FEDEVEL
Platform forum

grosfaignan , 10-25-2019, 07:37 AM

hi there,

i try to draw an USB C edge connector but i'm not able to assign both side pad to pin symbol's. i tried this method : https://www.eevblog.com/forum/altium...multiple-pads/
but it don't works, and return some various error even if i follow documentation : (https://www.altium.com/documentation...-components-ad)

so i want to make an USB C edge card connector, and thinked to create usb footprint pad only on one side (probably on top)to find other possibilities to do to clear properly this issue and solve multiple pad assignation problem.

so i would like to know your opinion and practices about that. could you help me.

i you can i would also know standard best practices about USB edge connector creation.

thanks

Anatoliy , 10-27-2019, 01:26 AM

I use two methods for those kinds of things-
-place pins on top of each other and hide numbers;
-spread the pins on the schematic symbol

could you please attach the errors you are getting? and perhaps upload the component for me to look at?

grosfaignan , 10-28-2019, 06:58 AM

hello

i placed pad on top and bottom with the same number but finally dont set jumper number... because it seems to be useless.

in releasing operation there is as number as pad "duplicad pad" error number (so 12 ... of course).

screenshot in attachments.

How do you spread pins ?

Anatoliy , 10-28-2019, 07:37 AM

I personally do not use the jumper option.
do you have a unique designator for each pad in your footprint' and a matching designator in your schematic component?

grosfaignan , 10-28-2019, 07:44 AM

nope

i have both of pad in my footprint (1 per side) called 1...12
i i don't know how matching designator in schematic component (because i have only 12 pin in my schematic and 2 pad per pin)

Anatoliy , 10-28-2019, 09:07 AM

well, first of all, a usb c connection has 24 pins' even if they are mirrored.
every pad and every pin should have a unique designator, and they need to match for altium to connect nets from schematic to pcb.
i have added a quick example-

here you can see, that pads on top and bottom are different;
and every pad has a matching pin.
hope this helps

grosfaignan , 10-28-2019, 09:17 AM

yes i now that but i hoped there is a technic to connect 2 pad to 1 pin, (i would like to use a 12 pin symbol)

Anatoliy , 10-28-2019, 09:38 AM

yes there is, sort of, here:

what you need to do, is take half the pins, hide their names and position them directly beneath each other.
then, you will see that net junction dot appear when connecting it all in schematic, this means that you have several pins connected to that same spot.
and just like that, you have a 24 pin component showcased in a 12 pin schematic symbol.

robertferanec , 10-28-2019, 11:21 AM

- I would highly not recommend to do that - very bad practice.

Every pad in PCB should have visible pin in schematic. It's not only clear and visible for everyone, it is easier for checking and easier for importing schematic between different CAD systems.

grosfaignan , 10-28-2019, 11:29 AM

ok thanks, i'll use a 24 pin symbol in that case

i tried to find a function to attribute pad to pin but altium don't seems to have... as like as eagle