Author Topic: Routing 4 layer boards  (Read 14052 times)

0 Members and 1 Guest are viewing this topic.

Offline Simon

  • Global Moderator
  • *****
  • Posts: 14986
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Simon's Electronics
Routing 4 layer boards
« on: May 07, 2017, 08:06:05 am »
I am trying to do my first 4 layer board in Proteus. This is proving to be a bit of a nightmare. Okay I’ll admit I have tried to make the auto router work and it does not seem to get it even though I have tried to specify routing pairs et cetera. The idea is to have the bottom layer as a ground plane and the top layer has mostly a ground plane carrying only power stuff that I manually route. Obviously the components all sit on the top layer as surface mount parts so they are going to need a via nearby and a short trace in order to get the connection into the middle pair of layers. I have also tried creating 2 types of via. One that goes through all 4 layers and one that goes from the top layer and only through the 2 internal layers. This via is not being used only the complete through-hole via is used. It also routes all over the top layer before trying to use the inner layers. Am I missing something significant or is the auto route the not really capable of doing for layers like this?

I’m also at a loss as to how I would choose to use a specific via while I am manually routing. Or indeed how do I choose which layer I am going to switch to.
 

Offline blueskull

  • Supporter
  • ****
  • Posts: 13759
  • Country: cn
  • Power Electronics Guy
Re: Routing 4 layer boards
« Reply #1 on: May 07, 2017, 08:19:34 am »
Most cheap PCB services only do through vias (from top to bottom). From top to inner layer is called blind vias, and from inner to another inner is called buried vias. Both are expensive process.
If you have any requirements on signal quality and routing density, do not use autorouter.
If you have any requirements on signal quality and routing density, do not use autorouter.
If you have any requirements on signal quality and routing density, do not use autorouter.
 
The following users thanked this post: daqq

Offline Simon

  • Global Moderator
  • *****
  • Posts: 14986
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Simon's Electronics
Re: Routing 4 layer boards
« Reply #2 on: May 07, 2017, 08:24:15 am »
I am using PCB cart. As far as I am aware they do do blind and buried via types.

I don't have any special requirements of the routing, there is nothing high-speed et cetera I'm simply trying to avoid EMC problems so am trying to keep anything that might be emitting inside the board.
 

Offline blueskull

  • Supporter
  • ****
  • Posts: 13759
  • Country: cn
  • Power Electronics Guy
Re: Routing 4 layer boards
« Reply #3 on: May 07, 2017, 08:31:23 am »
I've never seen ANY low cost PCB fabs offer free blind/buried vias. You better send them an email to confirm. From their website, their prototyping service doesn't offer blind/buried vias. You have to quote manually using their standard PCB service.

http://www.pcbcart.com/article/content/PCB-prototyping-vs-standard-PCB.html
 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 14986
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Simon's Electronics
Re: Routing 4 layer boards
« Reply #4 on: May 07, 2017, 08:36:04 am »
Yes their prototyping does not do blind/buried, as it also has limitations on number of layers and copper weights. I suspect that prototype boards are made on standard setups so that they can get lots of peoples boards on one tool, if they offered all options it would become impossible to group anyones design or they would end up with an expensive process to cover a few designs but that also applies to designs that should be cheaper breaking the "prototype" model. On production orders you are payinf for the tool and are keeping ownership of it so I guess they do as you want and charge you for it. Adding one blind via put the price up by about 15%
 

Offline mc172

  • Frequent Contributor
  • **
  • Posts: 318
  • Country: gb
Re: Routing 4 layer boards
« Reply #5 on: May 07, 2017, 09:31:20 am »
Unless you're working up at around 6 GHz and beyond, fully stacked vias aren't going to radiate anything or be particularly susceptible to RF. Blind vias are incredibly expensive and completely unnecessary for 99% of the time that people use them. I routinely use fully stacked vias up to 3 GHz. I don't work above 3 GHz much but doubt it would start to become a problem until at least double that.
If you are working up there in microwave voodoo land, you've got more to worry about than vias, such as the slot antenna formed by the thickness of the substrate material.
 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 14986
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Simon's Electronics
Re: Routing 4 layer boards
« Reply #6 on: May 07, 2017, 09:43:39 am »
Well I'm not too fussed about blind via's its more about trying to understand how to use proteus, it supposedly chooses the shortest via but then is clearly not doing so. Going for faraday cage style routing cannot be done with the autorouter. I guess if I manually put a via next to each component and force all routing to be on the inner 2 layers this would work.
 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 14986
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Simon's Electronics
Re: Routing 4 layer boards
« Reply #7 on: May 07, 2017, 09:49:47 am »
Unless you're working up at around 6 GHz and beyond, fully stacked vias aren't going to radiate anything or be particularly susceptible to RF.

This also depends on the class you are trying to pass. I have been told of an AVR held in reset failing EMC and all that would have been running would have been the clock inside the chip awaiting programming commands.
 

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 4621
  • Country: au
  • Question Everything... Except This Statement
Re: Routing 4 layer boards
« Reply #8 on: May 07, 2017, 10:29:50 am »
From what i can see by searching for it, the EMC issues with AVR's where primarily due to using a piezo susceptible ceramic capacitor on the reset line, and leaving inputs floating, failing around 1.3KV, while needing to pass 2KV

Oddly enough my searches turned up that the mega 128's SRAM does not clear on reset, atleast until VCC is below 0.3V, meaning part of the EMC susceptibility can be software related by not zeroing values after reset. I would assume this quirk would exist in similar models.
 

Offline mc172

  • Frequent Contributor
  • **
  • Posts: 318
  • Country: gb
Re: Routing 4 layer boards
« Reply #9 on: May 07, 2017, 10:31:35 am »
I appreciate that it doesn't help you use Proteus. Is the answer don't use the autorouter?:P
 

Offline mikeselectricstuff

  • Super Contributor
  • ***
  • Posts: 12135
  • Country: gb
    • Mike's Electric Stuff
Re: Routing 4 layer boards
« Reply #10 on: May 07, 2017, 12:45:20 pm »
Do not even think of using an autorouter.
More so if you are not experienced as you won't know how to set it up correctly. It will be a waste of time. 
Do not use blind or bured vias unless you absolutely need to - it adds cost and is not supported by most cheap services. Even where supported they tend to be only between the 2 inner layers due to the way the boards are made, which in practice isn't as useful as 1-2 and 3-4, which is a more expensive process.
Chances are 6 layers with through vias will be a similar cost to 4L with blind/buried vias.

On a 4L, one inner layer is usually dedicated to ground - either as a plane layer or a fill with a few tracks if necessary. In some cases you can get ground and post of power on one layer.
If you have to get power to lots of places, or have high power or low inductance requirements, the second inner layer is typically used for power. Again either as a complete plane or most of it filled with odd tracks you can't fit on other layers.
if you're very pushed for density (especially on through-hole PCBs) or need to maximise EMC performace, putting planes on the outer layers is sometimes done, but less so nowadays as you need the space for SMDs. It also makes PCBs basically impossible to track-hack.

 For a SMD layout you need the outer layer ( both if double sided) for parts so you shouldn't be relying on putting planes there.
The "default" starting position would be inner layers for ground and power, and see how you get on from there. By all means add surface fills in unused areas when you're done, but to start with, work on the assumption that  you won't be able to do that.
 
And never forget the three most important things to get a good layout:
Placement
Placement
Placement



Youtube channel:Taking wierd stuff apart. Very apart.
Mike's Electric Stuff: High voltage, vintage electronics etc.
Day Job: Mostly LEDs
 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 14986
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Simon's Electronics
Re: Routing 4 layer boards
« Reply #11 on: May 07, 2017, 02:55:48 pm »
From what i can see by searching for it, the EMC issues with AVR's where primarily due to using a piezo susceptible ceramic capacitor on the reset line, and leaving inputs floating, failing around 1.3KV, while needing to pass 2KV

Oddly enough my searches turned up that the mega 128's SRAM does not clear on reset, atleast until VCC is below 0.3V, meaning part of the EMC susceptibility can be software related by not zeroing values after reset. I would assume this quirk would exist in similar models.

it all amounts to the same thing EMC wise, the processor would stop working when pulled into reset but even then what is going on, on the chip can cause it to fail an EMC
 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 14986
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Simon's Electronics
Re: Routing 4 layer boards
« Reply #12 on: May 07, 2017, 03:02:51 pm »
Do not even think of using an autorouter.
More so if you are not experienced as you won't know how to set it up correctly. It will be a waste of time. 
Do not use blind or bured vias unless you absolutely need to - it adds cost and is not supported by most cheap services. Even where supported they tend to be only between the 2 inner layers due to the way the boards are made, which in practice isn't as useful as 1-2 and 3-4, which is a more expensive process.
Chances are 6 layers with through vias will be a similar cost to 4L with blind/buried vias.

On a 4L, one inner layer is usually dedicated to ground - either as a plane layer or a fill with a few tracks if necessary. In some cases you can get ground and post of power on one layer.
If you have to get power to lots of places, or have high power or low inductance requirements, the second inner layer is typically used for power. Again either as a complete plane or most of it filled with odd tracks you can't fit on other layers.
if you're very pushed for density (especially on through-hole PCBs) or need to maximise EMC performace, putting planes on the outer layers is sometimes done, but less so nowadays as you need the space for SMDs. It also makes PCBs basically impossible to track-hack.

 For a SMD layout you need the outer layer ( both if double sided) for parts so you shouldn't be relying on putting planes there.
The "default" starting position would be inner layers for ground and power, and see how you get on from there. By all means add surface fills in unused areas when you're done, but to start with, work on the assumption that  you won't be able to do that.
 
And never forget the three most important things to get a good layout:
Placement
Placement
Placement


A common practice these days for EMC is to use the outer layers as ground (I'm sure one could be power with no adverse effects) and run everything inside thus shielding it. Obviously you need a small trace on the part itself to go to a via very close by but after that it's all inside minimizing any length of trace that could act as a transmitter.

For real sensitive stuff I'd be tempted to run a row of vias around the edges of the board whilst using both outer layers as ground ;). in my case I plan to be caging the whole board anyway so traces on the top layer are not a problem but I am also just messing with settings trying to learn how to use Proteus.

Placement is indeed important and i spend a lot of time on it often using the auto router just to see how well I have done by eyeing up the complexity of the board layout. I generally undo it again and move stuff around and once happy I route power and sensitive stuff first then let the auto-router take care of what little is left.
 

Offline hammy

  • Supporter
  • ****
  • Posts: 437
  • Country: 00
Re: Routing 4 layer boards
« Reply #13 on: May 07, 2017, 03:58:26 pm »
A common practice these days for EMC is to use the outer layers as ground (I'm sure one could be power with no adverse effects) and run everything inside thus shielding it. Obviously you need a small trace on the part itself to go to a via very close by but after that it's all inside minimizing any length of trace that could act as a transmitter.

There are four requirements:
1. Decoupling
2. EMC-Immission/-emission
3. Signal-Integrity
4. Self-Interference

A layer-stackup like this:
GND/SIGNAL/SIGNAL/GND
or:
GND/SIGNAL/SIGNAL/VCC
isn't effective for at least three of these four requirements.

Decoupling: If VCC and GND are not on adjacent layers the capacetive effect is impossible by means.
EMC: The VCC layer isn't next to a GND layer. One signal layer in this stack-up is not next to GND. VCC will radiate.
Signal-Integrity: Bad if another Signal layer is between Signal and Gnd-Layer.

Only boards with 6 or more layer can fulfill all requirements. 4 or less layer are always a compromise. A stack-up described above is the worst possibility.

Consider something like SIGNAL/GND/VCC/SIGNAL or SIGNAL/GND/SIGNAL/VCC but - maybe it sounds strange - PCBs with GND and/or VCC on outer layers are never good regarding EMC. It is better to shield the board by edge plating.

Cheers
hammy
« Last Edit: May 07, 2017, 04:04:11 pm by hammy »
 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 14986
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Simon's Electronics
Re: Routing 4 layer boards
« Reply #14 on: May 07, 2017, 04:09:16 pm »
coming from a 2 layer board where you still would not have protection from self interference or signal integrity. All I am doing is putting a screen around an existing 2 layer PCB. EMC failures happen when traces that have no shielding carry varying currents/voltages usually with high speed swings. I'm not sure how GND-Signal-GND-Signal shields that outer signal layer and how having a ground plane under it stops it emitting other than the fact that the signal may go to ground rather than emit into free space. Obviously at the end of the day component leads are still exposed but I plan on shieldng the overall board anyway.
 

Offline hammy

  • Supporter
  • ****
  • Posts: 437
  • Country: 00
Re: Routing 4 layer boards
« Reply #15 on: May 07, 2017, 07:17:23 pm »
All I am doing is putting a screen around an existing 2 layer PCB.

But what about board-thickness, prepreg, epsilon-r, return path and core? Have a look into this document or this document.
(There are more documents from EMC labs out there, a lot of research about this topic.)

Don't think about GND-layers, think more about reference planes. Not only GND-planes offer a return path. You want to keep your signal close to their reference plane with a constant impedance. Also proper decoupling is needed.

Something to think about: The idea about GND-layer on the outer layers of a PCB is nothing new. But in all these years, with all these smart guys out there, no one is doing this (*). Also in HS-design classes something like this is not taught.

A PCB with SMT and GND-layer on the outside needs way more vias. This is not the best practice regarding density and signal integrity. If a signal changes reference plane it needs a path for it's return current nearby. With two GND-planes you can us a via connecting these two planes. With a GND-plane and a VCC-plane you need a capacitor and two via nearby. All not good regarding signal integrity and more board space.
Anyway, theoretically two GND-planes on the outside could reduce EMC. But in reality it is not worth the effort because components on this GND-layer consume all space. If your layout and design is so bad regarding EMC-emission that you need the GND-layers on the outside, you made something wrong.

What do books like "HS Design Black Magic" from Johnson and "Signal and Power Integrity" from Bogatin say about this? I'm not sure, but I don't remember they recommend this.

Simon, give it a try. Why not? Nothing bad about trying new stuff. But be aware it is not best practice.  And always ask yourself "What would Johnson or Bogatin do?" or "What was taught in this design-class?" or "Am I really smarter than all these guys out there?"  :)

No pun intended!

*) Anyone?  ;)

Edit: "OpAmps for everyone" chapter 17.2.3
Quote
There has been a lot of confusion in the past over what is the optimum order for PCB layers. Take, for example, a 4-layer board consisting of two signal layers, a power plane, and a ground plane. Is it better to route the signal traces between the layers, thus providing shielding for the signal traces – or is it better to make the ground and power planes the two inner planes?

In considering this question, it is important to remember that no matter what is decided, there will still be signals exposed on one or both of the top and bottom planes. The leads of the op amp PCB package, and the traces on the board leading to nearby passive components and feed-throughs will be exposed. Therefore, any shielding effects are compromised. It is far better to take advantage of the distributed capacitance between the power and ground plane by making them internal.

http://electronics.teipir.gr/menu_el/personalpages/papageorgas/download/2/YLIKO_MELETHS_2012/sloa089.pdf
« Last Edit: May 08, 2017, 11:14:57 am by hammy »
 

Offline blueskull

  • Supporter
  • ****
  • Posts: 13759
  • Country: cn
  • Power Electronics Guy
Re: Routing 4 layer boards
« Reply #16 on: May 07, 2017, 08:34:50 pm »
Usually I do this layer stackup:
Top: local trace (inside a function block, around a single IC), some ground, but gnd plane may not be connected due to crowd traces
Mid 1: ground and horizontal inter block traces
Mid 2: ground and vertical inter block traces
Bottom: solid ground plane and very few traces
 

Offline rob77

  • Super Contributor
  • ***
  • Posts: 1848
  • Country: sk
Re: Routing 4 layer boards
« Reply #17 on: May 07, 2017, 08:48:50 pm »
A common practice these days for EMC is to use the outer layers as ground (I'm sure one could be power with no adverse effects) and run everything inside thus shielding it.

and where you place you parts ?  :-// on a densely populated board you don't have too much (actually none at all ) surface for the shield...  if you just want to have some shielded traces inside a PCB without any components , then a bunch of coaxes would do a better job :D

i would definitely listen to Mike and go for inner ground + power without blind vias :)
 

Offline timb

  • Super Contributor
  • ***
  • Posts: 2528
  • Country: us
  • Pretentiously Posting Polysyllabic Prose
    • timb.us
Routing 4 layer boards
« Reply #18 on: May 07, 2017, 11:10:07 pm »
Yes, Signal + Ground + VCC + Signal is the way to go. I've done this on 4 layer boards running high speed clocks (1GHz) and and 1Gsps DACs without issue. You want a complete, unbroken ground plane and you can't get that with it on the top or bottom, because parts and traces break it up.

Sometimes, if the board isn't too crowded, I'll do a copper pour on the top and bottom layers and then via stitch them into the inner ground plane. If done right and in the proper circumstances it can help EMC issues. (Note: That's not true in all cases, sometimes it can make things worse.)
« Last Edit: May 08, 2017, 11:24:55 am by timb »
Any sufficiently advanced technology is indistinguishable from magic; e.g., Cheez Whiz, Hot Dogs and RF.
 

Offline mikeselectricstuff

  • Super Contributor
  • ***
  • Posts: 12135
  • Country: gb
    • Mike's Electric Stuff
Re: Routing 4 layer boards
« Reply #19 on: May 08, 2017, 08:34:26 am »
A solid ground plane in the middle is likely to do you more good overall than a broken one on the surface.
Youtube channel:Taking wierd stuff apart. Very apart.
Mike's Electric Stuff: High voltage, vintage electronics etc.
Day Job: Mostly LEDs
 

Offline Kjelt

  • Super Contributor
  • ***
  • Posts: 5834
  • Country: nl
Re: Routing 4 layer boards
« Reply #20 on: May 08, 2017, 12:10:14 pm »
A solid ground plane in the middle is likely to do you more good overall than a broken one on the surface.
+1  :-+
 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 14986
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Simon's Electronics
Re: Routing 4 layer boards
« Reply #21 on: May 08, 2017, 03:32:06 pm »
hm interesting, not sure which way to go, I and working at low frequencies in the few KHz range, my main reasoning was RFI shielding for some of the more stringent EMC standards.
 

Offline mikeselectricstuff

  • Super Contributor
  • ***
  • Posts: 12135
  • Country: gb
    • Mike's Electric Stuff
Re: Routing 4 layer boards
« Reply #22 on: May 08, 2017, 03:38:32 pm »
hm interesting, not sure which way to go, I and working at low frequencies in the few KHz range, my main reasoning was RFI shielding for some of the more stringent EMC standards.
Keep it simple - start with power/gnd planes in the middle.  This works just fine for the vast majority of cases. If that's not good enough, chances are you'll need external shielding anyway
Youtube channel:Taking wierd stuff apart. Very apart.
Mike's Electric Stuff: High voltage, vintage electronics etc.
Day Job: Mostly LEDs
 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 14986
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Simon's Electronics
Re: Routing 4 layer boards
« Reply #23 on: May 08, 2017, 03:40:36 pm »
Well I have other plans for external shielding also.

Sent from my Moto G (4) using Tapatalk

 

Offline bktemp

  • Super Contributor
  • ***
  • Posts: 1623
  • Country: de
Re: Routing 4 layer boards
« Reply #24 on: May 08, 2017, 04:40:40 pm »
A common practice these days for EMC is to use the outer layers as ground (I'm sure one could be power with no adverse effects) and run everything inside thus shielding it. Obviously you need a small trace on the part itself to go to a via very close by but after that it's all inside minimizing any length of trace that could act as a transmitter.
Here is a nice presentation on multilayer pcbs:
http://www.kbl-circuits.com/Layer%20stack%20up.pdf

Putting all traces in the inner layers does not make sense for a 4 layer pcb, but can be useful if you have 6 or more layers.
Also putting most traces on the inner layers makes troubleshooting very difficult, because you can't probe the traces.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf