ASME Y14.41, Digital Product Definition Data Practices, was introduced in 2003 to bring ASME Y14.5M into the digital age. In short, ASME Y14.41 allows you to dimension and tolerance a 3D model without the need for a paper drawing. SolidWorks 2008 took a big step in the direction of adopting this standard with the addition of the DimXpert for parts. DimXpert for parts uses feature recognition and topological recognition to supported manufacturing features in your model such as bosses, chamfers, cylinders, simple holes, slots and others. Today using the Auto Dimension Scheme will will dimension a simple part from our press assembly. Later in the week, I will be covering some more advanced techniques when using the DimXpert for parts.

Auto Dimensioning a Simple Part

In our simple part, select the DimXpertManager tab in the FeatureManager.

In the DimXpertManager click the Auto Dimension Scheme button.

In the Settings section select whether your part is a Prismatic or Turned part. A Prismatic part would be most likely machined using a mill and a Turned part is most often done with a lathe. Since our part is a simple block with a full holes and a groove, we will select Prismatic. Next, select what type of tolerance will be applied. If you are like most people you might want to pick Plus and Minus but give me a few weeks and you’ll jump into the Geometric tolerancing like a pro.

Next, we will select our Datum References. Every part is different and you have to think about how the part will be inspected by your quality control department. In this case, we want our datums to be the back, top and left planes of the part. These are considered mutually perpendicular planes and provide a good origin.

You will notice that the planes selected are color coded to match the Primary, Secondary and Tertiary Datums.

Select the Scope of the features you wish to be dimensioned. Since this is a simple part we can get away with selecting All Features, more complex parts may require you to individually select which features to be dimensioned. In the Feature Filters section, Select the features types that you wish to be recognized. Deselecting a feature type will cause all those features to be omitted from the calculation.

When you are finished with your selections, click the green check mark and the part will be fully dimensioned. The created dimensions are based on the actual geometry of the part and are not based on sketch dimensions. Depending on the complexity of your part you may find it necessary to change your layout for readability but since this is a simple part it is not necessary here.

Creating a Drawing from a Dimensioned Part

Even though, per ASME Y14.41, you do not need to create a drawing your company standards may still require you to do so. The best thing about using the DimXpert for parts, the work is already done for you. When you insert the model into your drawing select DimXpert annotations in the Import Options section and the drawing will be created with the annotations you created.

Now all you have to do is arrange your dimensions for optimum readability and you done. Too easy!

Now like a mentioned is is just a quick introduction to the DimXpert for parts. In future post I will be digging deeper into this powerful tool and show some cool things you will be able to do. SO make sure you stick around.

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