| ID: | 4470 |
| From: | ka...@aspodata.se |
| Date: | Tue, 27 Oct 2020 00:45:11 +0100 (CET) |
| Subject: | Re: [pcb-rnd] KiCad footprints |
| in-reply-to: | 4465 from Majenko Technologies <ma...@majenko.co.uk> |
matt@majenko.co.uk:
> Can we use kicad footprints as direct subcircuits in the footprint library,
...
Yes, but since kicad doesn't specify the clearance for pins/pads, it is
probably better to convert them and set the clearance you want.
///
File -> Import -> Load subcircuit data to paste-buffer
choosing git/kicad-footprints/ .... some footprint.kicad_mod
works, gives this warning:
io_kicad warning at 52.2: Couldn't determine pad clearance, using 0.25mm
///
You can covert kicad fp en masse like:
$ fp2subc /Net/git/kicad-footprints/Oscillator.pretty/Oscillator_DIP-8.kicad_mod
fp2subc: saving subcircuit in /Net/git/kicad-footprints/Oscillator.pretty/Oscillator_DIP-8.kicad_mod.subc.lht
W: io_kicad warning at 37.2: Couldn't determine pad clearance, using 0.25mm
W: io_kicad warning at 38.2: Couldn't determine pad clearance, using 0.25mm
W: io_kicad warning at 39.2: Couldn't determine pad clearance, using 0.25mm
W: io_kicad warning at 40.2: Couldn't determine pad clearance, using 0.25mm
W: There are 2 layers that got lost in the smash because they were on unbound subc layers
This normally happens if your subcircuits in buffer refer to layers that do not exist on your board.
E: save error: versions below lihata board v6 do not support arbitrary text width - will render with default width
E: near 3.6663 mm -11.2075 mm
E: (Leave the thickness field empty (zero) and depend on the automatism)
///
$ cat tt.sch
v 20200319 2
C 10000 24900 1 0 0 res_v.sym
{
T 10000 26500 5 10 0 0 0 0 1
device=Resistor
T 10000 26300 5 10 0 0 0 0 1
footprint=R_0603_1608Metric.kicad_mod
T 10050 25550 5 10 1 1 0 0 1
refdes=R1
T 10050 25050 5 10 1 1 0 2 1
value=1k
}
N 10000 24900 9600 24900 4
N 9600 24900 9600 25700 4
N 9600 25700 10000 25700 4
$ cp /Net/git/kicad-footprints/Resistor_SMD.pretty/R_0603_1608Metric.kicad_mod
"somewhere where pcb-rnd can find it"
$ lepton-netlist -g tEDAx -o tt.tdx tt.sch
...
$ pcb-rnd
File -> Import -> Import tEDAx schematics
works as well as one can expect.
Regards,
/Karl Hammar
Reply subtree:
4470 Re: [pcb-rnd] KiCad footprints from ka...@aspodata.se