Hi again, After my first excitement I had to realize that I can not get path polylines from pcbnew. Instead I could only get separate linear line segments without connectivity information.
So I startet modifying the algorithm to use a round end style, to make it work. However this way I did not have any butt lines from the polygon that I could test whether they were on the leaf vertices. Anyway, after some reworking, I think I have the first KiCAD integrated version available. Right now the feature list is the following: - Plugin is installable in ~/.kicad_plugins - Then Highlight a Net in pcbnew - Run the plugin using Tools->External Plugins - At this point only a matplotlib generated window is shown, no actual vias are placed on the board - But so far this gives satisfactory results. It is also possible to run the python script stand-alone. It loads a path from the .json file and runs the algorithm on it, showing it in a matplotlib plot. https://github.com/skuep/kicad-plugins https://github.com/skuep/kicad-plugins/blob/master/via-fence-generator.png Tell me what you think. Now I am a lot smarter when it comes to path operations (Jesus, that was new to me!) Best Regards :-) Simon Am 03.06.2017 um 17:48 schrieb Simon Küppers: > Hi everyone, > as promised I started working on the via fence generator plugin for > KiCad. > > The idea behind the plugin is that you can somehow select a trace in the > pcbnew program and run the plugin so that you get vias all around the > trace to shield it from other parts of your circuit boards. This > technique is often used in RF design with grounded coplanar waveguide > (GCPW) or substrate integrated waveguide (SIW) type of transmission lines. > > Now I am very new to KiCad itself and thusfar I only worked on the > generation of the correct positions to place the vias. I have not yet > worked on the integration into KiCad, because I still have some > questions regarding that. > > Now down to business. In my repo at > https://github.com/skuep/kicad-plugins > you can find via-fence-generator.py. At this point in time, it is not > integrated into KiCad. Right now it functions only as a test suite that > you can simply execute with any Python 2 interpreter. > > The required libraries are pyclipper and math. For the test suite also > numpy and matplotlib are required in order to plot some stuff in a 3D > window. Those libraries will not be required for the actual via > placement, since it is not so straight forward to get those installed > easily on a windows system. > > As I have found out today, it is not as easy as I have thought to make > via fences along tracks and still pass the DRC. > My first thought was to use pyclipper to offset the track to the left > and to the right, so you get new tracks that are a constant distance to > the original track. Then the vias should be equally spaced on those > generated offsetted traces. The problem with that is, that if you have > acute angles in your original track (ok, it is unlikely but still!) and > place the vias at a constant distance along the path, vias at the > "inside" corner get way too close together. > > But I think I have found a really neat solution that already gives much > better result than I have ever had in Altium Designer. What I did is, > that I find kinks in the offsetted paths and place fixed vias at these > positions. Then I am basically left with a lot of path space between > those fixed vias, which I then fill with a constantly spaced distance > along the path. > > Ah, one tricky thing I had to figure out was, how to actually get two > separated offsetted paths from the "expanded" polygon that pyclipper > generates. I think you can all spot it in the python code, it is fairly > well documented. > > You can see an example image here > https://github.com/skuep/kicad-plugins/blob/master/via-fence-generator.png > > You can try it out with your own settings and see if it breaks. > > For the integration into KiCad i thought there might be a way to select > traces in pcbnew. As I could not figure out how to do so, I suppose > there is no way to select tracks or line segments in pcbnew? > Another way (the Altium way) would be, to enter a Net name into a dialog > and the entire net would be via-fenced. I am not sure if this is > practical, but it might be the way we should start to integrate it. > > There is also the question where to get the values for viaOffset and > viaPitch for the algorithm. Should we pull these values somewhere from > the design rules? maybe make them dependent on the net class? I would > rather be able to override them using some sort of dialog. > > In RF PCB design there is something called a substrate integrated > waveguide. You can see it here > https://www.microwaves101.com/encyclopedias/substrate-integrated-waveguide > It basically is Top Copper, Bottom Copper and just two "walls" of vias. > There is no way to generate this automatically in any PCB CAD package > known to me. Where I work, we deal with frequencies above 100 GHz and > here SIW works much better, so we use them a lot. It would be really > really cool, if the via fence generator could support them. > > One way I could imagine this is the following: > We use a user defined layer (you can see, we need a lot more of user > defined layers...) and draw a track where the SIW is to be implemented. > Then we select the track (again, is that even possible?) or use all > tracks on the user defined layer as input to the via-fence generator. It > would then simply generate two walls of via with very well known offset > and pitch. > > Ok that is it for now, tell me what you think about it. Maybe I should > (have) post/ed it over in the forums.. hm? ;-) > > Best Regards > Simon > > _______________________________________________ > Mailing list: https://launchpad.net/~kicad-developers > Post to : kicad-developers@lists.launchpad.net > Unsubscribe : https://launchpad.net/~kicad-developers > More help : https://help.launchpad.net/ListHelp > _______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
