I think you are having a spot of finger trouble :-) If you get the lines for the 1uF you should get them for the 0.1. Just double check that there is a connection and that you get no ERC errors. If that is the case double check if you have selected the correct footprint. It will be something as simple as that.
Power flags, yes they can be a bit confusing. One of the things that the ERC checks for is power connections. In order to do this the system needs to know if there is power to the circuit. A circuit can be powered in two ways, the first is when you have a simple situation where you feed power to the circuit from off board, usually you connect a power source to a terminal pin. The other way that a circuit is powered is when you have a device on the circuit that generates power. An example of this is a three terminal regulator. If you look at the lib device for them you will see that the output pin is defined as a "power out" type. So if you have a device with a power out pin, ERC knows that that is "powered" and will work without any more work from you. i.e. you dont need a power flag for that line. If you have no power out devices you need to tell thr ERC that there is power, to do this you just add a power flag to whatever line needs it. Grounds are an oddity, in that they can be part of the power system and signal so they are not defined as power out on devices, but that are checked as part of the power system, so you need to tell ERC that they are also powered, hence you pretty much always need a power flag on the ground. Andy On Sat, 04 Jul 2009 02:51:57 -0000 "[email protected]" <[email protected]> wrote: > Whoops! I spoke too soon everything worked except the 0.1uf caps. > back to square 1. > > > --- In [email protected], "acidb...@..." <sunblast...@...> wrote: > > > > Thanks Andy your the Man! > > That worked! > > One more thing, in my schematic i had to use the power-flag tool > > for v+ and gnd. > > Do i have to enter those manually in PCbnew, since there not on my > > board ? > > > > > > --- In [email protected], Andy Eskelson <andyyahoo@> wrote: > > > > > > In your other post you mention a 0.1uF and a 1uF cap as examples. > > > > > > In eeschema you need to add from the devices lib a C for the 0.1 and a > > > capapol (polarised cap (electrolytic) for the 1uF > > > > > > Add the wires, annotate the circuit, then generate the netlist > > > Then run CvPCB. Select C1 for the 0.1 and C1V5 for the 1uF > > > > > > Save the result, which will generate a new netlist, and then import that > > > into PCBnew You should find that all your wires are there. > > > > > > > > > While you are in CvPCB, goto the 10th icon on the top bar, (Display > > > footprints list documentation) that's a pdf file of all the included > > > footprints with Kicad. It's very useful to have that handy when you are > > > selecting the footprints. > > > > > > > > > For documentation there is some: libs are covered in the eeschema docs, > > > and footprints in the PCBnew doc. There is also a tutorial. You should > > > find them in: > > > > > > /usr/local/kicad/doc (for linux) > > > > > > c:program files/kicad/doc (for windows) > > > > > > You have to drill down into whatever lang. you want. There is a help > > > folder and a tutorial folder. > > > > > > Do run through the tutorial a few times, as it takes a bit of practise to > > > get the hang of things, the key point to remember is that the pin names > > > and numbers must agree between the libs and modules. > > > > > > Also remember to save your libs and modules in your OWN directories, this > > > just safeguards against a new kicad version overwriting anything you have > > > done. > > > > > > > > > Andy > > > > > > > > > > > > On Fri, 03 Jul 2009 20:10:37 -0000 > > > "acidblue@" <sunblaster5@> wrote: > > > > > > > ok I think i'm beginning to see. > > > > Now i just need to find I tutorial on how > > > > to make/change modules. > > > > > > > > > > > > --- In [email protected], Andy Eskelson <andyyahoo@> wrote: > > > > > > > > > > The good grid size is one that matches the libs... > > > > > > > > > > Normally the default is fine. What can happen is that if you create > > > > > your > > > > > own parts, and use a different grid size then things don't align. > > > > > > > > > > As a silly example, say you set the grid to 55ml when designing the > > > > > part, and > > > > > still used 50ml for the normaly layout. That would cause all sorts of > > > > > problems. I've learnt to be very careful with grid sizes when > > > > > creating parts. :-) > > > > > > > > > > OK with ERC that's fine. It's probably a name mismatch as Alan > > > > > suggests. > > > > > > > > > > Dont forget that there very often there IS NOT a 1:1 relationship > > > > > between > > > > > a lib and mod. > > > > > > > > > > You could have a BC108, 2N3904, and any number of other transistors. > > > > > They > > > > > would all have the same footprints, so you would hope that they would > > > > > have the same pin names, i.e. ebc however some get numbered pins. Then > > > > > you have FETs, sgd pins rather than ebc but still the same footprint. > > > > > I've found diodes with pins 1 & 2 when a & k would be better. When I > > > > > find such problems I normally create another module and name it > > > > > something like TO92-ebc or LED-5mm-ak. > > > > > > > > > > Andy > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > On Fri, 03 Jul 2009 01:23:31 -0000 > > > > > "acidblue@" <sunblaster5@> wrote: > > > > > > > > > > > I always do an ERC check, till it gets to 0. > > > > > > Whats a good grid size? I always use the default,which i think > > > > > > is 50ml, should i try something smaller? > > > > > > BTW this always happens in kicad, i could never figure out why. > > > > > > > > > > > > > > > > > > > > > > > > > > > > > > --- In [email protected], Andy Eskelson <andyyahoo@> > > > > > > wrote: > > > > > > > > > > > > > > Every connection you make should have a wire in the rats nest. > > > > > > > > > > > > > > Have you run an ERC on the circuit? > > > > > > > The most common problem is that you forget to add junctions when > > > > > > > there > > > > > > > are more than one connection on a wire. (I'm always doing this) > > > > > > > > > > > > > > Another problem is that you mess up the grid size and the > > > > > > > connection does > > > > > > > not quite connect to a pin. > > > > > > > > > > > > > > In both cases the ERC check you throw up a list of bad > > > > > > > connections and > > > > > > > draw a little arrow where the problem is. > > > > > > > > > > > > > > > > > > > > > Andy > > > > > > > > > > > > > > > > > > > > > > > > > > > > On Thu, 02 Jul 2009 18:35:13 -0000 > > > > > > > "acidblue@" <sunblaster5@> wrote: > > > > > > > > > > > > > > > when i open Pcbnew, after CVPcb, i noticed some of my led's and > > > > > > > > resistors aren't connected, no rats nest. > > > > > > > > Shouldn't every module have a connection ?
