I have design a single side PCB on Allegro 15.7. Some times it was necessary to implement a SMD Jumper for jumping over other signals. I have place this jumpers on the schematic (design entry CIS) and connected bode pins of the jumper to the same signal.
It works, but I have a small cosmetic problem, for each jumper I placed, I get on the Layout guide (open connection).
Does some one know if there is a possibility to design a library symbol with two pins that can be automatically connected to the same potential?
Thanks in advance
Yes, this can be done. Select the part > right click > Edit Part > select the pin and change it's type to 'Power' - a power type pin is (automatically) connected to the net where in the net name is same as the (power) pin name.
Use a zero ohm resistor~Richard
Thanks for the responses, A zero ohm resistor has the same problem; each end of the component will be connected to a different net. So that it is not possible to connect both pins to the same net as example GND or so on.I will try to define the pins as power pins.Gustavo
I had tried to change the pin type to power pin. For the schematic it is clear, but on the layout I always get a ratsnet on between both pins. The result is the same as using a zero ohm resistor.Gustavo
That is a snapshot of the layout, were you can see the ratsnets. The PCB is functional routed by 100%. The big risk is the possibility to overlook really open connections.
Not sure if this will help but you can add net short property for the part pins in OrCAD Capture. The name of the property is NET_SHORT and the value is the name of the two nets separated by colon i.e. GND:AGND. Let us know if this works for you? Oh, and make sure that this property gets included in the netlist by adding the property (name) in the netprops section of allegro.cfg when generating the Allegro netlist. I think you can also add the property on to a pin in Allegro.
Thanks for the sugestion,
The NET_SHORT property is not what I need. This property works very fine if you need a star point (i.e. AGND:DGND) so it is possible to connect both signals to the same pin without DRC problem, but it dos not work with a jumper (zero ohm resistor) which both terminals are connected to the same net
Try the "No"RAT" property and see if it is what you are wanting.Best regards,Kishore
I mean "NO_RAT"
Thanks for that input, the NO_RAT function is applicable always to the entire net. Do you know if there is a possibility to use these function for a component only?
For the moment it seems to be an applicable solution before I do the post process.