[EE] Bypass capacitors and oscillator on the opposite side of the MPU

[Electron]

Hi,
talking about PCB design:

While Microchip specifies that the bypass capacitors should not only very near
the IC, but also on the same side (I'm pretty sure I've read it in some datasheet),
I am fond of the idea, especially on bigger IC's, to place them, even the crystal
or oscillator, on the opposite PCB side of the MPU, as this solves a lot of space
constraints and problems on the main side. While I do understand Microchip's concerns,
I believe they're pretty exaggerate, as the vias and traces may even get shorter,
practically, by moving these components on the opposite side of the PCB, in the end.

What do you think about this issue?

With kind regards,
Mario

[Richard Prosser]

Hi Mario,
I can't help comparing the situation with "real" CPUs, where the CPU is
placed on one side with its BGA and the decoupling caps are on the other.
Seems to work OK provided it's done correctly (think ground planes as
well). Same with crystals. It's not unusual for the oscillator balls to be
several mm from the crystal and again it works OK as long as you're
sensible.

Richard P

Post by Electron
Hi,
While Microchip specifies that the bypass capacitors should not only very near
the IC, but also on the same side (I'm pretty sure I've read it in some datasheet),
I am fond of the idea, especially on bigger IC's, to place them, even the crystal
or oscillator, on the opposite PCB side of the MPU, as this solves a lot of space
constraints and problems on the main side. While I do understand Microchip's concerns,
I believe they're pretty exaggerate, as the vias and traces may even get shorter,
practically, by moving these components on the opposite side of the PCB, in the end.
What do you think about this issue?
With kind regards,
Mario
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist

[David C Brown]

You are trying to minimize the inductance of the trace from the chip to the
capacitor and vias have a significant inductance. But design calculations
I did for several projects just before I retired convinced me that using
the opposite side of the board with vias was usually preferable to longer
leads to the other side. With SMT devices you usually have vias near the
pins connecting to the power planes and putting the decouplers really near
to those vias is acceptable.

__________________________________________
David C Brown
43 Bings Road
Whaley Bridge
High Peak Phone: [phone]
Derbyshire eMail: ***@gmail.com
SK23 7ND web: www.bings-knowle.co.uk/dcb
<http://www.jb.man.ac.uk/~dcb>



*Sent from my etch-a-sketch*

Post by Electron
Hi,
While Microchip specifies that the bypass capacitors should not only very near
the IC, but also on the same side (I'm pretty sure I've read it in some datasheet),
I am fond of the idea, especially on bigger IC's, to place them, even the crystal
or oscillator, on the opposite PCB side of the MPU, as this solves a lot of space
constraints and problems on the main side. While I do understand Microchip's concerns,
I believe they're pretty exaggerate, as the vias and traces may even get shorter,
practically, by moving these components on the opposite side of the PCB, in the end.
What do you think about this issue?
With kind regards,
Mario
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist

[Harrison Cooper]

Everyone seems to have an opinion, or experience on the best way to do bypass caps. I've always gone by the rules that Intel published many years ago, as do others I work with, that the bypass cap should be as close to the pin your decoupling as possible, and that the power trace runs thru the pad, and not intersect between the device pads. Back in the days of thru hole technology, you would think of the lead of the cap being part of the via feeding it as well. Todays technology, where large BGAs take up room for pin escapes, its not always possible to put the cap as close as possible, and not have the power feed to the cap first and then via to the ball. But perhaps the larger contributing factor is that there are multiple planes creating capacitance on the board as well based on the stack-up, and where app notes specify for best operating conditions use a power and ground plane, you should do so. Also consider the frequency that your operating at as well. When I rout!
e a device, I always try to place the decoupling caps first and drop the vias for them, and route the signals around those. Then the critical clock lines, high speed and finally the slower or less dynamic signals. PCB design is certainly an art.

-----Original Message-----
From: piclist-***@mit.edu [mailto:piclist-***@mit.edu] On Behalf Of David C Brown
Sent: Monday, October 16, 2017 2:35 AM
To: Microcontroller discussion list - Public. <***@mit.edu>
Subject: Re: [EE] Bypass capacitors and oscillator on the opposite side of the MPU

You are trying to minimize the inductance of the trace from the chip to the capacitor and vias have a significant inductance. But design calculations I did for several projects just before I retired convinced me that using the opposite side of the board with vias was usually preferable to longer
leads to the other side. With SMT devices you usually have vias near the
pins connecting to the power planes and putting the decouplers really near to those vias is acceptable.

__________________________________________
David C Brown
43 Bings Road
Whaley Bridge
High Peak Phone: [phone]
Derbyshire eMail: ***@gmail.com
SK23 7ND web: www.bings-knowle.co.uk/dcb
<http://www.jb.man.ac.uk/~dcb>



*Sent from my etch-a-sketch*

Post by Electron
Hi,
While Microchip specifies that the bypass capacitors should not only
very near the IC, but also on the same side (I'm pretty sure I've read
it in some datasheet), I am fond of the idea, especially on bigger
IC's, to place them, even the crystal or oscillator, on the opposite
PCB side of the MPU, as this solves a lot of space constraints and
problems on the main side. While I do understand Microchip's concerns,
I believe they're pretty exaggerate, as the vias and traces may even
get shorter, practically, by moving these components on the opposite
side of the PCB, in the end.
What do you think about this issue?
With kind regards,
Mario
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist

--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive View/change your membership options at http://mailman.mit.edu/mailman/listinfo/piclist

[Van Horn, David]

I'm currently using X2Y caps from Johanson for decoupling, on the same layer as the MPU, with as short a track as physically possible. VCC comes up from a plane layer below the processor outboard of the caps and passes through the caps.

That said, for most applications, adding a via's worth of inductance probably isn't an issue in most applications. Might pay to minimize the via inductance and make sure the series resonant point with the cap isn't going to do anything interesting.


--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive View/change your membership options at http://mailman.mit.edu/mailman/listinfo/piclist

[David C Brown]

This is an extract from a design review I did some ten years ago. I doubt
that the physics has changed since then

*Power distribution and decoupling generally attempts to follow the chip
manufacturer’s guidelines (though these are at best ambiguous and at worst
contradictory). Where no specific guidelines exist a 100nF decoupling
capacitors is fitted for each 1 or 2 package pins.*

*Placement requirements are determined by: calculating the resonant
frequency of the capacitor and its self inductance and mounting inductance;
converting that to a wavelength based on a propagation velocity of c/√Er;
and placing the capacitor within λ/40 of the pin it is decoupling.*


The phrase in parentheses is very apposite :-(


__________________________________________
David C Brown
43 Bings Road
Whaley Bridge
High Peak Phone: [phone]
Derbyshire eMail: ***@gmail.com
SK23 7ND web: www.bings-knowle.co.uk/dcb
<http://www.jb.man.ac.uk/~dcb>



*Sent from my etch-a-sketch*

On 16 October 2017 at 20:43, Van Horn, David <

Post by Van Horn, David
I'm currently using X2Y caps from Johanson for decoupling, on the same
layer as the MPU, with as short a track as physically possible. VCC comes
up from a plane layer below the processor outboard of the caps and passes
through the caps.
That said, for most applications, adding a via's worth of inductance
probably isn't an issue in most applications. Might pay to minimize the
via inductance and make sure the series resonant point with the cap isn't
going to do anything interesting.
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at http://mailman.mit.edu/
mailman/listinfo/piclist
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist

[Van Horn, David]

I had one component advise on a signal that looped out from the chip through some other components and back, to keep the output and input track separated as far as possible, and on those tracks to minimize loop area.
Once you have the components shoved together and tetrised to the IPC limits, those requirements are quite contradictory.

[RussellMc]

​What they all said, and, suggestion only (disagreement or modification

welcome):

Watch loop​ area - go/return leads ideally have minimum separation on the
same layer or run immediately on either side of each other on adjacent
layers. A larger area loop has greater inductance and a greater propensity
for transmitting and receiving. Of the two receiving noise from adjacent
tracks etc is probably the more important.


Russell

[Electron]

Hi,
is there a wonder-IC that will take 3.3V in input and give 5.0V in output well
filtered (similar to a linear voltage regulator output), and that doesn't require
many components?

I was thinking about an integrated boost converter + LDO but the requirement of
an inductor plus n resistor and capacitors doesn't make me really enthusiast.

Maybe a more integrated IC?

Or a charge-pump based one?

Current requirement is low, 50mA would suffice.

Do you know / can you suggest a nice and not too expensive IC which requires as
few external components as possible? I've searched but I am more lost than before.

Thank you very much.

With kind regards,
Mario

[a***@stfc.ac.uk]

Post by Electron
Hi,
is there a wonder-IC that will take 3.3V in input and give 5.0V in output well
filtered (similar to a linear voltage regulator output), and that doesn't require
many components?

http://www.linear.com/products/inductorless_(charge_pump)_dc%7Cdc_converters

[Jason White]

Would a small board mount power supply module/brick work for your
application? That wouldn't require a lot of components.

Post by Electron

Post by Electron
Hi,
is there a wonder-IC that will take 3.3V in input and give 5.0V in

output well

Post by Electron
filtered (similar to a linear voltage regulator output), and that

doesn't require

Post by Electron
many components?

http://www.linear.com/products/inductorless_(charge_
pump)_dc%7Cdc_converters
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist

[Richard Prosser]

There's a pretty wide range of stuff available - the main factor being
current. At low currents a charge pump is likely to be the simplest but at
more than a few mA you are in the realm of inductive boost converters.
These will normally need at least an inductor and a couple of caps and
probably a couple of resistors as well. At high currents greater than a few
amps or so the inductor is going to need to be switched by a MOSFET, adding
a bit more complexity and at higher currents again you'll need a MOSFET
driver as well.

Older chips operate at lower frequencies and need larger inductors and
probably more support components, new ones will operate in the MHz range
and the inductors are quite small (physically & in value). Higher
frequency operation can lead to more noise issues if it's an RF product but
even at lower frequencies you have to do things sensibly - follow the data
sheet recommendations. Older chips also are probably going to be less
efficient although this is countered at the higher frequency of the new
ones. A good conversion efficiency would be in the 85-90% region at the
operating power level. For the larger power levels you do need a way to get
rid of that wasted heat.

A modular approach may suit as these are available quite cheaply from
Aliexpress/eBay etc or a bit more costly from Digikey/Mouser. Effectively
you put these in position & forget about them.
I can't remember the type numbers as I mainly use buck converters but TI,
Linear Tech, Rohm etc... all provide suitable parts. Some will send free
samples & provide evaluation boards it you're looking at quantity
manufacture .

RP

Post by Jason White
Would a small board mount power supply module/brick work for your
application? That wouldn't require a lot of components.

Post by Electron

Post by Electron
Hi,
is there a wonder-IC that will take 3.3V in input and give 5.0V in

output well

Post by Electron
filtered (similar to a linear voltage regulator output), and that

doesn't require

Post by Electron
many components?

http://www.linear.com/products/inductorless_(charge_
pump)_dc%7Cdc_converters
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist

--
Jason White
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist

[Electron]

Post by Electron

Post by Electron
Hi,
is there a wonder-IC that will take 3.3V in input and give 5.0V in

output well

Post by Electron
filtered (similar to a linear voltage regulator output), and that

doesn't require

Post by Electron
many components?

http://www.linear.com/products/inductorless_(charge_pump)_dc%7Cdc_converters

LTC1754-5 looks good, and doesn't need an inductor.. great, thanks.

Post by Electron
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist

[a***@stfc.ac.uk]

Post by Electron

Post by Electron

Post by Electron
Hi,
is there a wonder-IC that will take 3.3V in input and give 5.0V in

output well

Post by Electron
filtered (similar to a linear voltage regulator output), and that

doesn't require

Post by Electron
many components?

http://www.linear.com/products/inductorless_(charge_pump)_dc%7Cdc_c

onve

Post by Electron
rters

LTC1754-5 looks good, and doesn't need an inductor.. great, thanks.

For what you want to do an inductor should not be a problem, so many manufacturers (Wurth, Coilcraft, Murata, etc.) have off the shelf items available for exactly these sort of devices. Most switcher app notes tell you what manufacturers inductor, including full part number, to use, and the inductors are not much more expensive than most other passive components.