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" <[email protected]> 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 > > >
