Multiple Ref Des text on a footprint

[Iccor_56]

regarding:

Multiple Silkscreen Refs for Footprint

Hi, I am working on a project that uses a through hole connector which can be populated on either side of a PCB, depending on the application. To this end I’m trying to design a connector footprint that has the connector outline, component reference, and component value on both sides of the board. However, when I copy and paste the REF** and the component value silkscreen text in the footprint editor, it shows up on the board as silkscreen reading REF** and the generic name of the component resp…

i also have this issue. on min i have a switch but i want the reference desgination on the back side as well as the frontbecause that is the side it will be trouble shot from. is there any way to have the same reference duplicated to multiple positions in a footprint file?

[jmk]

The only way I have found is a bit messy. Others may have found an easier way.

Open “Footprint Properties”, create more lines with the + button, fill in the text and select BSilk.

When this is done, highlight each text, in turn, in the Footprint Text Properties and Reverse with the Reverse button.

[bertrand_meneroud]

Rather than the ref, you can display a text variable.
And then you can has many copy of the text as you want in the footprint

and in your footprint, you can add a text label using this variable

Here I display it on both top and bottom silkscreen

[Iccor_56]

thank you.

really strange it does not work when you put them directly in the footprint file.
I hope they fix that

[bertrand_meneroud]

I think that you can use the variable ${REFERENCE} to place multiples text object with the reference in the footprint.
In my case, I wanted to display an actual name and not the reference, so I’ve created a new variable.
the Ref*** is coming from previous version and it seems that you can have only one copy of it in the footprint

[jmk]

@bertrand_meneroud

and it seems that you can have only one copy of it in the footprint

I did some more exploring

It turns out you can have more than one copy of the Ref in the footprint. The Ref may be hiding in a pad if that pad is also the anchor for the footprint.

Also, the second stage (Footprint Text Properties) I posted above is superfluous if the layer is changed to B.Silk. in the Footprint Properties. The text is automatically reversed if the B.Silk is selected.

My problem was I didn’t change the Layer in the Properties, so I had to make the changes in the Text Properties.

[eelik]

@bertrand_meneroud

I think that you can use the variable ${REFERENCE} to place multiples text object with the reference in the footprint.

That’s the right way to do it, there’s nothing complicated. ${REFERENCE} is a built-in variable, containing the reference designator of the footprint, coming usually from the corresponding symbol. There’s another for ${VALUE}, and in general you can use any field name from the corresponding symbol (see PCB Editor | 7.0 | English | Documentation | KiCad).