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

Parents
  • oldmouldy
    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.

  • anowack
    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?

  • oldmouldy
    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.

  • DH202512105348
    0 in reply to oldmouldy

    If you do connect a power pin to a net, does that net get shorted to the net with the same name as the power pin?  For example. If I have a part with power-pin named 'GND', and I connect it to a net called 'AGND', will the 'AGND' and 'GND' nets be shorted, or does that only happen if a power pin is left un-connected?

  • oldmouldy
    0 in reply to DH202512105348

    No, "deliberate" wire connections win over unconnected Power Pins.

Reply
  • oldmouldy
    0 in reply to DH202512105348

    No, "deliberate" wire connections win over unconnected Power Pins.

Children
No 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.