Stats

  • Locked Locked
  • Replies 4
  • Subscribers 164
  • Views 20118
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Power Pin assignment in ORCAD

archive

Hi Guys,

I have a burned up board over here due to a netlist mistake.

I had created a symbol of an IC in ORCAD with vcc pins assigned as Power pins.

Now I had connected some of the  vcc pins to a power net while i left one pin disconnected.

I was using two refdes of this symbol in my schematic page : U1 and U2.

ORCAD has generated a net by the name VCC and connected the two left out pins on U1 and U2.

Can anyone tell me how to avoid this problem?

I though of some solutions as below, but they have problems:

1- I tried to add NC symbol on these pins, but it does not apply to power pins, atlease thats what i think.

2- Next, I made the disconnected pins as Passive, this solved my problem. But now the problem is that, the symbol is usually made by some other designer while schematic hookup is done by another. T

he symbol creater usually attached Power pin attribute to all pins which are related to power supply, etc. Shall the power pin information be communicated between the two designers?

So any ideas / solutions??? How are other guys avoiding this problem?

Hassan




Originally posted in cdnusers.org by hshahzad

  • Hi Hassan,

    Is this unconnected power pin an intentional unconnect where you do not want a net applied ?

    you can check this pre-layout :
    In Capture's DRC there is an option to report "visible unconnected power pins"

    If you edit the schematic symbol in Captures Part Editor and goto :
    > View Package
    > Edit Properties

    you will see a column called "ignore"
    flag this power pin as ignore and it will be ignored.


    Originally posted in cdnusers.org by rbennett

  • Hi Hassan,

    Power pins are global in nature, that is, a power pin is connected to a net where in the net name is same as power pin name, even if power pins are left unconnected.

    Have the schematic designer follow these steps to not have power pins connect to net(s):

    1. Place the part in the schematic
    2. Right click > Edit Part
    3. Go to View > Package
    4. Edit > Properties
    5. In Package Properties window check ignore box for the desired pins
    6. Click on OK button
    7. Close Part Editor
    8. Select Update Current or Update All

    Varun


    Originally posted in cdnusers.org by khurana

  • Thanks for solutions......

    I tried flagging the power pin as ignore. It makes the power pin invisible........ is there a way to ignore the pin and keeping it visible...........???

    Anyways the DRC report on "visible unconnected power pins" is usefull.


    Originally posted in cdnusers.org by hshahzad

  • I don't think so.. you will have to graphically draw a dummy pin with Capture if you want to see this on the schematic.


    Originally posted in cdnusers.org by rbennett
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.