Capture CIS netlist error to PCB Editor 

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

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

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

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.

Thanks Steve!

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.

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.....)

 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

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. 

 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