Home
  • Products
  • Solutions
  • Support
  • Company
  • Products
  • Solutions
  • Support
  • Company
Community Blogs System, PCB, & Package Design (System Analysis… BoardSurfers: Managing Silkscreen Data Using Allegro 3D…

Author

anandd
anandd

Community Member

Blog Activity
Options
  • Subscriptions

    Never miss a story from System, PCB, & Package Design (System Analysis: EMI/EMC/ET, PCB) . Subscribe for in-depth analysis and articles.

    Subscribe by email
  • More
  • Cancel
17.4
BoardSurfers
3D Canvas
17.4-2019
Allegro PCB Editor
silkscreen
Allegro

BoardSurfers: Managing Silkscreen Data Using Allegro 3D Canvas

24 Aug 2022 • 3 minute read

 The silkscreen layer plays a crucial role in the assembly, repair, and testing of a PCB. You can add a variety of information to this layer, such as the location of the components, polarity, component orientation, on-off switches, LEDs, and testpoints.

During the silkscreen cleanup process, we tend to assume that all the components are placed correctly, and just moving the reference designators away from the components is sufficient to clear any overlaps. But in the real world, that may not be the case. After component assembly, the silkscreens may be blocked by the components, and reference designators may be partially visible to the end user. You can see this conflict in the following illustration:

In this post, we’ll see how to utilize Allegro 3D Canvas to place and update data on silkscreen layers judiciously.

Reviewing and Updating Silkscreen Data in Allegro 3D Canvas

To counteract unintentional hiding of the silkscreen data, use Allegro 3D canvas during silkscreen cleanups. Allegro 3D Canvas lets you update the silkscreen layers interactively when you modify a 2D design. To manage silkscreen data using 3D Canvas, follow these steps:

 1.    To open 3D Canvas, type 3D in the Command window or choose View – 3D Canvas from the Allegro® PCB Editor menu.

         invoke 3D canvas from Allegro

2.    In the 3D Canvas Filter dialog box, select options to display autosilk or package/board geometry silkscreens, as required.

3.     Select other objects in the filter as shown in the following image and click OK:

          Allegro 3D Canvas filter options

After the design is loaded, the Allegro 3D Canvas window opens.

4.    In the 3D canvas window, choose Setup – Preferences and change the following settings:

i. To enable the interactivity between 2D and 3D designs, choose  Setup – Preferences.

ii. Under the Interactive category, select the Enable 2D / 3D Interactives option.

               Allegro 3D Canvas interactivity settings

iii. Under the Appearance – Projection category, select the Orthographic option.

              Allegro 3D Canvas projection settings

iv.  Select the Symbol Representation category and choose The STEP Model, if available, or else the Boundary Shape.

v.  Set the Boundary Shape Source to Place Bound.

               Allegro 3D Canvas symbol representation selection

vi.  Click OK to apply these settings and close the Allegro 3D Canvas Preferences dialog box.

5.    Adjust the camera view in Allegro 3D Canvas so that it displays the Top view of the design in 3D.

6.    Place Allegro PCB Editor and Allegro 3D Canvas windows side by side as shown in the following image:

       Updating silkscreen in allegro and 3D canvas

 7.    Move a reference designator in the silkscreen layer in the 2D canvas of Allegro PCB Editor.

       The relevant text in silkscreen gets updated in 3D Canvas instantly.

The following animation shows how to adjust the placement of silkscreen data in 2D while reviewing the manufactured output in 3D Canvas. 

silkscreen update in Allegro 2D and 3D video

Conclusion

You can leverage Allegro 3D Canvas capabilities of visualizing the manufactured design to improve silkscreen data and ensure that the required information is available with the final product.

 To learn in detail about the features of Allegro 3D Canvas, watch training bytes related to Allegro 3D Canvas in Allegro PCB Editor Basic Techniques (Video Channel) on the Cadence Support portal.


You can also enroll in online training courses and become Cadence Certified by grabbing free Digital Badges. 

Contact Us

For any feedback or any topic you want included in our blogs, write to us at pcbbloggers@cadence.com.

Do SUBSCRIBE to stay updated about upcoming blogs.

About BoardSurfers

The BoardSurfers series provides solutions to the various tasks related to the creation and management of PCB design using the Allegro platform products. The name and logo of this series are designed to resonate with the vision of making the design and manufacturing tasks enjoyable, just like surfing the waves. Regular, new blog posts by experts cover every aspect of the PCB design process, such as library management, schematic design, constraint management, stackup design, placement, routing, artwork, verification, and much more.


© 2023 Cadence Design Systems, Inc. All Rights Reserved.

  • Terms of Use
  • Privacy
  • Cookie Policy
  • US Trademarks
  • Do Not Sell or Share My Personal Information