Stats

More Content

Total Etch Length Matching

SLSCORP

How to set up constraint for this kind of etch length matching. Currently, it is very difficult process as we calculate it individually and sum it to match the total length. If a board is having multiple this kind of nets and more number of components in series then the length matching consumes too much time. What is the best method to do this kind of length matching?

Parents
  • oldmouldy
    0

    This is what PCB Editor calls an XNet, eXtended Net. In any PCB Editor product, you can create XNets by assigning Signal Models to components with the Discrete Class property value through the Setup>More>SI Design Setup. (Setup>SI Design Setup with the legacy menus) Two pin components with the Discrete Class property value can be automatically assigned signal models based on Value. Components can also be moved between Classes during the setup to get them into the correct Class for SI. Once the setup is complete, the Constraint Manager will then list the "combined" Nets as XNets and Constraints can be applied to the entire XNet.

Reply
  • oldmouldy
    0

    This is what PCB Editor calls an XNet, eXtended Net. In any PCB Editor product, you can create XNets by assigning Signal Models to components with the Discrete Class property value through the Setup>More>SI Design Setup. (Setup>SI Design Setup with the legacy menus) Two pin components with the Discrete Class property value can be automatically assigned signal models based on Value. Components can also be moved between Classes during the setup to get them into the correct Class for SI. Once the setup is complete, the Constraint Manager will then list the "combined" Nets as XNets and Constraints can be applied to the entire XNet.

Children
  • SLSCORP
    0 in reply to oldmouldy

    Thanks for the reply...

    We tried to create xnets with the steps shown in below images but were unable to create. Created a simple schematic to test. Can you please help what steps we are missing?

  • JuanCR
    0 in reply to SLSCORP

    Open your Constraint Manager (Setup > Constraints > Constraint Manager ...). Then go to Tools > Options and make sure that you have this option set up like this: 

    If you have it setup like this, you should see the Xnets automatically appear in your Electrical Worksheet.

  • SLSCORP
    0 in reply to JuanCR

    Thanks for your reply. We successfully created XNet with 2 pin discrete components. Is there any method to include IC's in the XNet?

  • Schulz Jordan
    0 in reply to SLSCORP

    The discretes can only be considered for XNets not ICs.

  • steve
    0 in reply to SLSCORP

    There is a solution on the Cadence Online Support site that may help:- How to create Xnets through ICs (cadence.com)

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.