Is there a way to prevent the netlister from removing parts in the schematic with no pins? We create parts in our schematics that represent the PCB board part number in the BOM and have text in the PCB for symbolization. Is there a configuration to prevent the ALG0060 warning and resultant removal of the part from the Allegro?
Try with the part fixed in Allegro then import netlist. Make sure that Ignore Fixed Property is not checked.
In reply to Khurana:
I am not sure exactly what you are saying. I thought the Fixed Property was in Allegro PCB. I am talking about generating the schematic in Allegro Design and then creating the PCB netlist.
I guess I could instantiate the schematic symbol in Design and load the footprint manually in PCB, but that defeats the purpose.
In reply to mvonahnen:
OK. What are you using for schematic (OrCAD Capture or Allegro Design Entry HDL)? And, what version of the tools are you using? So, you are adding a zero pin part in the schematic? And, you want that part to be included into the netlist for Allegro?
I am using Allegro Design Entry CIS.
The version is SPD 16.01.
I have created a schematic symbol that has no pins and only text to be added to the schematic.
I have created a "Footprint" that contains text on the Top Etch layer and text and shapes on the Top Silkscreen layer.
I would like to have the netlister load the footprint in the PCB when it is instantiated in the schematic, just like other components.
Hmm...the only way I can think of is to use NC pins property to this bogus part - this is required for the part to be "placeable" in Allegro. Otherwise, even if a mechanical part sucessfully made it into the netlist, then Allegro PCB Editor would not allow you to place it since the part is mechanical (i.e. has no pins). The drawback by adding NC pin is that when you run drc then it will say that one is unconnected.
Call Cadence and create an enhancement request.
mvonahnenThis works, but I noticed that this does not work if the pin is a power pin. I could see cases (like mounting holes) where a single power pin device would be desired on a PCB.
Recall that electrical connections such as mounting holes need to appear in the schematic and be attached to a net. We do this all the time for mounting holes -- no issues. Don't use a NC pin for those components.
A non-electrical mounting hole is a different story. You really can't fool Allegro because it'll want the part to be in the netlist but it technically is not in the netlist. Can it be done? See the above poster's comments. It should be a part of the board symbol however....
A serial number label can be brought in as a dummy part but you need to build it like an electrical part to get it go into the netlist. You can turn visibility of pins off to make it appear as if it's not connected. Be sure to X out the pin so the Capture DRC check does not squawk.