| ID: | 3254 |
| From: | ge...@igor2.repo.hu |
| Date: | Thu, 8 Aug 2019 04:46:45 +0200 (CEST) |
| Subject: | Re: [pcb-rnd] import .fp, modify and save as new footprint |
| in-reply-to: | 3253 from James Battat <jb...@wellesley.edu> |
| replies: | 3255 from James Battat <jb...@wellesley.edu> |
This message is in MIME format. The first part should be readable text,
while the remaining parts are likely unreadable without MIME-aware tools.
--0-269357287-1565232405=:2358
Content-Type: TEXT/PLAIN; charset=UTF-8
Content-Transfer-Encoding: QUOTED-PRINTABLE
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).=C2=A0 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_mis=
c.mod/arduino_header.fp
> and rename to arduino_header_nohole.fp
>
> =3D=3D=3D Approach #1 =3D=3D=3D
> * Open footprint in pcb-rnd:
> =C2=A0 $ pcb-rnd arduino_header_nohole.fp
Good so far.
> * Break up subcircuit
> =C2=A0 Select all visible: {s a a}
> =C2=A0 Break selection subcircuits to pieces {s b s}
Do not do this! If you open the subcircuit directly, you are editing a=20
subcircuit, not a board. The title of the window will indicate this. In=20
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=20
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=20
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=
=20
with the default layer stackup
2. import the footprint using File/Import/Load subciccuit data, or from=20
the library (you can configure both edakrill and gedasymbols to show up in=
=20
the library window if you have wget installed so you can browse them=20
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=20
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=
=20
subc)
7. save buffer subcircuits to file (buffer menu)
I recommend using method A in your case. A major advantage of method A is=
=20
that the layer stackup is your subcircuit's, no subc-to-board layer=20
binding is ever done, so you can edit an existing footprint without having=
=20
to worry whether you miss a layer (a layer the footprint uses but your=20
board you use for editing doesn't have). But, this won't be a problem=20
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=20
subcircuits into one.=20
(The reason we allow breakup in direct subc editing is that it will make=20
sense with multi-level subcircuits (subc-in-subc), breaking up a subc that=
=20
is whithin the subc you are editing - so it's better if we get used to it=
=20
now than if I change the behavior later)
HTH,
Igor2
--0-269357287-1565232405=:2358--
Reply subtree:
3254 Re: [pcb-rnd] import .fp, modify and save as new footprint from ge...@igor2.repo.hu
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