Thanks so much Andy. Though a large portion of what you said I had already figured out the hard way, there were key points that clarified a lot.
Yes, the power thing is a bit confusing, but now that I understand it I know how helpful it is. Also I got the new kicad libraries which helped a lot Thanks again Andres --- In [email protected], Andy Eskelson <andyya...@...> wrote: > > Don't worry, it can be VERY frustrating at first. > Do run through the tutorials a couple of times that helps a lot. > > > cct. That me sorry, cct = circuit > > > When creating a circuit in eeschema you use parts from the various > library packages. > > These library parts define the pins that a part uses. There is nothing > special about a pin, it's just a circle and a line, and it is the > connection point for the wires. what you can do is give that pin various > attributes which eeschema can use to check the circuit and also help you > in layout. At this stage you don't need to do anything about this as > you will be using libs that are already created. > > Every part that you use, as far as eeschema is concerned is the same sort > of thing. It will have some sort of symbol and have some connections. > > So in the conn library you will find all sorts of connectors, the 1pin is > just that, a pin that you stick in the PCB. If you know Vero products > such as the copper stripboard, or plain matrix board the pins that you > push into the holes are essentially what the 1 pin connector is. > > At this point you don't know or really care what it looks like > physically, that comes later after you have designed the circuit. > > You need to add the various power ports as needed by your circuit. This > is the one area that really can confuse people at first. In order to > reduce the number of lines on the circuit diagram, eeschema makes use of > named buses and connections, see the tutorial for more info on this. In > the same way, the power connections can also use this idea. So if the > device has a power in pin, say the 5Volt input on a 7400, then that will > be given a special name. In the case of the 7400 if you examine it with > the lib editor you will see that pin 7 and 14 are in black and so are > invisible and pin 7 is called GND and pin 14 is called VCC > > Somewhere on your circuit you place a power port(s) Right hand icon bar, > 4th one down, in the case of the 7400 you would need a VCC port, and a > GND port. These are not "real" parts, they are just labels, and eeschema > will automatically connect any labels with the same name together, but > you will NOT see the wires. This is a bit odd at first, especially with > very simple circuits, but when the circuits get bigger then getting rid > of the power lines makes things easier to see. > > Now comes the confusing bit (at least is was for me) > > If your circuit has a device that PROVIDES power, i.e. it has a pin that > is defined as a "power out" type, that pin will also have a name which > will match one of the power port names. In this case you do not need to > place a power port of that name on your circuit because the device > already provides it. > > Think of this in two situations, if you are designing a board where the > power is provided from a seperate power supply, then you need to tell the > system that there is power on some pin or other, if you were designing a > power supply the the device would be providing that power anyway so you > don't need to tell eeschema anything about it. > > So in the 7400 case, you will place a VCC and a GND power port, and you > really don't need to do anything else with them, however if you select > show hidden pins then you DO need to connect the power ports to the power > pins on the 7400. Now you need to provide a means of connecting some > wires to the board so that you can feed in some volts, to do this you > place a 1pin connector and wire that to the power port(s) > > The last wrinkle is that you need to tell eeschema that there is actually > power being provided. This is used for the Design Rules Check (DRC) > function. Again if a device has a power out type pin then this is > automatically done. In the case of the 7400 only, then you need to tell > eeschema that the power port has some volts on it, all you do is add a > power_flag to the power port net (a net is simply the connections to a > series of pins) You nearly always have to add a power flag to the GND > power port net, and sometimes to the VCC. > > That's the basics of it really. Once you get to that point you should > have your circuit drawn up and all the pins conected to something. > Remember that any unused pins should either be connected to something or > identified as not connected (The X icon about halfway down the right hand > side bar) > > You then need to annotate the circuit, (Top bar 4th from right hand end) > this gives you things like R1, R2 U1 and so on. You can run the DRC to > see if there are any missing connections or other errors. > > Next you generate the netlist, and then you can start on the PCB side of > the operation. What you have to do is associate a particular part on > your circuit with an actual physical part on the PCB. Think of things > like an NPN transistor, it is the same symbol on the circuit, but in > practise it could be a TO3, TO220, TO92 or one of the many SMD > footprints. The PCB layout program needs to know what one you want to > use. > > > So you then run CvPCB this gives you a list of the parts in your > circuit, and you can select the various footprints to use. In CvPCB there > is a "display footprints list documentation" top bar, 3rd icon from right > that is a pdf of the provided footprints. I found that it was useful to > have a copy to hand. > > I the case of the 1pin connectors, just select 1pin footprint. > Once you have assigned the footprints you save that netlist again and > then you can run PCBnew. > > In PCBnew create the board outline then load the netlist and you will > find your components all on top of each other normally in the top left > hand corner. you drag these to the board where ever you want them, > you can then start creating the tracks and so on. > > PCBnew uses MODULES and the design of the module consists of the shape > and the pads. In the case of the 1pin connector it is just a single pad. > During layout you can modify the properties of the pads via the context > menu (right click) DO NOT edit the module itself until you know what you > are doing, and even then create a copy and work on that. > > Don't forget that there is not necessarily a one to one relationship > between a library part in eeschema and a module in PCBnew, as with the > NPN example one part can have many modules. > > > > > Again, do run through the tutorials as that will help a lot. If you get > stuck shout. I can always create a couple of simple examples to help get > you started if need be. (There are several examples provided in the > package) > > Andy > > > > > > On Tue, 09 Jun 2009 04:41:49 -0000 > "Andres Cimmarusti" <andrescimmaru...@...> wrote: > > > > Oh! is that all, > > > just shove some 1pin connectors on the cct and connect that to the power > > > net, you can then place the connector on the PCB wherever you want and > > > use it as a pad. > > > > I'm failing at this...the pins only appear in the lib editor and I honestly > > don't know what cct means :-(. When you say "connect that to the power" do > > you mean I should add a pin to a power symbol? > > > > > One thing, I prefer to modify the pad settings for the 1 pin connector, > > > so that I have more copper and a smaller hole. > > > > I'm also failing at this...I wish this kind of thing were in the help > > files.. > > > > Sorry for being so slow with this... This is my very first electronics > > project... > > > > > > > > > > ------------------------------------ > > > > Please read the Kicad FAQ in the group files section before posting your > > question. > > Please post your bug reports here. They will be picked up by the creator of > > Kicad. > > Please visit http://www.kicadlib.org for details of how to contribute your > > symbols/modules to the kicad library. > > For building Kicad from source and other development questions visit the > > kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups > > Links > > > > > > >
