Be careful using SOLIDWORKS Convert to Bodies on models with referenced drawings

Article by Chris Briand, CSWE updated November 7, 2016


In an earlier article, I introduced the New Convert to Bodies functionality available in SOLIDWORKS 2017. If you are considering the use of the “Convert to Bodies” functionality be cautious of models that have drawings referenced to them. Below are the details that are worth knowing before you get yourself knee-deep in dangling dimensions.

The “Fine Print” on SOLIDWORKS Convert to Bodies

Be aware that the use of SOLIDWORKS Convert to Bodies can have an impact on dimensions that appear in related drawings during the process of discarding the feature data from your model. The behavior will differ, depending on how the dimensions were created on the drawing. If the “Model Items” tool was used to import the dimensions directly from the model, they will become a set of dangling dimensions you see in the image below.

Linked Dimension Blown Apart

Linked Dimension Blown Apart

If the smart dimensions tool was used to create reference dimensions within the drawing, the dimensions on the drawing will remain unaffected.

The checkbox that Saves the Day!

If model dimensions are present on the drawing, a mess of dangling dimensions can be avoided completely. This is done by selecting the checkbox that will preserve your reference geometry and sketches during the conversion of the part to a featureless model.

SOLIDWORKS Convert to bodies preserve reference geometry and sketches option

Preserve reference geometry and sketches option

SOLIDWORKS will prompt you to save the converted model with a new filename in an effort to preserve the original.

During the “Save As” process the related drawing will have the model swapped out for the newly created featureless version. The proper result being that the dimensions on the drawing are not disturbed by the conversion (image below).

Back to the original “dimension”

The super nifty feature of this entire workflow is that you can re-establish the link between the original (Non converted) model and the drawing with ease. Simply use the open dialog to modify the part model that the drawing views are referenced to and the dimensions will  “magically” find their original referenced features – this makes the process reversible and reduces the changes of stale annotation data on your drawings if you choose to use the “Convert to Bodies” option.

Linked dimensions reestablished

Linked dimensions reestablished

SOLIDWORKS 2017 Resources

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SOLIDWORKS 2017 Resources

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Chris Briand, CSWE

Chris has been educating and supporting Engineers, Designers and IT Personnel within the 3D CAD industry since 2002, and was adopted into the fantastic team of applications experts here at Javelin Technologies in early 2006 and migrated along with his team members to the TriMech Solutions team in 2021.  Chris enjoys the continuous learning driven by the ingenuity and challenges Designers bring forward. Innovation using 3D Printing, 3D CAD and other technologies, combined with a diverse background as a technologist, allows Chris to find solutions that accelerate Designers, and take Design Teams to new heights. Chris is currently being held at an undisclosed location, near Halifax, Nova Scotia, Canada.