Home > Community > Forums > PCB Design > Capture CIS netlist error to PCB Editor

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Capture CIS netlist error to PCB Editor 

Last post Wed, Mar 24 2010 3:40 AM by otto9otto. 9 replies.
Started by SharonPaige 17 Jun 2009 04:35 PM. Topic has 9 replies and 8608 views
Page 1 of 1 (10 items)
Sort Posts:
  • Wed, Jun 17 2009 4:35 PM

    Capture CIS netlist error to PCB Editor Reply

    My schematic has a part U12 with duplicate pin names like GND on pins 2 and 4.  When trying to create an Allegro PCB Editor netlist, I get an error message "Duplicate Pin Name "GND" found on Package LT3009_2, U12 Pin number 2: .....Please renumber one of these.  I have done this in many previous schematics and can netlist fine into OrCAD Layout but the netlist into PCB Editor aborts and says to please correct the above error and retry.  Is this duplicate pin name situation not allowed in Allegro? We are new to Allegro...

     Thanks,

    Sharon

    • Post Points: 20
  • Wed, Jun 17 2009 8:47 PM

    • Prasanna
    • Top 100 Contributor
    • Joined on Thu, Oct 16 2008
    • Bangalore, Karnataka
    • Posts 71
    • Points 1,705
    Re: Capture CIS netlist error to PCB Editor Reply

    Sharon,

    Yes, this is not allowed in allegro.  If duplicate pin is creating the problem then change the name of the pins like  GND1, GND2 for remaining ground pins, it works without any error. Ans also keep in mind that all pins ahould be numbered properly.

    Hope this helps....

     Thanks,

    Prasanna Hegde

    • Post Points: 20
  • Thu, Jun 18 2009 12:11 PM

    Re: Capture CIS netlist error to PCB Editor Reply

    Prasanna,

    Thanks for your reply.  Funny thing, Capture allowed duplicate power names in the same schematic.  I changed the ground names and all was well.

     -Sharon

    • Post Points: 20
  • Fri, Jun 19 2009 1:45 AM

    • steve
    • Top 10 Contributor
    • Joined on Fri, Jul 18 2008
    • Woking, Surrey
    • Posts 1,199
    • Points 19,530
    Re: Capture CIS netlist error to PCB Editor Reply

    If the pin type is power then capture will allow duplicate pin names. If it is not then you will get the duplicate pin names error.

    • Post Points: 35
  • Fri, Jun 19 2009 10:19 AM

    Re: Capture CIS netlist error to PCB Editor Reply

    Thanks Steve!

    • Post Points: 5
  • Wed, Jun 24 2009 5:50 AM

    • John Davies
    • Top 150 Contributor
    • Joined on Tue, Aug 12 2008
    • Glasgow, Strathclyde
    • Posts 45
    • Points 810
    Re: Capture CIS netlist error to PCB Editor Reply

    steve:

    If the pin type is power then capture will allow duplicate pin names. If it is not then you will get the duplicate pin names error.

     

    That's interesting. I had to rename several unconnected pins on a header recently so that their names were not all NC but presumably could have avoided that if I had redefined them as power pins. Would that have any undesirable side-effects? Or would the NC property be better? I don't want to hide the pins.

    • Post Points: 20
  • Wed, Jun 24 2009 6:55 AM

    • steve
    • Top 10 Contributor
    • Joined on Fri, Jul 18 2008
    • Woking, Surrey
    • Posts 1,199
    • Points 19,530
    Re: Capture CIS netlist error to PCB Editor Reply

    If you use the POWER pin type and have mutliple pins called NC then Capture will join all these pins together with a power net called NC. The Power pin type is used specifically for POWER nets. It saves you wiring these up on the schematic. Most people use this type for VCC, GND etc. Have a look at Capture User Guide Chapter 14 for everything you needed to know (but were afraid to ask.....)

     

    • Post Points: 35
  • Tue, Mar 23 2010 9:42 AM

    • otto9otto
    • Not Ranked
    • Joined on Tue, Mar 23 2010
    • Posts 2
    • Points 10
    Re: Capture CIS netlist error to PCB Editor Reply

     I had a need for a dual op-amp, the usual dual 8-pin SOIC type, the usual pinout... So I selected the 1458 op-amp graphic and simply renamed it. Now, trying to netlist, I get the error of "duplicate pin 4" which is GND of type POWER. So it seems that I am following the suggestion above, but still have this error. Any suggestions?

     

    Otto

    Filed under:
    • Post Points: 5
  • Tue, Mar 23 2010 10:21 AM

    • redwire
    • Top 10 Contributor
    • Joined on Thu, Jul 17 2008
    • Allen, TX
    • Posts 876
    • Points 13,500
    Re: Capture CIS netlist error to PCB Editor Reply

     

    steve:

    If you use the POWER pin type and have mutliple pins called NC then Capture will join all these pins together with a power net called NC. The Power pin type is used specifically for POWER nets. It saves you wiring these up on the schematic. Most people use this type for VCC, GND etc. Have a look at Capture User Guide Chapter 14 for everything you needed to know (but were afraid to ask.....)

     

     

    Not sure that's the standard way to do this.  Allegro/Cadence has had a great way of handling NC pins for years and have implemented a more straightforward solution in OrCAD and Concept. The NC property can be added to the symbol to indentify which pins are truly NC.  In OrCAD you can choose to show these pins or keep the NC property hidden.


    Changing them to NC as POWER is not suggested but it is possible to do. 

     Have a look at the user guide for NC pins. :)
    • Post Points: 20
  • Wed, Mar 24 2010 3:40 AM

    • otto9otto
    • Not Ranked
    • Joined on Tue, Mar 23 2010
    • Posts 2
    • Points 10
    Re: Capture CIS netlist error to PCB Editor Reply

     Not being able to find much in the user manual, and being pressed for time, I have resorted to creating an 8-pin part with op-amp graphic inside the part body. No more "duplicated" GND and power pins. Thanks for your help, though.

     

    Otto

    • Post Points: 5
Page 1 of 1 (10 items)
Sort Posts:
Started by SharonPaige at 17 Jun 2009 04:35 PM. Topic has 9 replies.