Stats

More Content

Assign Power Pin to Power Net of Different Name

anowack

Hi there,

I've read several topics on this, and remain confused on how to address this topic.

I have several parts with different naming conventions for the power rails, some support single supply, some dual supply. Another has two different voltage supply sources. Between these parts I have power pin names of GND, VEE, VS-, VCC, VS+, VDD, VCC_2. I have global nets named +5V, +3_3V, GND, and I want to connect them to these pins as I choose. I would prefer to not alter the schematic symbol pin names, as I intend to reuse these parts in the same schematic with other instances connect to other voltage supplies.

When running the DRC I get many errors of "Warning,Electrical,WARNING(ORCAP-1589): Net has two or more aliases that might lead to a short. Ensure nets are not shorted together or nets do not have two or more aliases. This message is displayed because 'Report all net names' is set in Design Rules Check dialog.,U4,VCC VCC  +5V,SCHEMATIC1"

What is the correct way of doing this? I tried adding a POWER_GROUP property to the part instance with entry of "VDD=+3_3V" but this did not result in any changes.

Here is an example picture from my schematic, and the DRC marker from before is from the VCC pin on this part

Thank you

- Aaron

  • +1

    If you think like me I guess that you are always connecting the symbol power pins in the schematic to a wire. (Instead of leaving the pins floating, and relying on global net assigned to the pin.)

    In that case, I recommend that you modify all your schematic symbols. To change the pintype of the power and ground pins, and assign them to "PASSIVE". It should fix your problem and you wont have to face those annoying DRC warning.

  • 0 in reply to gvellet

    I think this is the simplest option to keep my schematic parts reusable. I'll go with this unless there is a feature or method, I briefly looked into using hierarchical blocks, but didn't arrive at a working solution.

    I'm still curious how people manage all these power nets, for parts that can have a variety of supply voltages. Maybe it's more common to treat a part library as a template to modify in each design?

  • 0

    This DRC is based on an uncommon practice and can be safely ignored by the vast majority of users who name Power Pins according to the Manufacturer's Datasheet and connect the required Power Net in the Schematic. Just disable the Power Ground Short check, PCB>Design Rules Check, Rules Setup, Physical Rules, uncheck “Check power ground short” and run the DRC check again.

  • 0 in reply to oldmouldy

    Ah, okay. Thanks for the insight on the history of that. As a follow up, is it still useful to mark those pins as power pins vs passive pins?

  • 0 in reply to anowack

    In OrCAD Capture Pins of Type Power cannot be unconnected, they will always connect to a Net of the same name if left unconnected. Also the ERC Matrix checks Pin Type against Pin Type and Passive Pins "defeat" the checking since "Passive to <anything>" is never a DRC as far as the default ERC Matrix is concerned. Following the datasheet Pin Types, as far as practicable, also eases checking Schematic Parts against the Manufacturer data.

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.