Electronics > Beginners
Why am not able to get a grasp of PCB designing?
Rerouter:
Had a play around trying to reduce how many headaches there where (e.g. trying to keep the switching node at least a little away from the USB differential, and how to lay that out with minimal crossing)
seems to me the best result is if you treat the chip like a switch mode converter first, keeping loop area as small as possible and all that fun, then running the USB in the order you have it assigned (even if the USB is just for signalling, my mind is still clinging to routing it out with minimal crossings,
Also had a play with your battery connection area to keep the connections as short as possible,
next steps from here would probably be to shift the micro more central, to keep those battery connections short, while keeping as much distance as possible from the inductor switching node and the usb pairs.
those 0201 components will be a right pain to solder, if you can, I would recommend larger parts for ease of assembly,
I should also mention, the trace width calculations can be cheated a little, sometimes it is better to have a thinner but shorter connection than a wider but longer one, the big one may reduce the amount of heat per unit distance, but a shorter connection reduces that distance.
thinkfat:
The correct land pattern is shown on p.83, if you used that one it's likely OK, but also the it's quite a huge component, 11mm x 10mm. Looking at their datasheet, you could likely go with a smaller device, like an SPM5050xxx. I've used Coilcraft XAL5030 inductors for switching converters with good results. For example, the XAL5030-222MEC, it's around 5mm x 5mm, could fit your design.
About flipping the transistors to the other side - well, you need to make up your mind, I would put each of the transistors closer to the USB receptacles they will switch power to, but keep in mind that you also need to route the sense wires. You need to develop a general idea of where certain nets should go. For example, you could decide that the high-current stuff should stay on the top layer and that you'll route the sense wires on the bottom.
It might be a good idea to route the VOUTP net as a beefy trace on the border of the PCB, out to the right and then up and then to the left along the top edge, and feed the mosfets from there. That keeps the power distribution out of the way of the USB signals that you also need to route. You could then drop the sense lines and the gate signals to the bottom layer of the PCB and route them back to the IC. They have no speed or current requirements and might not mind a few vias.
thinkfat:
--- Quote from: Rerouter on December 03, 2019, 10:31:27 am ---Had a play around trying to reduce how many headaches there where (e.g. trying to keep the switching node at least a little away from the USB differential, and how to lay that out with minimal crossing)
seems to me the best result is if you treat the chip like a switch mode converter first, keeping loop area as small as possible and all that fun, then running the USB in the order you have it assigned (even if the USB is just for signalling, my mind is still clinging to routing it out with minimal crossings,
Also had a play with your battery connection area to keep the connections as short as possible,
next steps from here would probably be to shift the micro more central, to keep those battery connections short, while keeping as much distance as possible from the inductor switching node and the usb pairs.
those 0201 components will be a right pain to solder, if you can, I would recommend larger parts for ease of assembly,
I should also mention, the trace width calculations can be cheated a little, sometimes it is better to have a thinner but shorter connection than a wider but longer one, the big one may reduce the amount of heat per unit distance, but a shorter connection reduces that distance.
--- End quote ---
That looks pretty good already. I agree the controller should be more central, close as possible to the battery protection circuit. but still positioned so that the display socket doesn't obstruct the USB traces. Close to the bottom would be good I think.
Also, I don't see a reason for putting all the high-power components on the bottom side, there's plenty of space between the USB receptacles to put e.g. the mosfets and there isn't much more that you need to place. As a general strategy I'd use "power distribution and usb signals on top layer, ground plane, slow signals and sensing on the bottom". The small jellybean stuff can go to the bottom side too.
redgear:
--- Quote from: Rerouter on December 03, 2019, 10:31:27 am ---Had a play around trying to reduce how many headaches there where (e.g. trying to keep the switching node at least a little away from the USB differential, and how to lay that out with minimal crossing)
seems to me the best result is if you treat the chip like a switch mode converter first, keeping loop area as small as possible and all that fun, then running the USB in the order you have it assigned (even if the USB is just for signalling, my mind is still clinging to routing it out with minimal crossings,
--- End quote ---
Thanks. I will try to do it again from scratch.
--- Quote ---Also had a play with your battery connection area to keep the connections as short as possible,
next steps from here would probably be to shift the micro more central, to keep those battery connections short, while keeping as much distance as possible from the inductor switching node and the usb pairs.
--- End quote ---
@thinkfat suggested I keep the inductor on the top layer but I find it is on the bottom layer in your design. Should I place it on the top layer?
--- Quote ---those 0201 components will be a right pain to solder, if you can, I would recommend larger parts for ease of assembly,
--- End quote ---
Bigger components takes more space, so I was thinking to go with reflow method.
--- Quote ---I should also mention, the trace width calculations can be cheated a little, sometimes it is better to have a thinner but shorter connection than a wider but longer one, the big one may reduce the amount of heat per unit distance, but a shorter connection reduces that distance.
--- End quote ---
Thanks for the tip...
--- Quote from: thinkfat on December 03, 2019, 10:36:36 am ---The correct land pattern is shown on p.83, if you used that one it's likely OK, but also the it's quite a huge component, 11mm x 10mm. Looking at their datasheet, you could likely go with a smaller device, like an SPM5050xxx. I've used Coilcraft XAL5030 inductors for switching converters with good results. For example, the XAL5030-222MEC, it's around 5mm x 5mm, could fit your design.
--- End quote ---
Yes, I used the same dimensions. Ok, I will try to look for components with smaller footprints. I tried using the Digikey filter before I started but sadly I did not find any.
--- Quote ---About flipping the transistors to the other side - well, you need to make up your mind, I would put each of the transistors closer to the USB receptacles they will switch power to, but keep in mind that you also need to route the sense wires. You need to develop a general idea of where certain nets should go. For example, you could decide that the high-current stuff should stay on the top layer and that you'll route the sense wires on the bottom.
--- End quote ---
Alright, I will redo it. Hope I develop these over time so I could do it right the first time.
--- Quote ---It might be a good idea to route the VOUTP net as a beefy trace on the border of the PCB, out to the right and then up and then to the left along the top edge, and feed the mosfets from there. That keeps the power distribution out of the way of the USB signals that you also need to route. You could then drop the sense lines and the gate signals to the bottom layer of the PCB and route them back to the IC. They have no speed or current requirements and might not mind a few vias.
--- End quote ---
Ok, let me try this.
Thanks.
redgear:
--- Quote from: thinkfat on December 03, 2019, 10:36:36 am ---For example, you could decide that the high-current stuff should stay on the top layer and that you'll route the sense wires on the bottom.
--- End quote ---
If I choose to have the high current stuff at the top, should also flip the battery protection to the top layer?
--- Quote ---It might be a good idea to route the VOUTP net as a beefy trace on the border of the PCB, out to the right and then up and then to the left along the top edge, and feed the mosfets from there.
--- End quote ---
If I am going to do this, can I remove the net-ties?
Navigation
[0] Message Index
[#] Next page
[*] Previous page
Go to full version