| ID: | 3668 |
| From: | Gabriel Paubert <pa...@iram.es> |
| Date: | Sun, 12 Jan 2020 09:03:09 +0100 |
| Subject: | Re: [pcb-rnd] Connections in Netlist but don't appear in PCB-rnd |
| in-reply-to: | 3667 from ge...@igor2.repo.hu |
| replies: | 3672 from Jesse Frey <je...@gmail.com> |
Hi Igor2 and Jesse,
On Sun, Jan 12, 2020 at 06:25:00AM +0100, gedau@igor2.repo.hu wrote:
> Hello Jesse,
>
> On Sat, 11 Jan 2020, Jesse Frey wrote:
>
> >Hi, Igor2
> >I think I am getting somewhere. I was following the instructions given
> >by gsch2pcb-rnd to run the command file. I saved as lihata v6 board is
> >now a .lht file. Now when I optimize the rats nest a log window pops
> >up (I don't think it did this before) and from reading the output I
> >realized that pins 3-6 were all named pin3 (I feel dumb now). I also
> >found that another part that I was having trouble with also had an
> >incorrectly numbered pin.
>
> Don't worry, such errors happen all the time! You can use {v n} over
> padstacks or the subcircuit to make the numbers visible.
>
> >I fixed the .fp files and tried re-importing
> >the schematic (using import schematics, as you suggested) I still see
> >the same isues. How do I refresh the footprint?
>
>
> Yup, sch-import (or gsch2pcb-rnd) won't notice if you did a fix in
> the library so they do not reload footprints from the lib. They look at
> the board, and if there's a subcircuit with the given refdes and
> matching footprint attribute, they accept it's an already imported and
> placed part.
>
> There are two very easy options for force replacing from lib:
>
> 1. Just delete the subcircuits that should be re-imported, before the
> import; missing subcircuits are always read from the library so you would
> get the new version placed. Drawback: pcb-rnd won't remember where they
> were placed so you will need to place them again.
>
> 2. If you have a netlist and a board and everything placed already, and
> you know nothing changed, only the footprint in the lib, it may be cheaper
> to manually replace the footprint manually. This is done by opening the
> library window (key: {w n}),
surely you mean {w l}
> selecting the footprint and placing it over
> the original subcircuit on the board while pressing the shift key. This
> will replace the old subcircuit with the one you just loaded from the
> library, copying all attributes from the old one (so you won't lose
> refdes). If you do this by clicking at the origin of the subcircuit, you
> can even keep the placement. (But you need to do the rotation manually,
> just like if you did the initial placement).
Actually I do it differently, I select the subcircuit(s) I want to
replace, go to edit attributes {e p}, then delete the footprint
attribute and reimport the schematics.
It keeps the location/rotation/side/refes (except for the refdes
position). And it works for batches, say that you have changed the
footprint for SOIC-8, you select all SOIC-8 (for some reason I've not
been able to select using "Advanced search and select" ({s s}) command)
and replace them by batch with schematics import.
There is one this that it does not keep: the thermals. Which is a bit
annoying when the subcircuit in question is a 320 pin connector with
240 thermals.
Regards,
Gabriel
Reply subtree:
3668 Re: [pcb-rnd] Connections in Netlist but don't appear in PCB-rnd from Gabriel Paubert <pa...@iram.es>
3672 Re: [pcb-rnd] Connections in Netlist but don't appear in PCB-rnd from Jesse Frey <je...@gmail.com>
3673 Re: [pcb-rnd] Connections in Netlist but don't appear in PCB-rnd from ge...@igor2.repo.hu
3674 Re: [pcb-rnd] Connections in Netlist but don't appear in PCB-rnd from Jesse Frey <je...@gmail.com>