Re: gEDA-user: Warning: All of the pads are on the opposite side?

[bumpelo <bumpelo@xxxxxxxxxxx>]

Bob Paddock wrote:

> On Sunday 24 July 2005 11:20 am, bumpelo wrote:
>
>  
>
> > Here's probably how you want to fix this:
> > Go to File->Preferences->Layers under the "setup" tab change the
> > checkboxes so that Group 1 which contains the layer named "component" is
> > on the component side and group 2 is on the solder side.
> >    
>
> I just discovered that by doing that, it now becomes impossible to 'name' a 
> pad, to give it a pin number, as you can not get it selected.
>
>
>  
First off, I put a patch in CVS but it won't help any existing 
installation because the bad layer groups were automagically saved in a 
local .pcb/preferences file for all existing installations. Once you 
change the layer grouping you must check the "use as default" option to 
fix the preferences file.

Now, my description was how to prevent the "those pads are on the wrong 
side" message when creating elements in the first place. If you have 
created the element already with the pads on the opposite side from the 
silkscreen, you must fix the element itself. Break the element to pieces 
then move the tracks to the correct side. Do that by making the correct 
side the active drawing side then using the "m" key to move each track. 
Then convert to an element again.

In order to understand what is going on, you need to understand that the 
layer grouping only influences elements *at the time of creation*. If 
you change the grouping after an element exists, it will not affect the 
element, only all of the other copper. What you originally did was to 
create an element that physically resided on the component layer 
(because you were viewing the component side) but that had pads on the 
solder (opposite) side of the board. Once the element is made this way 
it can't be undone except by smashing the element and fixing its pieces.

h.