Hi
I want to modify components(footprints?) on the PCB
from pcbnew import *
board = GetBoard()
for fp in board.GetFootprints():
print(fp.GetName())
I get this error
AttributeError: 'BOARD' object has no attribute 'GetFootprints'
while in the doc, that function clearly exists
please help me
thanks
Your kicad version? GetFootprints() is available from 6.0.
just installed it, I am going to give it a try
should I really use footprints ?
I want to set these settings to all components on the PCB
how do I change the “Show” & “Layer” values ?
Value() and Reference() methods of the footprint return FP_TEXT object which has SetVisible() and SetLayer().
Also read this Edit Multi Text plugin for KiCad - #4 by paulvdh
nope, they dont
print(dir(board.GetFootprints()[1].GetReference()))
['__add__', '__class__', '__contains__', '__delattr__', '__dir__', '__doc__', '__eq__', '__format__', '__ge__', '__getattribute__', '__getitem__', '__getnewargs__', '__gt__', '__hash__', '__init__', '__init_subclass__', '__iter__', '__le__', '__len__', '__lt__', '__mod__', '__mul__', '__ne__', '__new__', '__reduce__', '__reduce_ex__', '__repr__', '__rmod__', '__rmul__', '__setattr__', '__sizeof__', '__str__', '__subclasshook__', 'capitalize', 'casefold', 'center', 'count', 'encode', 'endswith', 'expandtabs', 'find', 'format', 'format_map', 'index', 'isalnum', 'isalpha', 'isascii', 'isdecimal', 'isdigit', 'isidentifier', 'islower', 'isnumeric', 'isprintable', 'isspace', 'istitle', 'isupper', 'join', 'ljust', 'lower', 'lstrip', 'maketrans', 'partition', 'removeprefix', 'removesuffix', 'replace', 'rfind', 'rindex', 'rjust', 'rpartition', 'rsplit', 'rstrip', 'split', 'splitlines', 'startswith', 'strip', 'swapcase', 'title', 'translate', 'upper', 'zfill']
print(dir(board.GetFootprints()[1].GetValue()))
['__add__', '__class__', '__contains__', '__delattr__', '__dir__', '__doc__', '__eq__', '__format__', '__ge__', '__getattribute__', '__getitem__', '__getnewargs__', '__gt__', '__hash__', '__init__', '__init_subclass__', '__iter__', '__le__', '__len__', '__lt__', '__mod__', '__mul__', '__ne__', '__new__', '__reduce__', '__reduce_ex__', '__repr__', '__rmod__', '__rmul__', '__setattr__', '__sizeof__', '__str__', '__subclasshook__', 'capitalize', 'casefold', 'center', 'count', 'encode', 'endswith', 'expandtabs', 'find', 'format', 'format_map', 'index', 'isalnum', 'isalpha', 'isascii', 'isdecimal', 'isdigit', 'isidentifier', 'islower', 'isnumeric', 'isprintable', 'isspace', 'istitle', 'isupper', 'join', 'ljust', 'lower', 'lstrip', 'maketrans', 'partition', 'removeprefix', 'removesuffix', 'replace', 'rfind', 'rindex', 'rjust', 'rpartition', 'rsplit', 'rstrip', 'split', 'splitlines', 'startswith', 'strip', 'swapcase', 'title', 'translate', 'upper', 'zfill']
Don’t call GetValue(), call Value(). It’s a different method. Same with Reference().
are there constants for layers ? so far I have to take a wild guess with numbers
board.GetFootprints()[0].Value().SetLayer(0)
board.GetFootprints()[0].Value().SetLayer(6)
also my code is not working
for fp in board.GetFootprints():
fp.Reference().SetVisible(False)
fp.Value().SetVisible(True)
reference is still visible
Maybe this can help:
https://docs.kicad.org/doxygen/layer__ids_8h.html#ae0ad6e574332a997f501d1b091c3f53f
PCB_LAYER_ID
enum PCB_LAYER_ID : int
A quick note on layer IDs:
The layers are stored in separate enums so that certain functions can take in the enums as data types and don't have to know about layers from other applications.
Layers that are shared between applications should be in the GAL_LAYER_ID enum.
The PCB_LAYER_ID struct must start at zero for compatibility with legacy board files.
Some functions accept any layer ID, so they start at zero (i.e. F_Cu) and go up to the LAYER_ID_COUNT, which needs to be kept up-to-date if new enums are added. This is the definition of all layers used in Pcbnew.
The PCB layer types are fixed at value 0 through LAYER_ID_COUNT to ensure compatibility with legacy board files.
Enumerator
UNDEFINED_LAYER
UNSELECTED_LAYER
PCBNEW_LAYER_ID_START
F_Cu
In1_Cu
In2_Cu
In3_Cu
In4_Cu
In5_Cu
In6_Cu
In7_Cu
In8_Cu
In9_Cu
In10_Cu
In11_Cu
In12_Cu
In13_Cu
In14_Cu
In15_Cu
In16_Cu
In17_Cu
In18_Cu
In19_Cu
In20_Cu
In21_Cu
In22_Cu
In23_Cu
In24_Cu
In25_Cu
In26_Cu
In27_Cu
In28_Cu
In29_Cu
In30_Cu
B_Cu
B_Adhes
F_Adhes
B_Paste
F_Paste
B_SilkS
F_SilkS
B_Mask
F_Mask
Dwgs_User
Cmts_User
Eco1_User
Eco2_User
Edge_Cuts
Margin
B_CrtYd
F_CrtYd
B_Fab
F_Fab
User_1
User_2
User_3
User_4
User_5
User_6
User_7
User_8
User_9
Rescue
PCB_LAYER_ID_COUNT
Definition at line 58 of file layer_ids.h.
{
UNDEFINED_LAYER = -1,
UNSELECTED_LAYER = -2,
PCBNEW_LAYER_ID_START = 0,
F_Cu = PCBNEW_LAYER_ID_START,
In1_Cu,
In2_Cu,
In3_Cu,
In4_Cu,
In5_Cu,
In6_Cu,
In7_Cu,
In8_Cu,
In9_Cu,
In10_Cu,
In11_Cu,
In12_Cu,
In13_Cu,
In14_Cu,
In15_Cu,
In16_Cu,
In17_Cu,
In18_Cu,
In19_Cu,
In20_Cu,
In21_Cu,
In22_Cu,
In23_Cu,
In24_Cu,
In25_Cu,
In26_Cu,
In27_Cu,
In28_Cu,
In29_Cu,
In30_Cu,
B_Cu, // 31
B_Adhes,
F_Adhes,
B_Paste,
F_Paste,
B_SilkS,
F_SilkS,
B_Mask,
F_Mask, // 39
Dwgs_User,
Cmts_User,
Eco1_User,
Eco2_User,
Edge_Cuts,
Margin, // 45
B_CrtYd,
F_CrtYd,
B_Fab,
F_Fab, // 49
// User definable layers.
User_1,
User_2,
User_3,
User_4,
User_5,
User_6,
User_7,
User_8,
User_9,
Rescue, // 59
// Four reserved layers (60 - 63) for future expansion within the 64 bit integer limit.
PCB_LAYER_ID_COUNT
};
pcbnew.F_Cu etc. For some reason they don’t all follow the same naming conventions. (What would follow some naming convention in pcbnew API?)
EDIT: I have written some documentation for my own internal use in Plugin howtos · Wiki · eelik-kicad / KiCad Documentation · GitLab. Maybe it can help. The layer constants are documented there, too.
That’s really helpful. Thanks for sharing.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.