ASME Y14.41 revisited with SolidWorks, Minimum Content Drawings

Minimum Content Drawing
After investigating ASME Y14.41 Digital Product Definition Data Practices and receiving great assistance from users in this forum, I
would like to share my findings as promised at SolidWorks World. The Y14.41 standard is used in conjunction with Y14.5.
A Minimum Content Drawing (MCD) documents key features during electronic distribution of the model. As a designer, you supply model data to the manufacturer. You also determine the critical dimensions and annotations that must be adhered to in the manufacturing and inspection process.
The MCD contains some or all of the following: overall dimensions, specific feature dimensions, tolerance, datums and annotations that are critical. The drawing also documents the name of the electronic file and references the standard.
In the SW model, the following annotations are inserted: Notes, Geometric Tolerances, Datums, and Dimensions, including tolerance and precision on the individual dimension.
To display dimensions and annotations, Right-click on the Annotations folder, select Display Annotations, select Display Feature Dimensions. Drag the dimensions and annotations outward to leave space. To hide dimensions on features, Right-click Hide All Dimensions. Work only with key features. This can get very messy in the model; select only the information that is critical.
Hide All Dimensions for Hole Wizard holes. Label Hole dimensions as a Note. Example: &#8220;<mod-diam>4.9-5.1<hole-depth>3.4-3.8&#8221;.
Annotated Isometric views are required in the drawing. Control these views with configurations in the part. The first configuration is an Extruded Cut that represents a section view. The second configuration is a simple rectangular sketch with a note &#8216;A&#8217; and a direction arrow indicating a Sketch plane on the Full view. The drawing requires a section plane not a section line to indicate the cutting plane.
Create new named views in the part to show additional features.
You could also utilize the True Isometric option and display a reference plane in the Isometric Drawing view. However, no letter or arrow is displayed with this option.
Once inside the drawing, utilize Insert Model Items to bring over notes and geometric tolerances into an Isometric view. Model dimensions do not insert into an isometric of the drawing. Verify that note arrows point to the profile (visible) of the feature.
Activate the Drawing view before inserting notes, dimensions or any sketched item. The view boundary is displayed in green when activated.
Create dimensions in the Isometric view for overall width-height-depth of key features. Select dimension references carefully in the Isometric view. Select lines versus points. Return to the part to verify dimensions.
Insert additional Isometric views. Right-click Properties in the view and display the different configurations for the Section view and Section plane.
A Datum annotation can be inserted onto a face parallel to the top plane in the Isometric view. Insert Datum symbols on the dimension or on feature control frame.
You can create a Detail view of an Isometric view.
Work outside the sheet boundary to add notes and or other views to reference.
Insert additional views that complete the documentation. MCD drawings utilize multiple sheets as more features are documented. Modify sheet names to assist in locating features and views.
Add a note on the drawing the references the electronic model file and the standard.
The Y14 Engineering Drawing and Related Documentation Practices are published by ASME (
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