| Electronics > Beginners |
| Many errors on DRC check for Schematic KiCad |
| (1/4) > >> |
| redgear:
I just completed a schematic and when I run the DRC, I get many errors. All the errors are either Pins not being driven or conflict problem between pins. I made a custom symbol for a part and I should have messed up while assigning the type of pins which is causing the conflict errors. I assume I can ignore them. What is with the pins not being driven? I checked all connections and they are properly connected. I'm attaching my schematic and the error log. Can anyone help me with it? Thanks |
| jhpadjustable:
--- Quote ---ErrType(3): Pin connected to other pins, but not driven by any pin @(242.57 mm, 134.62 mm): Pin A9 (Power input) of component J6 is not driven (Net 1). --- End quote --- Place a PWR_FLAG on the VBUSC net. Ditto for pin 2 of U1. Also the other VBUSes. --- Quote ---ErrType(5): Conflict problem between pins. Severity: error @(82.55 mm, 63.50 mm): Pin 27 (Power output) of component U2 is connected to @(82.55 mm, 99.06 mm): pin 9 (Power output) of component U2 (net 34). --- End quote --- Pin 27 (and 28) are not power outputs. They are just current sense leads. Mark them input or passive. --- Quote ---ErrType(5): Conflict problem between pins. Severity: error @(82.55 mm, 99.06 mm): Pin 9 (Power output) of component U2 is connected to @(82.55 mm, 101.60 mm): pin 14 (Power output) of component U2 (net 34). ErrType(5): Conflict problem between pins. Severity: error @(82.55 mm, 101.60 mm): Pin 14 (Power output) of component U2 is connected to @(62.23 mm, 105.41 mm): pin 13 (Power output) of component U2 (net 34). --- End quote --- Same here. These also should be connected to your power bus. Leave a reminder for yourself with the text tool if you care to Kelvin-connect them during layout, but I'm not sure it matters a whole lot if you make your VOUT traces nice and wide. I've never seen that chip before and can't find data, so I can't be sure. Have you given up on the IP5328, then? You shouldn't put more than one label on a single net (VOUTA, VOUTC, etc.) or the extras might get pruned on the way to layout. --- Quote ---ErrType(5): Conflict problem between pins. Severity: error @(82.55 mm, 73.66 mm): Pin 4 (Output) of component U2 is connected to @(82.55 mm, 78.74 mm): pin 2 (Output) of component U2 (net 53). --- End quote --- SW pins are bidirectional, for both charging and discharging. Adjust your symbol accordingly. You can assign just one pin to a signal, instead of multiple shield pins. In the footprint, you can then assign that same pin number/name to multiple pads, which will all be connected to the net or no-connect, as appropriate. |
| redgear:
--- Quote from: jhpadjustable on November 22, 2019, 06:03:34 am ---Same here. These also should be connected to your power bus. Leave a reminder for yourself with the text tool if you care to Kelvin-connect them during layout, but I'm not sure it matters a whole lot if you make your VOUT traces nice and wide. I've never seen that chip before and can't find data, so I can't be sure. Have you given up on the IP5328, then? --- End quote --- When I was mid-way building the PCB with IP5328, I found this IC with better features so I started redoing the whole design with this IC. This a SW6208 from ismartware. I will attach the datasheet below. --- Quote ---You shouldn't put more than one label on a single net (VOUTA, VOUTC, etc.) or the extras might get pruned on the way to layout. --- End quote --- Ok, will remove them. --- Quote ---You can assign just one pin to a signal, instead of multiple shield pins. In the footprint, you can then assign that same pin number/name to multiple pads, which will all be connected to the net or no-connect, as appropriate. --- End quote --- The shield pins are getting connected to the ground. Can I use the same pin number as GND for the pads and remove the shield pins from symbol? Thanks |
| jhpadjustable:
--- Quote from: redgear on November 22, 2019, 09:14:01 am ---When I was mid-way building the PCB with IP5328, I found this IC with better features so I started redoing the whole design with this IC. This a SW6208 from ismartware. I will attach the datasheet below. --- End quote --- Where? --- Quote ---The shield pins are getting connected to the ground. Can I use the same pin number as GND for the pads and remove the shield pins from symbol? --- End quote --- Bad idea. Shield should be tied to ground only at the upstream e- oh, wait, that's you. ;D I still advise against combining them in the symbol, since the pins serve very distinct functions and you want to avoid passing current through the shield. Any noise on it will then be radiated instead of contained inside the cable. You should connect the others to ground, but you'd definitely want to leave the charging port facing upstream (J3?) non-connected. (EMC greybeards can please tell me if I'm full of it) |
| redgear:
--- Quote from: jhpadjustable on November 22, 2019, 09:45:37 am ---Where? --- End quote --- Oops. I forgot to attach it. I am attaching it with this reply. --- Quote ---Bad idea. Shield should be tied to ground only at the upstream e- oh, wait, that's you. ;D I still advise against combining them in the symbol, since the pins serve very distinct functions and you want to avoid passing current through the shield. Any noise on it will then be radiated instead of contained inside the cable. You should connect the others to ground, but you'd definitely want to leave the charging port facing upstream (J3?) non-connected. (EMC greybeards can please tell me if I'm full of it) --- End quote --- Alright. But the datasheet has the shield pins connected to GND on the J3 port. |
| Navigation |
| Message Index |
| Next page |