microstrips in kicad - Page 1
Forum section: electronics / projects

author: on8vq
author_rank: Newbie
timestamp: January 23, 2014, 07:02:24 am
content: Hello,I am educating myself into rf electronics (I got myself a ham license(*) a while back), and after doing some HF experiments, I'm slowly reaching the point (VHF-UHF) where I need to learn about micro-strips and all that fun stuff. I like to use kicad (open standards mean a lot to me), and although it has a tool to calculate micro-strip widths, I haven't found a way to actually draw the strips, with edged ends ending into SMD components, round corners to minimize losses and all that stuff (Again, I'm not an expert, and I don't know at what frequencies those things become really important).So, can anyone get me up to speed on the latest talk concerning the subject? What's the status in kicad, and if I'm out of luck, is it a topic of concern? Are there any work-arounds? Are there people actually doing RF designs on kicad? I would be very interested in *any* information you may provide.(*): I'm the homebrew kind, so I'm mainly interested in the technology, not in buying rigs and plugging it into a wall socket.

author: Rerouter
author_rank: Super Contributor
timestamp: January 23, 2014, 07:58:30 am
content: I'm using the BZR4011 build and no sign of the features your looking for with mine,reading further is seems all of kicad's curves are based on piecewise linear, which means its straight lines approximating a curve down to 1% accuracy, however so far the curves are only allowed on drawing layers,There was stuff added by CERN recently, (or other similar accelerator) which may include that kind of functionity, otherwise if your heart was set on kicad, you could set the grid smaller and trace the piecewise linear of a drawing curve,It appears that as of the 14th this year it is still on the wish listhttp://wiki.xtronics.com/index.php/Kicad

author: Dago
author_rank: Frequent Contributor
timestamp: January 23, 2014, 12:30:19 pm
content: I've drawn some microwave RF boards with kicad by using fills. Very tedious but I don't think any comparable tool (free or cheap) can do microstrips much better. Usually microwave circuits use mitered bends. The details don't get too critical until you start getting way in to GHz territory. I've heard that when "features" on your PCB start being 1/10th of the wavelength in question you need to start worrying about the details.

author: nctnico
author_rank: Super Contributor
timestamp: January 23, 2014, 06:15:02 pm
content: Just use an online trace impedance calculator to calculate the width for the traces. If you use 45 degree corners you'll be ok.

author: LukeW
author_rank: Frequent Contributor
timestamp: January 24, 2014, 11:13:05 am
content: Personally, I use Eagle not KiCAD but I think the answers are probably basically similar.AFAIK there are no tools in the software to "hold your hand" if you're doing RF layout. That sort of stuff generally requires $$$ software.Things like transmission line models (CPWG, microstrip, whatever) you'll probably need to calculate using external software, and then bring in the resulting information (the track width and the trace-to-groundplane separation distance on the top layer in the case of CPWG) and just set those parameters manually in your layout. There's nothing special that you have to do, but it doesn't magically do it for you - you just set those properties as normal.You can make rounded corners the usual way, or draw a square corner and use the "restrict" layer (at least that's what Eagle calls it) to make a mitred corner, since that will force it to "cut" the corner off in that area. You'll need to calculate it by hand.I make wiggly meandered tracks that are lambda/4 long by hand, by manually adding up the lengths of each bit and moving them around - very tedious and annoying! But it works, and I don't know of any better way to do it.

author: on8vq
author_rank: Newbie
timestamp: January 24, 2014, 02:47:58 pm
content: Calculating the widths is not a big problem, there even is a tool for that in Kicad itself! In the main Kicad screen, choose pcb calculater, then choose the TransLine tab.But it seems that for adapting microstrip lines to e.g. chip pin width, I'll have to do some manual work. Using fills is perhaps a good idea, I'll give it a try.Thank you all for your answers! I know I have a lot to learn.

author: nctnico
author_rank: Super Contributor
timestamp: January 24, 2014, 03:00:34 pm
content: Doesn't matter. Just start with a thin trace from the chip and use a thick track where it fits. A tapered impedance converter takes a lot of space. Besides that many RF chips have current sinking outputs. You need 50 Ohms traces from the pull-up resistors.

author: Dago
author_rank: Frequent Contributor
timestamp: January 25, 2014, 08:12:00 am
content: Impedance matching microstrip lines to component pins starts to really matter in the high GHz (5GHz+++) area and there is no single trivial "right" way to do it because it depends on the devices parasitics etc. Usually this kind of stuff is simulated with Agilent ADS or similar tool. Same thing with grounding via locations which can be very critical for very high GHz stuff.

author: nctnico
author_rank: Super Contributor
timestamp: January 25, 2014, 08:43:41 am
content: Grounding can also be optimised by using Sonnet to simulate a layout. Then again grounding is also important for circuits with normal components at lower frequencies. I once followed the advice of an RF expert to make a 700MHz low pass filter. That filter didn't work very well. A current density simulation with Sonnet quickly showed the grounding was wrong. After adding a via to the ground plane close to the capacitors connected to ground it worked as expected.