next topic »

[Reply #15 on:]

"One end of the PCB could be the power end, both sides - whilst the other end would be control, both sides. "

That's what I was saying in #9.

I had misunderstood what you meant, and thought you were implying that I should put all my components on one side, and use the other layer of the PCB for routing traces.

Thank you!

EDIT - I have tens and tens of 5v and ground connections on the control end of my board, given these are away from all the power ICs the other side of the board, would it be appropriate or acceptable to have some sort of plane system on the control end of my board?

[Reply #16 on:]

I do.  The star approach is great, but when you have multiple components requiring power and ground connections, it becomes less and less feasible to home-run each one.  So, you prioritize.  Anything high-current gets its own run.  A bunch of similar things (like decoupling caps) can share a ground fill that has a single run back to the main ground point, etc.  You just have to get a feel for what is a reasonable amount of isolation with real benefits, and what is pointless overkill that makes layout impossible.

[Reply #17 on:]

The "star" grounding scheme looks good on paper, but quickly falls apart in real-world implementation, especially when doing complex PCB design. 
(Now, if you're doing point-to-point wiring, yeah, star-grounding is your friend. But we're not building vacuum tube amps here.)

I've had designs that called for separate analog and digital grounds but in the end, I just combined them all and made judicious use of ground planes on both top and bottom layer. Even amplifying weak analog signals 2000x voltage gain, there's no noise in the system (even with several relays being energized, SPI, etc running on the board.)

It also helps to confine analog and digital circuitry on their own sections of the board (if using a single board).... maybe even design it so it's two separate sections, (each with their own ground plane), and separated from each other by "moating" and just connect the grounds at a single point.

Another option is use (2) boards, and separate your logic board from the driver board. Just connect both boards with a ribbon cable. Distance is also your friend.

[Reply #18 on:]

I would use as much free area top & bottom for ground polygon as you can.
The two layers also provide some additional capacitance for decoupling.
Layout start with smart parts positioning. I find eagle will do a pretty good autorouting
if you have good parts placement to start. Then you add a ground via here & there,
maybe tweak a trace here & there to let the ground fill more area, etc.

[Reply #19 on:]

Thanks for all the input so far, here are some screenshots of my layout - well, part placement at least.

So, the d-pak packages on the left hand side are power switching FETs / IGBTs. The gate drivers are the small ICs between the rows. The IGBTs subject to a large inductive spike are the top row, top and bottom layers. The h - bridge is the through hole 11 pin vertical package.

My power supply, i.e. regulator, fuses, tranzorb, caps etc is the is central where the two horizontal d-paks are. Underneath however is a general purpose low side driver chip to configure which external relays should be powered. These will only switch during power up / off really.

I wanted to move the power supply away from the IGBTs a little, but the ICs to the right of my power supply are conditioning ~10kHz AC signals, converting USB to UART, reading thermocouples etc.

Bottom right is a flash IC, latch & external RAM - I've tried to keep these as far away as possible as random memory corruptions are not something I'm keen on getting. The two ICs underneath the MCU are SPI devices, so I'm hoping there's not an issue there with noise? The jumpers are to select between external filters for these two ICs, and i've left room around there to route signals over to the left hand side gate drivers.

I've still got ~40 resistors, ~20 caps to pull on to the board from outside of the outline, but these are small 0603 parts, as are the ones present currently on the board.

Does anybody have any recommendations, comments, criticisms (constructive of course, this is the first PCB i've laid out, and my first venture into SMD - all my other projects have just been through hole on vero board)?

I would use as much free area top & bottom for ground polygon as you can.

Earlier on in the thread however, I was told I should avoid doing this as it will help interference get in to the ground. Or would that only typically be the case if I had a power component on the other side of the board, and I put a ground plane on the other?

Top and bottom, together -



Top -



Bottom -

[Reply #20 on:]

I can see a potential problem with using global fill, in that it violates the star-grounding
idea.

Is this diagram the same thing we've been talking about for the past few days? I don't
see anything about separate power input for the h-bridge, or main caps. I was thinking
of seeing something more like,

http://www.robotshop.com/Images/pololu-trex-jr-motor-controller-detail.jpg
http://www.skpang.co.uk/catalog/images/robotics/motor_drive/0J111.600.jpg

[Reply #21 on:]

I can see a potential problem with using global fill, in that it violates the star-grounding
idea.

What I proposed, is the left side of the board would be star grounded, whilst the right hand side - which is just control circuitry - would have planes due to the number of 5v and ground connections required.

Is this diagram the same thing we've been talking about for the past few days?

Absolutely

I don't see anything about separate power input for the h-bridge, or main caps

On the 60 way connector to the board, I'll have two power in pins, and 2 ground pins. One 'set' will supply all the lower power devices, the other will supply the noisy devices and these will star back to their own ground pin.

C46 is the 220uF main cap, but I've just realised my 1uF h-bridge cap is a small 0603 cap, C7 - i'll change that to another can-type electrolytic.

I just wanted to show my main component layout to catch and potential problems early...

[Reply #22 on:]

That's what I thought. First off, you have to make sure that the pins of that connector
can handle the current levels. Secondly, I would locate the h-bridge right next to the
connector, rather than on the other side of the board, and of course, use wide pcb
traces - as shown in the links I gave.

[Reply #23 on:]

It looks like male into female headers are rated at 3A, but I'm not mating them with female headers - instead, they'll be soldered into holes on a small board at 90 degrees that will house the actual connectors, then the whole lot slots into an aluminium enclosure. So given the cross area of the headers, I'm sure they'll cope with more 3A @ ~ 14V.

I was thinking of moving the bridge up the where the power supply is too, but I was a little worried about sticking the bridge right next to the small ICs in the top right... They're the sensitive ones.

I'll have a jig about, see what I can come up with...

EDIT - Just thought, with the bridge near to the headers, I can also save on power trace width by running them on both sides from the same bridge pin, to the same header pin.

[Reply #24 on:]

What you notice is, on the links I gave, they have a nice segregation of the different
parts of the board, and the motors have their own connectors separate from the
logic connectors. But you have to do what you have to do, and see how it goes. The
further away from the connector that the h-bridge is, the more possible noise it's
traces can propagate to the rest of the pcb cktry.

[Reply #25 on:]

But you have to do what you have to do, and see how it goes.

I think that'll dictate a lot of things with this board!

The further away from the connector that the h-bridge is, the more possible noise it's
traces can propagate to the rest of the pcb cktry.

Well! Take a look at the reworked version, first pic - both layers. Second, top layer. Third, bottom layer.

I did a quick autoroute, without changing any settings, and with no connections from the ICs to the headers. It ended up with about 300 vias - now, inexperience here, would that be because I've got so many components on a two sided PCB, or because the layout is far from ideal?

I know a lot of these are probably vague ideas, but it's good to be steered in the right direction still... and once again - thank you hugely for your help so far, everybody.