Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

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

Status
Not open for further replies.
T

The_Dutchman

Member level 1
Member level 1
Joined
Feb 12, 2008
Messages
37
Helped
0
Reputation
0
Reaction score
1
Trophy points
1,286
Activity points
1,704
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?

altiumratsnest.jpg

Thanks already
 

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

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

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
 

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.
 
luben111 said:
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.
Click to expand...

Thanks!!! It was very useful!!!
 

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.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top