| ID: | 3255 |
| From: | James Battat <jb...@wellesley.edu> |
| Date: | Thu, 8 Aug 2019 01:28:08 -0400 |
| Subject: | Re: [pcb-rnd] import .fp, modify and save as new footprint |
| in-reply-to: | 3254 from ge...@igor2.repo.hu |
| replies: | 3257 from ge...@igor2.repo.hu |
Aha!
I had originally tried direct editing of the subc (without breaking up)
but wasn't able to remove the holes. So I tried breaking up the subc.
But after getting your message I went back to direct editing of the subc
(your Method A below) and was able to delete the hole.
The first time around, I had selected the hole and hit "Delete" button
on my keyboard (no action), and I didn't see a right-click-context
option for "delete" or similar. But after your email, I realized that I
should have used the "Del" button (skull-and-crossbones) or {e d}. That
worked for me.
Bottom line, thanks to your response I was able to modify the .fp as
desired and successfully import into my board layout using "Import
gschem schematics". I do have a different question (about preserving
rotation of imported fp) but will ask in another thread.
As always, thanks for your help.
James
On 8/7/19 10:46 PM, gedau@igor2.repo.hu wrote:
>
> On Wed, 7 Aug 2019, James Battat wrote:
>
>> I'm trying to import an .fp file from gedasymbols, modify it (by removing a
>> hole), and then save it as a footprint (to be an attribute for a gschem
>> symbol). I can break up the subc and remove the hole, but then can't
>> reconstitute the subc.
>>
>> Here's what I've tried so far.
>>
>> I start with erich_heinzle's footprint from gedasymbols:
>> http://www.gedasymbols.org/user/erich_heinzle/kicad/footprints/w_conn_misc.mod/arduino_header.fp
>> and rename to arduino_header_nohole.fp
>>
>> === Approach #1 ===
>> * Open footprint in pcb-rnd:
>> $ pcb-rnd arduino_header_nohole.fp
> Good so far.
>
>> * Break up subcircuit
>> Select all visible: {s a a}
>> Break selection subcircuits to pieces {s b s}
> Do not do this! If you open the subcircuit directly, you are editing a
> subcircuit, not a board. The title of the window will indicate this. In
> that case you shouldn't break it up, just start editing.
>
>
>
> There are two methods that will work:
>
>
>
> Method A: direct subc edit
>
> 1. pcb-rnd file.fp
>
> 2. as this opens the footprint, just edit, no breakup or convert, just
> delete objets, draw new objects, everything is done directly on the subc
>
> 3. save the file like if you saved a board (but it will really save the
> subc that you can put in your lib and use as a footprint)
>
>
>
> Method B: edit on a board, using import and breakup/convert
>
> 1. start pcb-rnd without any file name argument so you get an empty board
> with the default layer stackup
>
> 2. import the footprint using File/Import/Load subciccuit data, or from
> the library (you can configure both edakrill and gedasymbols to show up in
> the library window if you have wget installed so you can browse them
> directly there if you want)
>
> 3. don't place the subc, but break up the subc in the buffer
>
> 4. place the broken up parts - they are now board objects
>
> 5. edit your board objects as you wish
>
> 6. select them all and conver the selection to subc
>
> (6.b. or cut them to buffer after the selection and convert the buffer to
> subc)
>
> 7. save buffer subcircuits to file (buffer menu)
>
>
>
>
> I recommend using method A in your case. A major advantage of method A is
> that the layer stackup is your subcircuit's, no subc-to-board layer
> binding is ever done, so you can edit an existing footprint without having
> to worry whether you miss a layer (a layer the footprint uses but your
> board you use for editing doesn't have). But, this won't be a problem
> with the old .fp format, as it couldn't have unusual layers.
>
> Method B is useful if you want to change the origin or merge multiple
> subcircuits into one.
>
> (The reason we allow breakup in direct subc editing is that it will make
> sense with multi-level subcircuits (subc-in-subc), breaking up a subc that
> is whithin the subc you are editing - so it's better if we get used to it
> now than if I change the behavior later)
>
> HTH,
>
> Igor2
Reply subtree:
3255 Re: [pcb-rnd] import .fp, modify and save as new footprint from James Battat <jb...@wellesley.edu>
3257 Re: [pcb-rnd] import .fp, modify and save as new footprint from ge...@igor2.repo.hu