No, Please, just don’t.
Place the main body of connectors and their Courtyards always on the front when designing footprints.
You can flip the whole footprint to the backside of the PCB when designing the PCB, but in the footprint itself, just keep it on the front.
For edge type connectors you can:
Place a single pad on the top layer.
Make an array of them.
2a. (Repeat that on the other side)
Select the whole array, press [Ctrl + C], [Ctrl + V] to Copy & Paste.
Place that array in some empty area in the Footprint Editor.
Select the just pasted array (if it is not still selected).
Right mouse button and Flip.
Hover over the selection and m for move.
During the move, press r for rotate untill the orientation is correct.
Finally place them where you want.
For edge type connectors it may make some sense to have courtyard info on both front and back courtyard layers. Graphics (from courtyard of any other graphics layer, can be flipped to their “opposite” side in a similar way.
With graphics you can also easily edit their properties (make a selection, then e for edit) and then choose a layer from the drop-down list.
Flip works with about any selection, while if you want to change the layer with e for Edit, then you have to do most things one-by-one. Most selections are not directly editable.
The procedure you outlined is what I currently do but it is annoying in that you have to copy and paste away from the original before the flip and then move them back to the exact location you started with (but now on the other side).
It’s not a huge issue, I’ll survive.
Regarding pads… the edge connectors I have often the same shape on top and bottom but not electrically connected and therefore different pin numbers so the All Cu layers approach doesn’t work… e.g. A,B,C… on the top… 1,2,3 on the bottom.
It’s easy to suggest you can do this but, it’s not too easy to start from scratch and expect results in 5 minutes. I will take 10 minutes…
But, once doing it a few times, clarity of what’s going-on stands out and success quickly arrives. Then, imagination takes over and you’ll think you’re an expert!
Example below shows moving objects to/from different Layers, including Tracks and changing their widths. Many things are possible…
I did not bother to add code to Move and also leave original in place (meaning, did not copy and paste, I just moved them because that’s what I use/want. But, you can gimmie up code to do both Copy & Paste)
It occurred to me that I forgot you’re most interested in Courtyard’s…
There is no plugin feature in the Footprint editor but, the demo I posted does move them after placing footprint in PCB.
Note: Because the PCB file is just a Text file, you can edit the layer names and/or write a program (in Java, Python… etc) to Parse the file and change layers… Not difficult but, not simple for non-programmer’s
However, you can change the Layers in footprint editor by Double-Clicking and setting to desired layer - vid below shows:
Shape made in F.CrtYd, copied&pasted in same layer, then, changed shape lines to B.CrtYd
This post triggered some memories of an edge connector I made quite some time (2 to 3 years) ago.
I manually had to renumber most of the pads. It was not such a biggie because I only did it once. If you do it more often however, a better approach is to draw a one dimensional array of pads. (One for top, One for bottom).
I was a bit confused of how this worked exactly, and therefore started this thread because I expected a bug (but was not sure).
However, after Rene pointed out the entry boxes I glanced over and used them, it all worked as expected.
Also, when designing new footprints from scratch, I find it helps if you start by making some sketches on good old dead tree carcasses, and then punch in some numbers for important coordinates.
If you have some coordinates, you can simply put those in the X and Y coordinates of a pad instead of lining them up visually.
Or make good use of the grid. Use a grid that is relatively coarse when placing pads in the footprint. If you visually line up footprints on a coarse grid, then either coordinates are perfect, or the mismatch is so big that you can clearly see it.
It is always recommended to create footprints considering that the components are mounted on the top layer. So, initially, you can create a footprint for the top layer. Once the footprint is imported to the board file, then select the component, right-click and choose the option “flip” (shown in the below image). This shifts all copper layers of the footprint to the bottom layer automatically.