I want the basic dimension 100 and the datum to be aligned with each other to symbolize a width datum. How do I do that? As can be seen above, I can attach the datum and basic dimension as separate "lines" but that's not what I want, I want them to be the same line. I'm using SOLIDWORKS 2017
Hey Bob,
Per ASME Y14.5:2009, a width feature is a feature of size. So here are the steps:
1. Click on the DimXpert Size Dimension, not Location Dimension;
2. Pick one face and select Create Width in the context command bar.
3. Pick the opposing parallel face.
4. Place the width feature size callout.
5. Click on the DimXpert Datum button.
6. Select one of the above face, the default option should be to establish the width as a datum feature.
7. You'll notice the datum symbol is automatically attached to the dimension, both faces are highlighted, and the datum symbol moves together with the dimension line to comply with the ASME Y14.5:2009 standard.
8. Please note that the datum (not datum feature) is the theoretical middle plane between the two parallel faces, so if you'd like to measure anything from a middle plane, a width feature can give you that.
Hope it helps.
-Oboe
Bob, excuse my ignorance as we do not use the MBD Feature but I would assume it should work just as if you were to dimension the feature on a drawing. You should be able to attach the Datum by selecting the dimension itself.
I tried it very briefly and was able to select the dimension, right click, select "annotations" and place a datum. The alignment/view was not what I would like to see but I'm hopeful it's my lack of experience using this feature.
