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: “4.9-5.13.4-3.8”.
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 ‘A’ 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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