Author Topic: First 4 Layer PCB: Traces on each layer a good idea?  (Read 8092 times)

0 Members and 1 Guest are viewing this topic.

Online EEVblog

  • Administrator
  • *****
  • Posts: 32752
  • Country: au
    • EEVblog
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #25 on: July 24, 2020, 11:58:14 pm »
Quote
Video just for you!
Thank you so much! I can't believe that's actually happening  ;D
This helps me tremendously as I am just starting to get into more serious PCB layouts.

Glad to help. Thanks for the example.
I have plenty of other PCB layout videos as well.
 
The following users thanked this post: soFPG

Online langwadt

  • Super Contributor
  • ***
  • Posts: 2393
  • Country: dk
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #26 on: July 25, 2020, 12:31:07 am »
Any opinions on this? Tips & tricks are very much appreciated.
No ground planes yet. Traces on Layer 1, 3 and 4.

Those bypass caps are all wrong. The traces are way too long. It's like you places them in the wrong rotation around the chip and then just routed them because that's what it said to do.
EDIT: Oops, I mistook the image sensor for the FPGA. The FPGA is a QFP and the image sensor is the BGA. So I was talking about the image sensor bypass caps here.

I might record a 2nd channel video reviewing this, as I think this layout could lead to some good discussion.

I often start layout with placement of components using a temporary netlist where the bypass caps are connected to the right pins but
no connection to power, that way it much easier to see from the rast nets where the bypass caps should be

 
The following users thanked this post: Clear as mud, tooki

Online Siwastaja

  • Super Contributor
  • ***
  • Posts: 3726
  • Country: fi
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #27 on: July 25, 2020, 06:10:42 am »
Not such a great blanket idea. 0402's are harder to place and inspect by both hand and machine.
0402 is the size where you have to have 0402 specific assembly machines (with good yield), and that can often rule out a lot of cheaper assembly houses, cheaper older production lines, backyard operators etc.
I'd only use 0402 if you have to for density reasons. 0603 and 0805 for everything else.

This advice is from 2005, maybe 2010.

Today you would struggle to find an assembly house that has any problems whatsoever placing 0402. If you do find such (for example: a very large scale Chinese fab specialized in very low-tech, large numbers manufacturing), they definitely can't place either the FPGA or the image sensor, so the point is completely moot.

I use 0402 everywhere by default, and this includes placement-by-tweezers and home reflow.

Nowadays 0201 is the "decision point" which may limit the choice of fab and prevent using some cheapest ones, like 0402 was a decade ago.

Again, layout-wise it's important to use a passive size so that a passive that connects between two device pins does not span the width of 10 device pins, blocking all nearby routing. Not only for minimized loops, but also to simplify routing work.

0201 would be optimal for 0.5mm pitch devices, you could place them right next to the two pins without creating any obstacles for other routing, but 0201 is a bit tricky and iffy from the cheap assembly viewpoint, hence 0402.

Many devices like FPGAs and high pin count fast MCUs easily require a bypass cap every 15-20 pins on a 0.5mm QFP. If you use 0805 on that, the bypass caps take all the space along the edges, and you need to route almost all IO through vias to other layers because the top layer is blocked. Or you need to place the bypass caps on the bottom layer, an extra assembly step when 0402 caps would simply be next to the pins.
« Last Edit: July 25, 2020, 06:19:38 am by Siwastaja »
 
The following users thanked this post: Alex Eisenhut

Offline Rudolph Riedel

  • Contributor
  • Posts: 20
  • Country: de
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #28 on: July 25, 2020, 07:52:36 am »
Just saw the video. :-)

Is that a CH340 for the USB/UART converter?
I would use a FT230X.
Not only for the smaller package and to get rid of the crystal but also for quality.
Alternatively maybe the CP2102N.
 

Offline -gb-

  • Contributor
  • Posts: 29
  • Country: de
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #29 on: July 25, 2020, 10:01:21 am »
Greetings from Germany,
could you upload the Schematic please? I would give it a try.

Oh and generally:
How about a little forum-layout-contest?

Dave defines the components and uploads a schematic. Then everyone can try and afterward it will be discussed. Oh and it would be possible to define different design-goals. One can optimize for area, price, lower layercount, handsolderability, ...
 

Offline Neilm

  • Super Contributor
  • ***
  • Posts: 1489
  • Country: gb
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #30 on: July 25, 2020, 03:27:38 pm »
Not such a great blanket idea. 0402's are harder to place and inspect by both hand and machine.
0402 is the size where you have to have 0402 specific assembly machines (with good yield), and that can often rule out a lot of cheaper assembly houses, cheaper older production lines, backyard operators etc.
I'd only use 0402 if you have to for density reasons. 0603 and 0805 for everything else.

If you are designing for large scale manufacturing you may not have a huge choice - I have found over the last few years that even 0603 are becoming expensive as manufacturers are concentrating on the smaller packages making 0603 harder to get. This is really noticable if you use 1206 reistors for power / voltage requirement.
Two things are infinite: the universe and human stupidity; and I'm not sure about the the universe. - Albert Einstein
Tesla referral code https://ts.la/neil53539
 
The following users thanked this post: Siwastaja

Offline soFPG

  • Regular Contributor
  • *
  • Posts: 243
  • Country: de
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #31 on: July 25, 2020, 09:25:33 pm »
Quote
Is that a CH340 for the USB/UART converter?
Yes.

Quote
Not only for the smaller package and to get rid of the crystal but also for quality.
There are other variants of the CH340 series which also don't need an external crystal. Not so sure what you mean by "quality". CH340 ICs are used in a lot of Arduino clones for programming (so at least there is some kind of reliability).

I am using the CH340G variant as I have it laying around and I don't want to buy new ICs if there really is no point besides "Nice to Have".

Quote
Greetings from Germany,
Hi :)

Quote
could you upload the Schematic please?
Unfortunately, I am using Wuerth Electronic's Altium libraries for some of the parts and I don't know if I am allowed to re-distribute them.

If I am thinking about how much it would cost to hire an expert PCB designer per hour to help you with your PCB project (actually I don't know but it would probably be several hundred $) it becomes even more apparent how much value the video from Dave has (for me)!
« Last Edit: July 25, 2020, 09:31:49 pm by soFPG »
 

Offline -gb-

  • Contributor
  • Posts: 29
  • Country: de
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #32 on: July 25, 2020, 10:20:07 pm »
Quote
Unfortunately, I am using Wuerth Electronic's Altium libraries for some of the parts and I don't know if I am allowed to re-distribute them.

OK, but a Screenshot from the Schematic would also help. I just want to try how much this board can be optimised and if it can be done as a 2 layer board.
One point Dave did not discuss is the dcdc, the traces in the area look a bit too thin.
 

Offline asmi

  • Super Contributor
  • ***
  • Posts: 1793
  • Country: ca
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #33 on: July 26, 2020, 02:06:17 am »
Not such a great blanket idea. 0402's are harder to place and inspect by both hand and machine.
0402 is the size where you have to have 0402 specific assembly machines (with good yield), and that can often rule out a lot of cheaper assembly houses, cheaper older production lines, backyard operators etc.
I'd only use 0402 if you have to for density reasons. 0603 and 0805 for everything else.
That is absolutely not true nowadays. Maybe it was so a decade ago, like was said above, but these days 0402 is the default size for pretty much everywhere, except where other packages are required for one reason or another. And $200 stereo microscope makes manual placement of these a non-issue, unless you have really shaky hands. Heck I even place and solder 0201s manually, and even though it's kind of PITA compared to 0402, they have some important advantages which makes them indispensable in some cases.
 
The following users thanked this post: Siwastaja

Offline asmi

  • Super Contributor
  • ***
  • Posts: 1793
  • Country: ca
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #34 on: July 26, 2020, 02:13:56 am »
To OP: Remember this once and for all times - 4 layer board has TWO signal layers, not three or four. You can snake a slow trace or two on a power plane layer in a pinch, but otherwise these two should be left alone for power/ground.
Also - get you priorities right. First you place everything, then you route important traces first, and power is never an important trace (because you have power/ground planes, so all it takes is to drop a via, and you're done). Bypass caps have to be as small as you dare, and placed as close as you can to the power pins. The capacitance value of these caps is not that important, the package size is everything!
0402 passives can be bought at LCSC for like 5-10$ per reel of 10k components, so they are effectively free.
« Last Edit: July 26, 2020, 02:33:33 am by asmi »
 

Offline winniethepooh_icu

  • Contributor
  • Posts: 24
  • Country: england
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #35 on: July 26, 2020, 03:28:34 am »
Better stackup would be:
1 - traces + ground fill
2 - solid ground plane, no traces
3 - traces + ground fill
4 - traces + ground fill
You want at least one completely solid plane because otherwise you need to analyze the stitching on the entire board to ensure no unintentional slots.
Power planes are useless on 4 layers, and decoupling is best done by placing a large valued MLCC directly below every power pin on each IC.
On a 4 layer board the planes are very distant, and so stitching is extremely important! With a power plane you need a capacitor at every stitching point, and the stitching is very imperfect because of the via distance to the capacitor.

Before the OP runs off and changes it, look at OwO's profile text that says "RF Engineer"  ;D
The OP isn't even remotely close to needing anything like that.


You are absolutely incorrect.  The words "buck converter" in Owo's post should have been a clue.
Don't discourage people from exploring the right way to do something by posing as an expert in something which you are not.
 

Offline james_s

  • Super Contributor
  • ***
  • Posts: 14407
  • Country: us
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #36 on: July 26, 2020, 05:15:03 am »
Not such a great blanket idea. 0402's are harder to place and inspect by both hand and machine.
0402 is the size where you have to have 0402 specific assembly machines (with good yield), and that can often rule out a lot of cheaper assembly houses, cheaper older production lines, backyard operators etc.
I'd only use 0402 if you have to for density reasons. 0603 and 0805 for everything else.

I've accidentally bought 0402 parts a few times and they're indeed tiny. You sneeze and they fly off the table never to be seen again. Trying to assemble by hand is like trying to solder a grain of sugar to the board. 0603 is a nice size though, still compact but not so small that you can't pick it up with tweezers or see what it is without a magnifier.
 

Offline soFPG

  • Regular Contributor
  • *
  • Posts: 243
  • Country: de
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #37 on: July 26, 2020, 08:39:22 am »
Quote
Unfortunately, I am using Wuerth Electronic's Altium libraries for some of the parts and I don't know if I am allowed to re-distribute them.

OK, but a Screenshot from the Schematic would also help. I just want to try how much this board can be optimised and if it can be done as a 2 layer board.
One point Dave did not discuss is the dcdc, the traces in the area look a bit too thin.

It can be quite certainly done with 2 layers. But as I have said, JLCPCB's 2 layer process doesn't allow for thin enough traces to route the BGA.

Quote
0402 passives can be bought at LCSC for like 5-10$ per reel of 10k components, so they are effectively free.
5$ for each value doesn't sound free to me. Also, there is no way I'll use 10k components.

Why is everyone getting crazy about 0402 components if it makes no real difference?

P.S: I already bought 0603 LEDs because I ran out of 0805 ones  ;)

Quote
To OP: Remember this once and for all times - 4 layer board has TWO signal layers, not three or four.
I got contradicting answers at the beginning, this is why I routed it like that in the first place.
 

Online mariush

  • Super Contributor
  • ***
  • Posts: 4068
  • Country: ro
  • .
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #38 on: July 26, 2020, 09:04:04 am »
Was the switching regulator really necessary in the first place?

How much current is the macho2 consuming?  I see the camera sensor say up to 20mA, the microcontroller should be something like a few mA, if I were to guess that fpga shouldn't eat more than 100-250mA or so.

Seems like you could have managed just fine with a 250-800ma ldo on the board, bringing 5v down to 2.8v will not be really efficient but do you really care? you'll just have half a watt or something like that wasted as heat ... you have plenty of pcb space to dissipate that heat.
 

Offline soFPG

  • Regular Contributor
  • *
  • Posts: 243
  • Country: de
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #39 on: July 26, 2020, 09:06:48 am »
No, probably not. But this is one of the things I want to test with this board. I plan to eventually use larger FPGAs and I want to have a working switching power supply when I start with that design.
 

Online Siwastaja

  • Super Contributor
  • ***
  • Posts: 3726
  • Country: fi
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #40 on: July 26, 2020, 09:23:44 am »
To OP: Remember this once and for all times - 4 layer board has TWO signal layers, not three or four. You can snake a slow trace or two on a power plane layer in a pinch, but otherwise these two should be left alone for power/ground.

True, but OTOH, if you don't need controlled impedance on all routing layers, and don't have high-speed edge rates, you can treat it as three signal layers. Then you have only one pair where the ground layer is "right next" allowing impedances between 50-100 ohms without massively thick traces, and 2 of the signal layers are "lower speed" layers, with the respective ground layer quite far away. But it's still just about a millimeter or so; these "slow" layers are then equivalent to what you have in the sole signal layer of the plain old double layer design when you use one side as a ground plane; quite good actually!

This 3 signal layers, 1 ground layer is still massively better than trying to have some clever routing on all 4 layers, accidentally (or purposefully) chopping up the sole ground plane.

And it so happens, you tend to come up with all sorts of low-speed control signals, once you have already routed most of the board. Oh, that power supply enable signal! Oh, and that gate driver enable! What about this status LED and we needed one more pushbutton we forgot completely. Input battery voltage must be measured for safe auto-shutdown, forgot about that one. Oh and that I2C temperature sensor we completely forgot to route.

Borrowing the 3rd layer for that routing is sometimes a time-saver.

So if the budget prevents a 6-layer board, and the designer (or beginner, in this case) struggles doing the routing on just 2 layers of the 4-layer board, I would not hesitate to recommend borrowing the third one for routing. Of course, for critical high-speed signals, be extra sure there is a plane right next to these signals (not 1mm away) and use calculator tools to determine the trace width to get the required impedance, even approximately.
« Last Edit: July 26, 2020, 09:27:05 am by Siwastaja »
 

Online Siwastaja

  • Super Contributor
  • ***
  • Posts: 3726
  • Country: fi
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #41 on: July 26, 2020, 09:37:32 am »
Quote
0402 passives can be bought at LCSC for like 5-10$ per reel of 10k components, so they are effectively free.
5$ for each value doesn't sound free to me. Also, there is no way I'll use 10k components.

You really need only one value for 99% of the bypass work. 0402, at least 100nF, can be up to 1uF, X7R or at least X5R, 10V is OK. You can buy just some 500pcs, but 10000pcs may cost the same or $1 more, it depends.

This will be the part you will sprinkle everywhere, no need to buy many different sizes. If you come up with some IC which requires larger capacitance for some reason, you can just put a few in parallel. You have a simple and predictable BOM, and the fewest number of different components to stockpile! And you don't forget to buy the bypass caps for the project if you always use the same part.

Your existing part collections with many different sizes of 0805 parts are not wasted, they are useful for everything else than basic <=5V IC bypassing, where you need different sizes. Here, you need fairly low number of each size, so no stockpiling full reels.

Similarly, you may want to have one "generic pull-up/pull-down resistor" 0402 10kOhm or so, and one "generic series termination resistor" 0402 47ohms or so. These are parts you may end up using in quite large numbers, depending on what you are doing.

Quote
Why is everyone getting crazy about 0402 components if it makes no real difference?

But it makes a whole lot of difference, as explained carefully.

Dave giving very outdated and thus wrong advice sidetracked this discussion, and every time part size is discussed, someone who has problems handling small parts pops up. It's a meaningless argument; the only one who can definitely answer that is yourself. Try it. Give it a few good shots.

If you can't handle 0402 parts (most can), that's understandable, but you should give it a shot because it will make everything just easier for you, and the result will be better as well. The smaller parts you can handle, the easier the routing given some final size constraints and electrical constraints, and the bigger selection of components, especially modern ICs that make design work much easier by solving problems for you, are available.
« Last Edit: July 26, 2020, 09:45:55 am by Siwastaja »
 
The following users thanked this post: xlnx

Offline soFPG

  • Regular Contributor
  • *
  • Posts: 243
  • Country: de
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #42 on: July 26, 2020, 09:44:52 am »
Quote
But it makes a whole lot of difference, as explained carefully.
On the previous page, you said:

Quote
Well, likely not that much, in the end.

Quote
I suggest you don't post questions if you don't want to hear the answers.
I want to hear the answers. Sorry if my reply sounded rude. It was just based on your reply a day ago.
 

Online Siwastaja

  • Super Contributor
  • ***
  • Posts: 3726
  • Country: fi
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #43 on: July 26, 2020, 09:48:17 am »
Read the rest. I replied that I expect your layout to perform likely "good enough" power integrity and EMC wise even with the 0805 caps with nonoptimal routing, but you increase your margins by doing better work, and what's most important, you make your own life easier with a smaller part, routed closer. You will see it at the latest when you have a QFP, you place the caps on the top layer, and you have first placed those caps, and then start to route the rest of the signals going to the QFP! Try it with different cap sizes.

The key is, your design does not suck, but there is still room for improvement. Hence you get comments about things that are not super-critical but are still meaningful.
« Last Edit: July 26, 2020, 10:00:30 am by Siwastaja »
 
The following users thanked this post: soFPG

Offline soFPG

  • Regular Contributor
  • *
  • Posts: 243
  • Country: de
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #44 on: July 26, 2020, 09:57:53 am »
Thank you, it's just hard for me to bring all the different information from different people together. Some are saying, 0805 is okay, others are saying 0402 is necessary. Some are saying you have to have a power plane on a 4 layer board, others say it's not necessary.
I get the point that routing is easier with smaller parts. I guess I have to read a book about that.
 

Online Siwastaja

  • Super Contributor
  • ***
  • Posts: 3726
  • Country: fi
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #45 on: July 26, 2020, 10:02:11 am »
When in doubt, try things out. Yes it will take more time, but you will get a better understanding.

Getting completely accurate and totally non-conflicting information would be nice, but it's impossible because there is no single correct solution to everything. Everything depends on something.
 
The following users thanked this post: soFPG, xlnx

Online EEVblog

  • Administrator
  • *****
  • Posts: 32752
  • Country: au
    • EEVblog
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #46 on: July 26, 2020, 11:12:10 am »
So if the budget prevents a 6-layer board, and the designer (or beginner, in this case) struggles doing the routing on just 2 layers of the 4-layer board, I would not hesitate to recommend borrowing the third one for routing.

Yes, that is quite common to do. Same with other layer counts like 6 to 8, 8 to 10, etc. Just lay what signals you need to on the power plane layer and then flood fill the plane in as the last step.
 

Online EEVblog

  • Administrator
  • *****
  • Posts: 32752
  • Country: au
    • EEVblog
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #47 on: July 26, 2020, 11:15:03 am »
Thank you, it's just hard for me to bring all the different information from different people together. Some are saying, 0805 is okay, others are saying 0402 is necessary.

Anyone who is saying you need 0402 bypass caps for this design is not being practical, that is demonstrably wrong advice.

Quote
Some are saying you have to have a power plane on a 4 layer board, others say it's not necessary.

Again, not necessary for this design. But there is no need to route signals on the power plane in this design, you have a ton of room.
 
The following users thanked this post: soFPG

Online EEVblog

  • Administrator
  • *****
  • Posts: 32752
  • Country: au
    • EEVblog
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #48 on: July 26, 2020, 11:18:00 am »
Dave giving very outdated and thus wrong advice sidetracked this discussion

What part of my advice was "outdated and wrong"?
You do not need 0402 for this design. 0805 bypass caps will work just fine. I'd bet a large sum of money on it.
I'm not saying don't use 0402 parts, I'm just saying that you don't have to.
 

Online EEVblog

  • Administrator
  • *****
  • Posts: 32752
  • Country: au
    • EEVblog
Re: First 4 Layer PCB: Traces on each layer a good idea?
« Reply #49 on: July 26, 2020, 11:19:35 am »
Was the switching regulator really necessary in the first place?
How much current is the macho2 consuming?  I see the camera sensor say up to 20mA, the microcontroller should be something like a few mA, if I were to guess that fpga shouldn't eat more than 100-250mA or so.
Seems like you could have managed just fine with a 250-800ma ldo on the board, bringing 5v down to 2.8v will not be really efficient but do you really care? you'll just have half a watt or something like that wasted as heat ... you have plenty of pcb space to dissipate that heat.

Yes, I would also be questioning the need for that.
EDIT: Ah, read your reply. Fair enough.
 
The following users thanked this post: soFPG


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf