Thanks for your suggestion. You're right that the connected power rail does not override the pin name on these logic chips.
Another solution might be to create a logic component with the relevant gates plus a power block that could be connected to the appropriate rail(s) and tucked out of the way (and associated on the schematic with the decoupling capacitor). Regards, Robert. On 16/03/2010 16:13, Andy Eskelson wrote: > You can manually connect the power if you enable show hidden pins in > eeschema, but that means that you have to manually connect all the power > pins up. What I don't know because I've never tried it, is if that > over-rides the pin names for DRC. I would guess not. > > In practise the solution is very simple. > > Duplicate the library part and change the name of the power pins to > something else. For example change Vcc to +5V, then you can use a +5V > power port which will connect to just that chip. > > Obviously you save the part under a different name, then that part will > connect to the new power net. > > You could also just identify the pins as power in, and not give them a > special name& untick the not drawn box, this would meant that you need > to manually connect them. For small circuits this is not much of a > problem, however it can get messy if you have a reasonable number of IC's > to connect. > > > Andy > > > > > > On Tue, 16 Mar 2010 14:07:21 +0000 > Robert<birmingham_spi...@gmx.net> wrote: > >> Thanks for your replies Carl and Andy. >> >> Speaking for myself, I have designs that use two instances of the same >> micro, with each instance on a different supply rail. These micros all >> have a power pin named VCC and I have no problems with ERC, so Kicad >> isn't covertly connecting my VCC pins together. >> >> The OP (Mark) wants to have logic chips on two different supply rails, >> but it seems that Kicad joins up all the hidden pins marked Vcc, even if >> you connect the power pin to a different rail. Is the critical factor >> that the pins are hidden, is it that the name case sensitive, or is it a >> feature of multi-part components? It's not that the pin doesn't have a >> number, because the logic chip symbols have both name and number >> specified for the power pins (like the symbols I have created for >> myself). What is the critical thing that Mark has to change to allow >> him to connect two logic chips to two different supply rails. >> >> Regards, >> >> Robert. >> >> >> >> On 16/03/2010 11:14, Andy Eskelson wrote: >>> Vcc IS the power to the chip, U2A in this case. >>> so why have you connected +5V to it as well? >>> >>> DRC is detecting that you have effectively shorted VCC to a different 5V >>> supply as well, and is complaining about it. >>> >>> Power flags are defined as power out pins, and you only have one power >>> out on a power net,m if you add a second power flag DRC will complain >>> about that as well. >>> >>> I think you are assuming that you need to connect 5 volts to the chip, >>> and so are adding the +5V port, which is another independent supply net. >>> Hence the confusion. >>> >>> The system works as has been mentioned by the power port names. When a >>> device has a power pin with a specific name, AND you set the pin to be >>> invisible you DO NOT need to connect anything else to it. As soon as you >>> put a power port with the same name onto the circuit diagram, that port is >>> automatically connected to all device power pins with the same name. >>> >>> >>> A power net needs to be energised or DRC will complain. That can be done >>> in two ways. Either a device such as a regulator can have a power out >>> pin, which will indicate that it is energised, OR you add a power flag, >>> which simply says that the net is energised. You use power flags in >>> situations where you are connecting an external power source to your >>> circuit via a connector, flying leads and so on. >>> >>> The one oddity is that GND is considered a power out type net as well, so >>> it also needs energising with a power flag. >>> >>> logic IC's have generally had their power pins identified by names >>> rather than the voltage, so you have Vcc Vss Vdd and so on. >>> >>> When you run into such chips, the same will apply, power ports of the >>> same name are already considered to be connected to the physical supply >>> >>> Andy >>> >>> >>> >>> >>> >>> On Mon, 15 Mar 2010 16:13:15 -0000 >>> "mtheling"<p...@swapout.de> wrote: >>> >>>> Hi Robert, >>>> >>>> if I connect for example a net "+5V" to a component U2A which has an VCC >>>> input as invisible pin, I see that in PCBnew the pin is connected to the >>>> "+5V" net as soon as I set an Powerflag to +5V. >>>> But the ERC check in eeschema states this as error : >>>> ErrType(5): Conflict problem between pins. Severity: error >>>> @ (5,1000 ",6,7500 "): Cmp #FLG01, Pin 1 (power_out) connected to >>>> @ (4,4000 ",6,7500 "): Cmp #FLG06, Pin 1 (power_out) (net 3) >>>> >>>> If I don't connect a Powerflag to the "+5V" net, in PCBnew the Power Pin >>>> of U2A is still connect to the VCC net and not to "+5V" as set in the >>>> schematic. >>>> Please see schematic for example: >>>> http://www.swapout.de/example_schematic.pdf >>>> >>>> What I am doing wrong? >>>> >>>> Thank you, >>>> >>>> best Regards, >>>> Mark >>>> >>>> >>>> >>>> >>>> ------------------------------------ >>>> >>>> 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 >>>> >>>> >>>> >>> >>> >>> ------------------------------------ >>> >>> 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 >>> >>> >>> >>> >>> >>> >>> No virus found in this incoming message. >>> Checked by AVG - www.avg.com >>> Version: 9.0.790 / Virus Database: 271.1.1/2749 - Release Date: 03/15/10 >>> 19:33:00 >>> >> >> ------------------------------------ >> >> 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 >> >> >> > > > ------------------------------------ > > 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 > > > > > > > No virus found in this incoming message. > Checked by AVG - www.avg.com > Version: 9.0.790 / Virus Database: 271.1.1/2750 - Release Date: 03/16/10 > 07:33:00 >
No virus found in this outgoing message. Checked by AVG - www.avg.com Version: 9.0.790 / Virus Database: 271.1.1/2750 - Release Date: 03/16/10 07:33:00
