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How to add dimensions in SolidWorks drawings?

Drawings are a means of communicating the relevant information and requirements to manufacture an part or product. This is accomplished by ensuring the necessary dimensions and tolerances have been included. Dimensions can be added to a drawing manually or automatically. This tutorial will cover Smart Dimension, Import Annotations and Model Items.

Smart Dimension

Use Smart Dimension to apply dimensions to a drawing manually. Changes to these dimensions do not affect the model. To change a dimension, edit the corresponding part or assembly. The dimensions in the drawing update after changes are made. Using smart dimension in a drawing is the same as creating dimensions in a sketch. Refer to the tutorial “How to smart dimension an angle in SolidWorks” for more information.

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Dimensions that do not update may have been overwritten, check the dimension properties. Overriding dimensions is not advisable, but it does occur. Check that <DIM> has not been deleted from the dimension text.

An overwritten dimension will have a value in place of <DIM>. To reset the link either type <DIM> or select the add value button.

Import Annotations

Dimensions from sketches can be imported to the drawing. When placing the front view, select “Import annotations” and “Design annotations” from the import options. If the view has already been placed, select the view and the same two options can be selected from the view properties.

SolidWorks imports dimensions that are marked for import.

Editing the values of imported dimensions will change them in the part. It is recommended to open the assembly to confirm the update has not caused interference.

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Tip: Place dimensions, in sketches, as they are to appear in the drawing. This will save time repositioning them in the drawing. Edit precision and add tolerances to dimensions to avoid this in the drawing.

Model Items

Model items is an alternative to import dimensions, it can import dimensions to all views. In the example to follow, the 85mm hole was replaced using hole wizard.

Source – Selected feature or entire model. Tick import items into all views or select the views to place the dimensions.

Dimensions – can import marked or not marked dimensions, instance/revolution count, tolerances, as well as hole wizard (profile, location, callout) information. The hole is constrained concentrically to curved edge of the extrude.

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Annotations – this section offers to import notes, surface finish, geometric tolerances and datums, weld information and end treatment information.

Reference Geometry – imports reference geometry including CoG, curves and routing points.

Options – Use dimension placement in sketch if they have been laid out thoughtfully. Try without this option to see if they are imported in a neater format.

Layer – Import model items to a specific layer.