Considerations when sizing (physical) SMD/SMT capacitors

Go To Last Post
20 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

G'day,

 

I've recently finished the schematics for my ~900 component device. I have primarily used 0805 capacitors as a starting point, as I'll be assembling the board manually (most likely using a toaster oven/stove to reflow at this point) and want a size which is relatively manageable. I've untangled the ratsnest and placed the components in their rough position, and I think 0805 is going to be too big. Note: I have larger electrolytics which aren't my concern, I'm more interested in the ceramic decoupling/bypass capacitors.

 

Given that I'll be reflowing, I think I should be fine to use 0402. Some of the capacitors require a 50V rating, so I'll use the smallest size I can for the given type (e.g. X7R, X5R, etc.).

 

My question: other than voltage rating and cost, are there any performance, capacitance, inductance, etc. considerations when choosing between two SMD/SMT capacitors of the same specification in two different sizes (e.g. 0402 or 0603 vs. 0805)? I came across a post on StackExchange where a user had posted part of their layout, and multiple commenters stated that the use of 0805 was sub-optimal (for the given purpose I assume), and that they should use 0402 instead, maybe 0603 at a push.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

In my opinion, unless you are working with a very high speed digital system (lets say, under 10ns rise/fall times) or RF much above, lets say, 50MHz, you will not be able to practically distinguish between 0805, 0603 or 0402 parts.

 

There are a few situations when the device is to be CE/FCC certified for emissions or susceptibility, that these criteria will fail. If these criteria DO fail, then usually you will find that the failures are typically above 100MHz. And, usually the problem is not the component but the layout (poor ground, poor selection of where to connect the bypass, and such). Been there, done that.

 

Jim

Jim Wagner Oregon Research Electronics, Consulting Div. Tangent, OR, USA http://www.orelectronics.net

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

1206 or 0805 or even 0603 sizes will be perfectly fine.  Why make things microscopic, unless you have a strong need?  There is a performance penalty for making the parts smaller...something has to give...performance isn't free...if you want 0.2uf in a very very very small package, then eventually some parameters (like voltage rating, stability, dielectric robustness, etc) will have to give way.  Parts need room to exist.   Now a 10pf cap might be a much different story, you need much smaller amount of storage compared to 200000pf.  Now at very high freqs(GHz), lead inductance (ESL) is a big issue, and of course all SMD parts are 10 steps ahead of a leaded 0.1uf cap. 

When in the dark remember-the future looks brighter than ever.   I look forward to being able to predict the future!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thank you both for your input, it's greatly appreciated. I am using a few high speed interfaces, namely USB 3.0 and an LVDS display (high-ish speed I guess). Given your comments, I'm going to go through the capacitors again and try and change the 0805s for 0603 and 0402 where feasible. In the cases of USB 3.0 and LVDS, I'll use whichever size is recommended in the respective datasheets and/or evaluation board schematics. Thanks!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

We’re talking very high speed data interfaces here - so component selection is critical and probably more so is the pcb design.
With the high capacitance ceramic caps, you need to read the datasheets carefully! They are not the simple component you might expect. The capacitance is related to the applied voltage, temperature, aging etc.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thanks Kartman, I'll be sure to pay extra close attention to the datasheets for the high speed interfaces :)

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Also, likely even more importantly than part size, is to have a large & solid gnd plane to connect all those caps to...Don't come back here & haggardly show up with your caps all grounded to some thin traces snaking around the bottom of the board...the key word is plane.  In some cases, a separation of planes is desirable, but a solid plane, solves so many of the world's problems.  Try to route as few traces on the bottom as possible..and NO long ones allowed (convert any long ones to a series of short runs)...you can do it, if you try.  Allocate 5x time you think you'll need.

When in the dark remember-the future looks brighter than ever.   I look forward to being able to predict the future!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I'm using a 4 layer stack, which has a dedicated, uninterrupted ground plane :)

 

As for routing traces on the bottom layer, it's going to be unavoidable in this case given the number of components and the size of the board. I'll be routing the highest speed, most sensitive interfaces first (USB 3.0, Ethernet, LVDS, USB 2.0, SDIO) to ensure I don't need to route traces on the bottom, leaving the slower, less sensitive interfaces (GPIO, UART, SPI, I2C, etc.) for any required bottom layer routing. Obviously I'll be paying close attention to both single ended and differential impedance for these traces, as well as both low frequency (least resistance) and high frequency (least impedance) ground return paths.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

jars121 wrote:
I'll be routing the highest speed, most sensitive interfaces first (USB 3.0, Ethernet, LVDS, USB 2.0, SDIO) to ensure I don't need to route traces on the bottom, ...
An RF jumper would save a layer change for a signal though those have a price.

DC to 6GHz

(I've forgotten USB 3's bandwidth)

jars121 wrote:
... leaving the slower, less sensitive interfaces (GPIO, UART, SPI, I2C, etc.) for any required bottom layer routing.
Jumpers for those to save signal's layer change though the cost is area.

 


Mouser

AVX X2A, X2B Series MLO Crossovers

https://www.mouser.com/new/AVX/avx-MLO-crossovers/

AVX

MLO™ RF-DC SMT Crossover

http://www.avx.com/products/rfmicrowave/crossovers/mlo-rf-dc-smt-crossover/

http://www.avx.com/products/rfmicrowave/crossovers/ 

Harwin

Surface Mount Links

https://www.harwin.com/product-highlights/surface-mount-links/

 

Edit: 3rd URL

 

"Dare to be naïve." - Buckminster Fuller

Last Edited: Thu. Sep 27, 2018 - 11:43 PM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thanks, I had actually not come across those before!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 1

avrcandies wrote:

Allocate 5x time you think you'll need.

I find this to be true about almost any task....

 

--Mike

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

One thing to note, within a given type (X5R/X7R) the larger packages tend to have less capacitance loss due to DC bias. For decoupling this isn't much of concern. The total capacitance is less important than having a low inductance from smaller packages.

 

My strategy for bottom routed signals is to keep vias as close as possible to the chips where the planes are well decoupled. When traces cross between power planes, I group them close together with a cap between the power planes, or a pair of caps to ground. Vias that can't be placed near a chip get grouped together in a 'crossroads' area with decoupling cap(s) to ground.

 

With that many components I hope a SS stencil is in your budget. I cringe at the thought of hand apply paste.

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

balisong42 wrote:
With that many components I hope a SS stencil is in your budget.
Two alternatives to stainless steel for stencils are mylar

https://www.pololu.com/product/446

and Kapton

https://ohararp.com/stencils/kapton/

https://www.oshstencils.com/

 

Edit: 2nd URL

 

"Dare to be naïve." - Buckminster Fuller

Last Edited: Fri. Sep 28, 2018 - 01:06 AM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

As for routing traces on the bottom layer, it's going to be unavoidable

Fine, all I was asking was to have one layer for gnd plane...assuming it was on the bottom of a 2-sider....but you have 4 layers so all is well.

 

Sound like you are on a roll & will have an excellent layout...

When in the dark remember-the future looks brighter than ever.   I look forward to being able to predict the future!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hand soldering components down to 0402 can be done with practice, a good lighted magnifier and a steady hand. 

Then use hot air to reflow to look nice.   Sounds like a fun project, hope you don't have to build too many of them!   

 

Please come back and post a picture of the completed project, yes us sparkies like seeing a well built project!

 

Jim

 

Click Link: Get Free Stock: Retire early! PM for strategy

share.robinhood.com/jamesc3274
get $5 free gold/silver https://www.onegold.com/join/713...

 

 

 

 

Last Edited: Fri. Sep 28, 2018 - 01:11 PM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Is this an ARM at X 100's MHz, or an AVR at 20 MHz?

 

If the project / PCB is running at high speed then go ahead and use the small components.

But Man-Oh-Man that is going to be a painful build by hand.

 

If the majority of the PCB is "just" a 20/32 MHz uC, then I'd build the majority of the PCB with at least 0603 parts.

I still build my boards with 0805 parts.

They are as easy to handle as the old through hole parts.

 

If there are some parts, (filters, pull-ups, etc.), on the high speed bus then go ahead and use the small stuff, but I'll confess my personal experience with that is minimal.

I did some VHF stuff with 0805 without any problems...

 

If you hand build a PCB with 1000 0402 parts come see me in the ER after words and we'll chat about ice packs, hot showers, Ibuprofen, muscle relaxers, and a good massage therapist; all needed to get the kinks out off your neck and upper back.

 

I'm glad Jim asked for a Photo, I was thinking the same thing.

 

It is always fun to see a nicely made project, even if it is someone else's!

 

JC

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

DocJC wrote:
But Man-Oh-Man that is going to be a painful build by hand.
... or bail to the local for-hire technician (did so once in mid-90s when was overly scared of QFP due to zero experience with SMT)

Nowadays, there's the turn-key prototype PCBA.

https://macrofab.com/

https://www.mouser.com/macrofab-events/ (Houston Texas)

 

"Dare to be naïve." - Buckminster Fuller

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I avoid anything smaller than 0603 (inch). They're pretty easy to place. 0402 are demonic.

The largest known prime number: 282589933-1

It's easy to stop breaking the 10th commandment! Break the 8th instead. 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I still build my boards with 0805 parts.

I also like 1206...anything that has markings that you can read...no markings, then it can become ultimate chaos.... whoops wrong parts in that bin of 100 I just installed.  Double whoops, was swapped with another bin that I just installed 200 of. 

Someone hands me a board, I want to be able to tell what part Billy installed where, without sleeping on a bed of nails.

 

 

When in the dark remember-the future looks brighter than ever.   I look forward to being able to predict the future!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Also, be aware of the current supply problems. A lot of these capacitors are on 50+ week leadtimes so it may be worth thinking about what values and the types of dielectrics you can actually obtain...

There are already a million monkeys in front of a million keyboards, and the internet is nothing like Shakespeare!

Last Edited: Wed. Oct 17, 2018 - 09:40 PM