Hi Ted, You are not the only one that has had problems getting started, I ran into quite a few problems at first.
n Eeschema it works by default in a "snap to grid" mode, so there is not really any need for a snap to pin. I see that you are creating your own parts - that's jumping in at the deep end for sure :-) - I mentioned this before, but do check this out again. It is VERY important to ensure that the grid used for the part and the grid used in eeschema are the same, and it is VERY easy to make an error here. A part that I made one time would not connect, it turned out that when I edited the part, I had zoomed into make a start, clicked down to lay out the first part of the parts and things seemed to go OK. However when I went to use the part, I placed it down and the reference point aligned up on a grid point, but because I had placed the rest of the part on something like 55tho 110thoi etc rather than 50, 100, 150 and so on, the pins fell just off the grid that eeschema used, so the wires would not connect. There are 1000's of components already defined in KiCad, it's worth sticking withe these for a bit until you get comfortable with the system. It's also a good idea to copy an existing part and use that as the basis for your own, that tends to get the grid and such like sorted out. Until a wire is connected, it will not create a net. That's the basic problem you are having there. Get the connections sorted out and the nets will work. The power names and such like, yes these can be confusing. There are two aspects to this, the first are the power names, and the second are the pin types. If you pull up a device, enter the lib editor and select edit pin, you get a list of all the possible pin types. Input, output, Bidi, 3 state and so on. Power in and power out are the odd ones. Other pin types do as expected, i.e. are an input, output, bidirectional, passive, unspecified and so on. You choose the type of pin that suits the part. Power in and power out are a bit different. Power in is pretty easy to understand, that's the power to the chip. Power out is a bit different. This is normally used with regulators and is a SOURCE of power or if you prefer it's a generator. This can cause a fair bit of confusion in creating circuits later. Associated with pin type are the pin names. IF the pin name is something like Vcc, Vss GND +5 etc (anything defined in the power type lib) then this is a NAMED net, you do not have to run wires to these pins, you just add a power connector and thats it. Now this is where things get confusing. If you design a circuit, and it uses named power, then in order for things to work these have to be connected to an active power source. This is fine if you have placed a regulator device that has a power out pin, as that is automatically a power source. If you have not placed such a device, perhaps your power comes in off board, then you have to tell eeschema that a particular power port is energised. You do this by connecting a power flag to it. (Even on regulators you normally need to place a power flag on the ground connection to show that it is energised). Vcc is a name, it can be both power out and power in depending on use. On something like a 7400, it's the power into the chip. However something generates Vcc, so what you do is connect a Vcc power port either to something that generates Vcc, or you connect it to a power flag to tess the system that it is powered. The thing to remember is that once you do this, ANYTHING called Vcc will automatically be connected to each other. Normally you will not see the power pins on a chip, they are hidden, so you just need to set up the power ports. I am a bit confused regarding your problems with polygons, a polygon is just a graphic line, it does NOT make connections to pins. Exactly what are you using it for. (It is used to draw the shape of a gate for example) You only make connections to pins with wires or busses when drawing the circuit. Keep trying and keep asking... after a bit you will wonder what all the fuss was about. (I've tried several different packages and you get much the same thing on the initial learning curve with all of them) Andy On Thu, 23 Apr 2009 09:45:18 -0700 (PDT) Ted Huntington <[email protected]> wrote: > I'm still having trouble connecting pins easily - I think there could be a > "snap to pins" option for eeschema that would make this very simple - my eyes > are not maybe as good - or perhaps I should make the wires thicker? Because I > have to try 4 or 5 times to get the wire to connect - so there is a square > (accept on power parts - which I can see are connected when the wire is > closed) to show that there is a node. > > Initially I think part of the problem was that - and I am a total newby so > sorry about this being so basic - but I had trouble understanding pin types - > for example I thought Vcc would be a "power out" and would connect to other > "power out" pins - but apparently the symbol Vcc (and GND) is a power in, and > connects with a power out or passive, input, or output. The Vcc on a chip is > apparently a PowerOut - or is this backwards? I searched for some standard > list of pin types on the web and couldn't find anything. I understand the > grid in the "check schematic" option which shows which pin types can connect > with each other. Should the view be that in or out is from the perspective of > connecting wires? Then, for example, I have terminals which I use for both > inputs and outputs depending on the design - so perhaps I should create > different parts - one Terminal_In and another Terminal_Out for the different > pins. I thought I would just make them passive and all > the warnings would be solved. But the main problem seems to be the > difficulty in physically connecting the pins - one idea is to keep clicking > around until you find that 1x1 pixel which will close the wire. I don't know > how people have been doing it successfully for so many years - maybe it takes > practice. > > Then I cannot get many nets to appear in the net list -are these created only > by eeschema or can a person create and name a net? I guess the net names come > from one of the pin names connected in the net? > > I did get the polygon making to work - it appears to be broken in the current > version but is ok in the stable version. Possibly the mouse tracks are from > Xwidgets? > > All together, I think kicad is ok to use for my projects - the last part I > need to figure out is how to make the pins and polygon connect - and this is > clearly by making the polygon have the same net as the pin 0 but the nets > depend on making pin connections which I can't easily - but then I did make > connections with a 7805 regulator (+24V, +5V, and GND) - but the nets do not > appear in PCBNew - I think I realize now that I need to delete and readd the > 7805 to PCBNew now to get new nets in the netlist to be recognized. I tried > adding nets by hand but PCBNew does not appear to be importing new nets - > because I deleted "GND" from the netlist - and it still appeared as the only > net- as if the net list is cached and new changed ignored. > > Thanks - and I'm sure I can get over this last hurdle, > Ted
