Continue to Site

Welcome to our site!

Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

  • Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

KiCad to produce PCB layout

Status
Not open for further replies.

lipschutz

Member
hi all

i have been trying to use KiCad for over a week to get a pcb layout done. here is what i got:

a) the schematics has been drawn using the Eeshcema
b) the netlist file and the footprint association has been done using Cvpcb

now is the time to create the pcb layout using Pcbnew. however i can not associate the previously created files with this successfully. the question is am i missing something on the process? i suppose once i connect the schematics to pcbnew the layout should be visible on the pcbnew screen.

i have a colinbus pcb milling machine in my lab likewise i need the gerber file created by the KiCad.

thanks all
lipschutz
 
i don't know about you but i've found kicad very intuitive (even though at that time it didn't support panning for example). when i goit it, i read help files and about an hour later i was working on my first project, that day i completed two PCBs.

standard workflow is:
1. create project (preferably in it's own folder)
2. use EESchema to create schematic
3. annotate schematic (use built in feature, don't do it by hand)
4. check schematic, if there is no errors, export Netlist
5. use CvPcb to complete Netlist (assign matching footprints to all parts) and save it
6. open PcbNew and import netlist (if you didn't mess around with file names, default netlist will be the correct one)
7. arrange components any way you like (flip, rotate, whatever)
8. optional: select number of layers (default is 2)
9. optional: create netclasses for types of signals and assign them (for example you may leave default as is, but use wider traces for power nets)
10. select board outline layer and draw it
11. route board
12. check board, if no errors are found, generate gerber files and drill file.
13. send the gerbers and drill file to PCB manufacturer
 
note, when you import netlist, all parts will be in same spot near upper left corner. you need to spread them around within PCB outline either manually or using built in functions. read the manuals or if you are stuck, ask specific question.
 
the netlist is imported and the layout is drawn as well with some difficulty, and eventually i will seek help onward.

thank
lipschutz
 
by checks i meant using ERC and DRC checks
if you are not aware of measuring tool, try it out, i find it invaluable when placing parts or making outline. when you move mouse, bottom of the screen shows mouse location. there are two positions: absolute and relative.
absolute is always with respect to origin. relative is more useful because you can set origin anywhere you like by simply pressing space bar. this is handy when placing components, checking alignment or making board outline. have fun...
 
in pcbnew, when adding tracks, it seems some of the white lines showing connections do not disappear as tracks are made. again in some cases the tracks are not at all connecting while connecting two nodes.
 
if the white lines ("rats nest") do not go away, your trace is not correct - it does not connect two pins. this can be result of several issues, here are the most common ones:
1. you are attempting to make connection on wrong layer or pcb side (take a closer look with 3D view)
2. you are using own (bad) footprints with pins that do not snap to grid (make sure to use 0.050" when making footprints)
3. you are using too fine grid and the traces start or end at wrong points (not on pins)
4. your schematic and/or netlist is incorrect (check ERC, duplication of net labels, footprint assignment, etc.)
5. you are attempting to route trace too close to other traces/zones/pads (check PcbNew settings, trace widths and minimum clearances)
6. you are trying to make a wrong connection, when you click on one pad, matching pads (ones on same net) light up. those are the only pnes you can connect to. if this is not what you want, you are making mistake, check schematic and re-import netlist
 
Last edited:
hi panic

sorry for being late in response. the pcb is made and it was easier than ever using kicad.

thanks
lipschutz
 
Status
Not open for further replies.

Latest threads

New Articles From Microcontroller Tips

Back
Top