Altium: How to use pins that are internally connected in the component

[The_Dutchman]

Hello,

In some components, for example a simple push button, 2 pads are internally connected to each other.
So I gave the pads the same designator, but when I connect one pad, altium still draws the ratsnest to connect the other pad.
How can I fix this?



Thanks already

 

[zula]

if its internally connected. you dont need to connect it on the pcb. so you can set the designator as a '0' or 'x' whatever.

 

[The_Dutchman]

Yes, but than I can't choose wich one I would like to connect to without pin swapping.

 

[zula]

as i know, there is no way to do this without pin swapping. You have to use pin swapping options.

 

[Anonymous_Ricky]

As these pins are connected in component internally you can also connect them in pcb as it will not effect the working of component also it will avoid your confusion and will not show in unconnected net report

 

[luben111]

it's easy
If you open the component into the PCBLib library and if you click on the pins you'll see a property called Jumper ID. If you set several pins to same jumper ID (non zero value) they will be considered as short circuit and Altium will not complain if you connect same net to different pins.

 

[zula]

thank you, i like it

 

[pablodecker]

it's easy
If you open the component into the PCBLib library and if you click on the pins you'll see a property called Jumper ID. If you set several pins to same jumper ID (non zero value) they will be considered as short circuit and Altium will not complain if you connect same net to different pins.

Thanks!!! It was very useful!!!

 

[TA37]

just make sure if there are any current requirements on the net, that you don't accidentally let current go in pin-1 and out pin-2 in excess of the part's capacity. Since the tool will let you route half your net to pin-1 and the other half to pin-2 and consider it fully routed through the 'jumper'. Or DNI the part in a design variant only to find out you've split your net in twain.