Move a component via (python) command line?

Layout
1

Is there a way to quickly snap a component to the cursor via (python) command line ? I’m used to the powerful command line that comes with EAGLE. There I can run something like

move R4

which attaches R4 to the cursor so that there is no need to search for it.
Thanks.

2

within eeschema or pcbnew?

if you open cvpcb from within eeschema and click on the component in the list there eeschema will focus on the part - at least in BZR6097.

if you have eeschema and pcbnew open at the same time, clicking on a component in either program will focus the other programs view on that component.

3

Have you tried using shortcut ‘T’ in Pcbnew, it will open a window where you type the component ref like R4 and it will snap to your cursor position and you can move and place it where you want.

I hope this is what you are looking for.

2 Likes
4

Hi,

In 2018 it is possible to use the python bindings to load / edit / save the file.
http://docs.kicad.org/stable/en/pcbnew.html#_kicad_scripting_reference

I here is a (simple) example that places D1 at 100,100 with a 45 degree rotation

#!/usr/bin/env python
import pcbnew

# Load the board
pcb = pcbnew.LoadBoard("take2.kicad_pcb")

# Find the component
c = pcb.FindModuleByReference("D1")

# Place it somewhere
c.SetPosition(pcbnew.wxPointMM(100,100))

# Rotate it (angle in 1/10 degreee)
c.SetOrientation(45 * 10)

# and save the file under a different name
pcb.Save("take2_mod.kicad_pcb")

This does require you to close the project and run from the command line. pcbnew also has a plugin system (that I tried yesterday based on sample code found here)


Combing this knowledge it should not be very hard any more to create a “python console” to execute the changes on a running document.

For now I am (generating) a layout.cvs file(with component name , x , y , angle)

D1, 133.00, 67.00, 270.00
D2, 130.40, 67.23, 280.00
D3, 127.87, 67.90, 290.00
D4, 125.50, 69.01, 300.00
D5, 123.36, 70.51, 310.00
D6, 121.51, 72.36, 320.00

and the following python script

#!/usr/bin/env python
import sys
import pcbnew
import numpy as np

data  = np.genfromtxt('layout.csv',delimiter=',',dtype=None)
print (data)
filename="take2.kicad_pcb"
pcb = pcbnew.LoadBoard(filename)

for i in data:
    c = pcb.FindModuleByReference(i[0])
    c.SetPosition(pcbnew.wxPointMM(float(i[1]),float(i[2])))
    c.SetOrientation(1.0 * i[3] * 10)

pcb.Save("take2_mod.kicad_pcb")

Additionally I figured out it is possible to do the same on an existing project. for that create a file in ~/.kicad/scritping/plugins called “layout_using_csv.py” with the following contents

import pcbnew

import Tkinter
import numpy as np
from tkFileDialog import askopenfilename

import os

class PlaceMyComponent(pcbnew.ActionPlugin):
    """
    contents of the layout.csv should be something like this (reference name, posx posy, angle * 10)

    D10, 100.00, 69.00, 450.00
    D9, 98.09, 69.17, 460.00
    D8, 96.24, 69.66, 470.00
    D7, 94.50, 70.47, 480.00
    """
    def defaults( self ):
        self.name = "Layout using CSV"
        self.category = "Modify PCB"
        self.description = "Move the components to match the layout.csv file in the project diretory"

    def Run( self ):
        print(os.environ['KIPRJMOD'])
        pcb = pcbnew.GetBoard()
        data  = np.genfromtxt( "%s%s%s" %(os.environ['KIPRJMOD'], os.path.sep  ,'layout.csv'),delimiter=',',dtype=None)
        print (data)
        for i in data:
            c = pcb.FindModuleByReference(i[0])
            c.SetPosition(pcbnew.wxPointMM(float(i[1]),float(i[2])))
            c.SetOrientation(1.0 * i[3] * 10)


PlaceMyComponent().register()

To place my components where I like.

Selection_261
Selection_2611701×1101 107 KB

2 Likes