Problems getting to grips with Kicad - Page 1
Forum section: electronics / general

author: Specmaster
author_rank: Super Contributor
timestamp: February 03, 2019, 01:57:41 am
content: I just downloaded this program so I can learn how to drive the bloody thing and start making boards etc. This is my first time with this type of software although I do know how to use AutoCad.I'm running Windows 10 64bit, and I downloaded the latest stable version 5.0.2 and printed out the document Getting started in Kicad only to find it does not appear to be referencing V5.0.2 at all as in many places it tells me to this and that and and insert a part and then it shows what the part should look like on screen but it looks nothing like it at all.In other parts of the document it instructs me to click on preferences, then select Manage Symbol Libraries except that option is not present in the drop down menu.I'm beginning to pull what little hair I have left and I'd rather not do that, its so cold latelyI uninstalled V5.0.2 and installed v4.0.0 thinking maybe that the tutorial document might be written with that version in mind...er no it wasn't so I'm no further advanced with this program which so annoying as I watch a video and it seems to be pretty powerful and yet I'm struggling on the tutorial.Can anyone actually tell me which version I should using to learn on and also provide me a link to the correct tutorial notes that refer to that version please?

author: Microcheap
author_rank: Frequent Contributor
timestamp: February 03, 2019, 03:51:33 am
content: There is a tutorial series on youtube sponsored by digikey that I found very useful and help me get started with kicad, you can just skip the annoying intro:https://youtu.be/vaCVh2SAZY4And don't mind the kicad documentation, apparently it is not kept updated.edit: just realized there is another series of videos with the changes in version 5.0https://youtu.be/gIf8sdd-JL4

author: MitjaN
author_rank: Contributor
timestamp: February 03, 2019, 06:27:32 am
content: V 5.0.2 is the preferred one. Besides the program enhancements, the V5 library is significantly better. The fact that the documentation is not synced with the SW is known and sad fact, but as it is a community effort this is what we have. I strongly recommend the FAQ section onhttps://forum.kicad.info/c/faq.Also you are more likely to get a fast response to your questions there.If you are on windows and you have installed V4, you might have to remove some environment variables when reinstalling V5. Also when installing V5, install just the base software without the libraries, and then install the libraries fromhttp://kicad-pcb.org/libraries/download/to a location of your choosing that you have write access. Then you'll have to tell the KiCad where the libraries are.

author: bson
author_rank: Unknown
timestamp: February 03, 2019, 04:50:14 pm
content: v5 has completely revamped how symbols, footprints, and libraries are managed. The changes are VASTLY for the better, except it obsoleted a lot of community contributed documentation. Yet it's still worth it.I'd create a test project, then just experiment with it. Create a schematic, create a symbol, add it to the schematic, edit the symbol to see how it updates the schematic. Press "E" on the component, find the footprint location, pick a footprint. Or go back to the main project navigator (the initial window) and run the footprint editor to create a new footprint. Just poke around, WITHOUT also trying to design anything at the same time. Learning PCB design and learning KiCad are two different things entirely. Press F8 to copy the schematic info the PCB and edit a PCB.Again, just poke around, do stupid things, see how things work. How to select and work on groups of parts. Invest time in it. It's really not hard, you just have to give it a little time to become familiar. Learn the keyboard shortcuts.Poke around with gerber generation (the plotter button in the PCB editor). Get a gerber viewer (ZofzPCB is excellent if you're on Windows) and see what you produce.Make sure you understand what each of the standard layers are for, how to run DRC, zones and zone fills, look up new terminology if you're totally new to PCB CAD (terms like annular, fillet, width & space, net class, zone, fill, via stitching, courtyard, keepout, track coupling, stackup, escaping a footprint, rat's nest, push & shove, etc etc etc). It's an entire world unto itself.

author: Specmaster
author_rank: Super Contributor
timestamp: February 05, 2019, 09:36:33 pm
content: Thank you to all those members who have replied to my post and offered advice. I'm making progress with this now but it is kind of slow, even with help of the video tutorials as the presenters of those assume by the way that they use the shortcuts etc, that the viewer almost knows as much as they do, which kind of defeats the object.My impressions of KiCad so far is that it is a wonderful piece of software but for the first time user, a very steep learning curve, especially if you want to make use of the simulation and also the PCB layout in order to get some PCB's made up. Using it to create a schematic I found is reasonably easy and I can throw together schematics fairly easy however there seems to some glaring omissions in the parts database, such as double pole, three position toggle switches, or indeed DP, 3 position of any kind of switches.Annotation is also an area that needs a bit more work, or it might just be me because maybe I have yet to learn it properly but I need to show 2 x double pole, 3 position switches in various parts of a schematic and I thought I had the answer by using the single pole versions and indicating that they were linked by using a dotted line between the two. Great I thought until I came to the annotation, it does like them being called SW1a and SW1b etc, is there a fix for this at all?Still struggling to get to grips with the "electrical rules check", it keeps throwing up the odd green arrows and less then helpful comments???. Like wise with footprints and layout and gerber parts of it but I have no doubt it will come.Does anyone know of a good book about version 5 that is available or is this not ready yet, the help notes and getting started guides all seem to be referring a version some years ago and are not really worth the paper I print them on.

author: saike
author_rank: Regular Contributor
timestamp: February 05, 2019, 10:06:19 pm
content: Wayne Stambaugh the head developer of Kicad has just given a short speech at Fosdemhttps://fosdem.org/2019/schedule/event/kicad/in which he talks about some of the problems encountered when running a project of this sort.A huge part of the functionality of Kicad is due to the work done by volunteers working in their own free time, and getting every component that everybody needs into the libraries means a lot of people volunteering to give up their evenings / weekends and holidays etc. and a lot of people do this.Kicad has gained a lot of traction in the past couple of years with interest / contributions from commercial companies and it has a very bright future, but patience is needed, or the alternative is to spend the $xxxxx dollars on a commercial program that sucks slightly less than Kicad which is not for me.Edit: altered the last sentence because it looked like a criticism of the op. not intended at all

author: Doctorandus_P
author_rank: Super Contributor
timestamp: February 06, 2019, 04:36:28 am
content: Quote from: Specmaster on February 05, 2019, 09:36:33 pmYou get an overview of all available switches, by typing "a"dd in Eeschema, and then type "switch" (which also lists lots of digital switch IC's) croll down to select the "switch" library with your mouse. Threre are some 3 position switches, for example: "SW_SP3T" and "SW_Rotary4x3".Quote from: Specmaster on February 05, 2019, 09:36:33 pmThe schematic symbol "SW_DPDT_x2" has 2 separate switches. After anotation one of the switches will be SW1A and the other SW1B. Note that the "A" switch has pin numbers 1,2,3 and the "B" switch has pin numbers 4,5,6. The dotted line you add are for humans only and have no meaning for KiCad. You can edit symbol propertys by simpl hovering over a symbol and pressing "e"dit.Quote from: Specmaster on February 05, 2019, 09:36:33 pmShow us an example and we can explain. The green arrows usually are real errors / omissions in the schematic.Quote from: Specmaster on February 05, 2019, 09:36:33 pmA quick search:https://duckduckgo.com/html?q="kicad+5"+tutorialleads to some tutorials which seem to be updated for KiCad V5. This one for example is divided in simple short chapters and mostly based on pictures:http://www.diytechstudio.com/tutorials/page/kicadTutorial/1I heard something about an un-finished KiCad V5 book. It may have been from Wayne Stambaugh's talk at Fosdem 2019 but I'm not sure.

author: Specmaster
author_rank: Super Contributor
timestamp: February 06, 2019, 01:18:46 pm
content: I have downloaded the recommended files and tutorials that have been suggested here and I have also purchased in the interim while waiting for the book on version 5, "KiCad like a pro" by Peter Dalamaris on Kindle from Amazon and hopefully between these sources I shall learn a lot more about this great program.I attach a schematic I drew up for a AF/RF probe for use in audio equipment and domestic radios (not my own design but one found in an old online magazine) that looking to create the PCB's for but when performing the electrical rules check it keep generating random errors and I attach print of the schematic below for info. I can see no electrical error at the points indicated, any thoughts at all?

author: grbk
author_rank: Contributor
timestamp: February 06, 2019, 02:50:34 pm
content: Quote from: Specmaster on February 06, 2019, 01:18:46 pmWithout trying it out myself or seeing the error messages, I believe you're getting an error on GND because you need a power flag somewhere on the GND net, and the error on pin 1 of C1 because Pin 1 of C1 isn't connected to anything -- that net doesn't go anywhere.But stepping back for a minute, what does "to probe" mean? How are you actually connecting the probe? A connector? Solder pads? Screw terminals? You need to put something in the schematic that represents those connection points, for two reasons:a) It will fix the DRC error on pin 1 of C1, because now that net will be going somewhere (i.e. connecting C1 pin 1 to the connector or solder pad or whatever, not just floating)b) Without it kicad won't add anything to the PCB for the connection point (whether that's a through hole for soldering wires or a connector footprint or whatever) because it has no idea what your intent is.This is just something that isn't necessarily obvious until you've gone through the whole CAD schematic and PCB process before, but in general *everything* on your PCB needs to be in your schematic. Even if it's electrically meaningless or obvious to you, your intent isn't obvious to the CAD system until you explicitly add it to your schematic. This means connectors, mounting holes (and whether they're grounded), etc.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: February 06, 2019, 03:33:12 pm
content: Show us the text of your error messages.I say it again:Show us the text of your error messages.Without the text of your error messages we can only guess what they are.A pdf of the whole schematic is not going to help.Or even better:When doing an ERC check, activate the checkbox in front of "Create ERC file report" and save the file as text, then post it here.I attached an example.You have to rename the *.erc file to *.txt or else you cannot upload to this forum.

author: Specmaster
author_rank: Super Contributor
timestamp: February 07, 2019, 01:16:15 am
content: Ok, here is the modified drawing with proper terminations on the probe input which removed one of the error messages. I put a _ve power flag on the GND which removed the second error message but then another appeared, again on a GND connection.Attached is the drawing and also the error message as requested.

author: Rerouter
author_rank: Super Contributor
timestamp: February 07, 2019, 01:24:36 am
content: Remove the VEE bit, and just add a power flag to ground.

author: Specmaster
author_rank: Super Contributor
timestamp: February 07, 2019, 01:44:22 am
content: Just removed the VEE bit and added another Power Flag and it passed rule checker, thank you. Now I can move onto the next stage and see if I can associate the footprints correctly and then run the traces and make a PCB file

author: Rerouter
author_rank: Super Contributor
timestamp: February 07, 2019, 06:02:33 am
content: Just to explain the why. Kicad lets you set electrical types to each pin on a schematic component. So power inputs. Power outputs. Inputs. Outputs. Etc. And has a table of what is allowed with what (that can be edited)If you have something set as a power input. It expects to be connected to a power output or similar. This is the rule it was testing.So your positive pins needed a flag to say "this net has a power output from somewhere", and same with the device ground. Because there is nothing to say the ground symbol you picked is actually powered from elsewhere. E.g. just 1 of them is set as VEE instead of ground. Kicad would raise an ERC violation.In short if pins are set as power inputs. And its intended to be powered from an external connector. It will need power flags in kicad.As for assigning components. Most common footprints are included these days. But learning how to add symbols is handy when you get to more complex projects. (Setting custom grids can make things like BGA footprints a breeze)

author: pierreraymondrondelle
author_rank: Contributor
timestamp: February 07, 2019, 02:12:59 pm
content: Hi!,A good habit is to put all the power signal definitions with the power flags and their interconnections when needed (ex. VSS and Gnd, +5 with Vcc, ...) in a corner of the sheet as well as the decoupling capacitors with their locations.Concerning the errors, they also may come from a wire overlapping a component's lead. This is not always easily visible. It often happens when a part is moved or badly dragged on the schematic. Make sure that all wires are ending on the component's dots.regardsPS. shame on me, I'm still on BZR4022 .......