SOLIDWORKS® Support Monthly News – April 2024

Hello to all,

Welcome to the new edition of the SOLIDWORKS® Support Monthly News! This monthly news blog is co-authored by members of the SOLIDWORKS® Technical Support teams worldwide. Here is the list of topics covered in this month’s Blog :

  1. Adding watermark on the Drawing Sheet: Approach -1

  2. Sheet Metal: Controlling the ‘Bend Radius’ of an imported solid body already in folded state

1. Adding watermark on the Drawing Sheet: Approach -1

-by Tushar NAYAK

We all have seen many companies across the globe putting their logos, names and words like “CONFIDENTIAL”, “DO NOT COPY” or “PRELIMINARY” etc. as watermarks on the technical drawings, as can be seen in below image.

There is more than one way to add such watermarks on SOLIDWORKS Drawings. These can be added to drawing sheet s and saved as Drawing Templates for future use. This blog explains Approach No.1 of adding watermarks to SOLIDWORKS Drawings.

Often, watermark is a word that is behind the contents on the drawing sheet i.e. the views, annotations, notes etc. If you simply add a word as a watermark using Notes and place a drawing view over it, the note superimposes the drawing view – this is not what the watermark is supposed to be like. The note has to be ‘Behind the drawing view’. For this, the most observed and common step is to add watermark notes on the Sheet Format instead of on the sheet. A general assumption after doing this is that the watermark notes will fall behind the drawing views because it’s a common belief that everything that is on the Sheet Format will always fall behind the sheet contents. However, this is not the case! The watermark notes will still superimpose drawing views and other sheet contents as the image below shows.

To make the watermark notes fall behind the sheet content, these steps can be followed.

  1. Right click on the blank area of the sheet and click on ‘Edit Sheet Format’.
  2. Insert the note with required font, font size, colour and orientation.
  3. Select the note to open its Property Manager.
  4. From the ‘Text Format’ section, select ‘Behind Sheet’ and click OK.
  5. Right click on the blank area again and click on ‘Edit Sheet’. This brings us to the sheet edit mode.

Adding drawing views or any other content on the sheet will now superimpose the watermark note(s). After performing above steps, the Sheet Format and Drawing Template can be saved as new files that can be used in future. The images added to the Sheet Format as watermarks do not need specific setting to be turned on as they by default fall behind the drawing views.

We will see another approach of adding a watermark to drawings in the next blog!

2. Sheet Metal: Controlling the ‘Bend Radius’ of an imported solid body already in folded state

-by Vinod KALE

‘Bend Radius’ of an imported feature can be controlled using:

  1. FeatureWorks: With the ‘Automatic’ recognition mode and relevant sheet metal features selected, convert the imported solid body into sheet metal part (refer left-side image).Once the features are recognized, edit the ‘Edge-Flange1’ and observe you have the ‘Bend Radius’ option available to control the bend of a part in folded state (refer right-side image).
  2.  Convert to Sheet Metal: If this command is used directly on the imported part, the ‘Bend Radius’ option will be greyed out by default (shown in below image). Even though you enable ‘Override default parameters’ and try to modify the bend radius value, it will reset to its original value.To get the bend radius in editable format for an imported feature using ‘Convert To Sheet Metal’ command, refer the following steps:
    1. Delete Bend: Remove the bend portion of an imported feature using ‘Delete Face’ command.
    2. Convert To Sheet Metal: Now use this command, select the fixed face and edge that represent bend. Observe the ‘Bend Radius’ option will be available and will also allow to modify the bend radius value as required.



Akhil C

SOLIDWORKS User success Engineering Specialist at Dassault Systemes
Mechanical Engineer with overall 5 years of experience in mechanical domain - Academics and Industry. 4+ years in Technical Support of Computer Aided Design and Supporting SOLIDWORKS suite of products. Certifications: 3DEXPERIENCE® Collaborative Industry Innovator, 3DEXPERIENCE® Industry Innovator, 3DEXPERIENCE® 3D Creator