← Back to team overview

kicad-developers team mailing list archive

Re: Latest usage of Kicad


Rob Frohne wrote:
Hi Dick,

If I can figure out the new features, I have an interest in doing a tutorial. It won't likely get done until I get a bit more practice at things. I am still back on the learning curve, but I would like to try and get my spring quarter electronics students to use Kicad for small boards, and a tutorial would be helpful for them.

Thanks for the encouragement. And any tips you can give on setting rules up for freerouter would be appreciated.

On this most recent board and with the most recent software, all the setting up of rules was done in pcbnew's netlist editor. About the only thing I did in freerouter was establish the snap modulus for the move component command. I did most all the small SMT part positioning in freerouter, and major connector part positioning in pcbnew.

Roughly, in sequence:

1) in pcbnew: establish board perimeter.

2) in pcbnew: establish any zones, inclusive of net association.

3) in pcbnew: load in the netlist so you have all the components defined and instantiated.

4) in pcbnew: do the degree of component placements you are comfortable with. It is a little easier to accurately position components in pcbnew than in freerouter, but either will work.

5) in pcbnew: set up the netclasses. power traces might be a little thicker. so add a netclass called "power". Make its traces thicker than what you establish for netclass "Default". Set spacing and vias for each netclass.

6) in pcbnew: export to DSN.

7) load up freerouter (keep it running for any subsequent iterations of 6) through 14) here ).

8) in freerouter: load the project's *.dsn file.

9) in freerouter: set your move snap modulus, which seems to default to 1 internal unit. 20 mils in x and in y is about reasonable.

10) in freerouter: finish placing any components, you can change sides of a part here also, rotate, whatever.

11) in freerouter: route the board, save frequently to a *.dsn file while routing, in case of power loss, not yet a session file but a full *.dsn file. The full freerouter *.dsn file is a superset format, one that fully defines the board and can be reloaded between power outages, whereas the *.ses file is not a complete design, but with the *.brd file constitutes a full design.

12) in freerouter: when done, or when you want to back import, then save as a session file, *.ses.

13) in pcbnew: backimport the session file

14) in pcbnew: at this point the zones have to be refilled. One way to do that is to simply run DRC.




Dick Hollenbeck wrote:


I just did a 4 layer board in about a week with Kicad and Freerouter.
What a joy this was in comparison to doing the same thing a year ago.

The netlist support was a dream. I was able to classify nets, setup
widths and spacing on each netclass (a total of 3), and then export to
Freerouter. In Freerouter I have gotten in the habit of manually
routing using the push and shove.

What was really slick was the ability to immediately round trip without
any additional setup. You got something you want to do back in PCBNEW,
such as tweak a zone, simply back import, make the change, re-export
back over to freerouter. No setup, just a very few button clicks.

Undo/redo was also used and appreciated.

Our efforts are paying off. Thanks Jean-Pierre, Wayne, and others for
all your contributions.

The user base is in for a treat whenever they get a hold of these latest
features. The documentation is probably lagging, but this stuff is
almost so easy it can simply be figured out, and is better than nothing.