Should Be Manufactured or Inspected

The purpose of a sketch in parametric modeling is to construct features geometrically in 3D. However, a sketch is not fully aware of the feature to be completed afterwards, so the dimensions and tolerances in a sketch can’t necessarily be used to guide manufacturing or inspection. For example, Figure 4 shows the sketch dimensions of a circular hole pattern.

Figure 4. Sketch dimensions of a circular hole pattern.

If your milling operation is based on linear x, y and z coordinates, then these sketch dimensions may work fine. However, if you index this circular hole pattern on a rotary table for drilling such as the one shown in Figure 5, what you conveniently need is probably the dividing angles between the hole instances and their pitch circle diameter.

Figure 5. Index a circular hole pattern on a rotary table for drilling.

Therefore, the polar dimensioning style using DimXpert as shown in Figure 6 may come in handy.

Figure 6. Define the polar dimensions of dividing angles and the pitch circle diameter using DimXpert.

Furthermore, this way of drilling may work faster and reduce the scrap and rework, because you only need to rotate the table by certain degrees to drill the next hole once the pitch circle diameter is locked down. You don’t have to move the drill bit at all. In contrast, to machine according to the linear dimensions as shown in Figure 4, you will have to adjust the x and y coordinates of the drill bit for each hole instance.

Another case is to provide key information for inspection. Let’s again take the sketch dimensions in Figure 4 as an example. We located the counterbore holes but didn’t tell an inspector the wall thickness, or the distance from the biggest hole to the outer diameter, should the thickness become a concern. Therefore, you may want to add a DimXpert annotation to call out a wall thickness as shown in Figure 7. Please note that you can adjust the arc conditions on the property manager to retrieve the minimum distance between the outer cylinder and the counterbore cylinder.

Figure 7. Adjust the arc conditions to retrieve a wall thickness using DimXpert.

Similarly, in the context of a manufacturing process, due to the lack of 3D feature awareness, sketch dimensions don’t support geometric dimensioning and tolerancing(GD&T) definitions such as datum features, datum targets or feature control frames, nor do they support surface finishes or weld symbols. These definitions are best conveyed in 3D models to convey instructions and requirements unambiguously. After all, 3D features are up to multiple modifications and refinements after the sketches are defined. Therefore, the initial sketches may not be accurate or actionable any longer for manufacturing and inspection.

More details about GD&T in the MBD context can be found in Three MBD Advantages over 2D Drawings in GD&T Compliances and Ensure Solid GD&T Datum Practices with SOLIDWORKS MBD.

  1. Sketch Dimensions Can’t Efficiently Drive Manufacturing Automations

In a previous article, I summarized the top 5 reasons to use MBD. In my opinion, the most significant benefit of MBD comes from the manufacturing automations, not from 2D drawing avoidances. For instance, based on the intelligent feature-based 3D annotations, machining and inspection software applications, such as computer-aided manufacturing (CAM) or coordinate measuring machines (CMMs),can make automatic decisions and cut programing time from hours to minutes. Figure 8 shows one example of the automated CMM programming and a quality heat map per 3D GD&T annotations.

Figure 8. Automated CMM programming and a quality heat map per 3D GD&T annotations.

This type of automations depends on the feature awareness, so sketch dimensions may fall short. However, in the future, maybe SOLIDWORKS can provide a capability to convert sketch annotations into intelligent feature-based annotations when certain sketches are representative enough of the 3D features. But for complex features heavily morphed away from basic sketches, sketch dimensions may not lead to meaningful actions worthy of any conversions.

I hope that this article clarifies the areas to be careful about when you are trying to reuse sketch dimensions. 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 the 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.

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