SOLIDWORKS MBD 2019: Security, Sheet Metal Support, and Copy Scheme

SOLIDWORKS Model Based Definition (MBD) 2019 introduces additional security settings for exported 3D PDF’s to protect intellectual property. MBD 2019 also now supports sheet metal parts and annotations such as bend notes and bend tables. Additional flexibility is given to the end user in the ability to copy DimXpert schemes across configurations and documents.


Increased Security 

Collaborating with 3D PDF’s allows the recipient to be able to view and interrogate Product Manufacturing Information (PMI) in 3D space. SOLIDWORKS MBD 2019 provides additional security settings to make sure that only necessary information is sent to the recipient.

3D PDF content can now be published using ‘Only Graphical Data’ instead of BREP data. This setting is found under the ‘Accuracy’ section of the ‘Publish to 3D PDF’ property manager.

BREP data contains enough information to be able to reverse engineer or manufacture the part. Using only graphical data will reduce the internal information of the product to help protect intellectual property.

Additional PDF security settings can also be set directly within the MBD ‘Publish to 3D PDF’ property manager by clicking on the ‘3D PDF Security Settings’ button.

A window will launch where PDF Security Settings can be set. The security settings that can be controlled include the ability to disable printing, copying, or editing the published PDF. Passwords can also be added so that the published PDF will not open without the password being inserted.


Support for Sheet Metal Parts

SOLIDWORKS MBD 2019 now supports sheet metal parts and annotations when creating 3D Views. Specific sheet metal annotations such as Bend Notes, Bend Lines, Bounding Box, and Bend Tables can be created in the flat pattern of the 3D model.


Inserting Bend Notes

Bend Notes and the Bounding Box will be applied and maintained in the Flat Pattern of the sheet metal part.

  1. Click on ‘Flatten’ from the Sheet Metal tab in the Command Manager or unsuppress the Flat Pattern from the feature tree.
  2. Right-click on the ‘Flat-Pattern#’ folder in the feature tree.
  3. Choose ‘Insert Bend Notes.’

The result is that Bend Lines and Bounding Box lines are automatically inserted into the flattened sheet metal part. Also included are the bend angles and directions in order to manufacture the part.

Bend Lines and the Bounding Box will be color-coded for easy viewing. Colors can be customized through the sheet metal MBD settings found the Document Properties:

Tools > Options > Document Properties > Sheet Metal MBD


Inserting Bend Tables

A Bend Table can be applied to the Flat Pattern of the sheet metal part.

  1. Click on ‘Flatten’ from the Sheet Metal tab in the Command Manager or unsuppress the Flat Pattern from the feature tree.
  2. Click on ‘Insert’ from the main menu at the top of the SOLIDWORKS user interface.
  3. Choose ‘Tables’
  4. Choose ‘Bend Table’

The result is that Bend Lines, Bounding Box Lines, a Bend Table, and associated bend Tags will be inserted into the Flat Pattern. The Tags will appear in the Bend Table along with the bend direction, bend angle, and the inner radius. The corresponding tags will also appear next to the respective bend lines on the Flat Pattern itself.


Capturing Bend Information in a 3D View

Once the bend notes and information have been added to the sheet metal Flat Pattern, this information can be captured in a 3D View for publishing to eDrawings or a 3D PDF.

The ‘Capture 3D View’ Property Manager will pull in the ‘Default <Flat-Pattern>’ configuration to capture the Flat Pattern, Bend Information, Zoom, Orientation, and any customizations added to the view.

The final 3D View will be placed in the ‘3D Views’ tab on the bottom of the SOLIDWORKS screen. This allows for future editing and easy access to this information in both SOLIDWORKS and the published formats.


Copying and Importing DimXpert Schemes

SOLIDWORKS MBD 2019 reduces work duplication by being able to utilize existing dimensions schemes for other parts and configurations. Specific ‘Copy Scheme’ and ‘Import Scheme’ buttons are in the 2019 MBD Command Manager.


Copying DimXpert Scheme to a Different Configuration

When a part file has multiple configurations, the DimXpert scheme from one configuration can be copied to other configurations in the part. This is ideal for configurations which have very similar geometry. Work and customizations can be created once and reutilized with minimum editing required.

To Copy the DimXpert Scheme:

  1. Create the DimXpert scheme in one configuration.
  2. Double-click to activate the Configuration that you want the scheme to be copied to. This configuration cannot have an existing DimXpert Scheme.
  3. Choose ‘Copy Scheme.’
  4. In the Property Manager you can now add the Scheme Name, Description, Comments, and specify the ‘Source Configuration’ where the DimXpert Scheme resides.
  5. Click ‘OK’ to finish the copy.


Import DimXpert Scheme 

DimXpert Schemes can be imported from one part file to another using the ‘Import Scheme’ in the MBD Command Manager.

  1. Open the file that you want to add your DimXpert Scheme to.
  2. Click ‘Import Scheme.’
  3. Browse to the part file that contains your original DimXpert scheme.
  4. Choose the source Configuration that contains the DimXpert scheme.
  5. Click ‘Open’.

The originating DimXpert scheme will now be added to your part file.

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