Factors to consider for small SMDs

[gauravmp]

Hi,

I'm wondering what the ramifications would be if I were to move from using say an 0805 or 0603 chip to say an 0402 or 0201?

Could someone tell me what factors I should be considering? I'm designing a board that's densely populated and would want to swap out these chips with very small ones. And I'm ok with soldering so I'm looking for other concerns.

Thanks.

[uncle_bob]

Hi,

I'm wondering what the ramifications would be if I were to move from using say an 0805 or 0603 chip to say an 0402 or 0201?

Could someone tell me what factors I should be considering? I'm designing a board that's densely populated and would want to swap out these chips with very small ones. And I'm ok with soldering so I'm looking for other concerns.

Thanks.

Hi

Well, it depends a bit on what sort of part you are talking about. Resistors have one set of issues. Capacitors have another set of concerns. Stuff like inductors and ferrite beads are less common, but they also have issues. It also depends a bit on the frequency range. If this is a microwave design, you will have a different set of concerns than on a MCU board with a bunch of LED's. A full and complete answer to all the possible ramifications could take a day or more to type in.

What sort of parts are you working with and what kind of design is it?

Bob

[MagicSmoker]

I'm wondering what the ramifications would be if I were to move from using say an 0805 or 0603 chip to say an 0402 or 0201?

Two factors that you might not consider and which can be surprisingly restrictive are power dissipation rating for the resistors and ripple current capability for the capacitors (the latter being especially difficult to assess ahead of time when the capacitors are used to decouple/bypass fast-switching digital ICs).

[juanfermed]

On top of my head, one factor you should consider with capacitors is the minimum creepage you need to maintain between pads if you are handling high voltages. I am telling this not from experience, but by learning if from others. Look at this:

https://www.linkedin.com/groups/4860717/4860717-6134243013490143232

Someone in the comments talks about what I am refering to.

I am sure you will like this thread..and also will consider joining this group.

[uncle_bob]

Hi

Ok, well I guess we aren't getting much guidance from the OP so here goes the random shotgun:

====

By far the biggest single thing you should consider is that the package models above 10 GHz will change quite a bit as you go between SMD parts. In designs above 40 GHz, most packages are quite specific to the task rather than generic.

===

By far the biggest single thing you should consider on capacitors as you change package size is their UL rating when attached directly to mains power.....

===

By far the biggest thing to consider on SMD package sizes is the cost function as it relates to the package. In high volume consumer electronics we always keep an eye on cost ....

====

When doing single piece hand assembly on proto boards, having parts that fit your board layout is king.....

(The "big thing to consider" is *highly* dependent on what you are doing ...)

Bob

[Rerouter]

For most ceramic capacitors, the smaller you go, the better the resonance frequency, but you also have a worse voltage de-rating curve,

For smd resistors, its all about voltage ratings and power ratings, other than that its just a resistance,

Also as far as making a densly populated board, take a good look at your footprint library compared to the standards, most times the pads will be quite generous, and the silkscreen will be twice the width of the part, so if you bring this in line with the standard you can pack far tighter,

Suppose the other thing is going smaller sometimes means more Via's as you reach a point where the trace cant fit under the part, for me 0603 can fit 2 traces, and 0402 can fit 1, but without going beyond the cheap pcb places you cant fit a trace between a 0201,

If you really want to go compact as possible, read the datasheets to see what the maximum sizes of the package is, bring your silkscreen inline with this, and you will magically find more room than you know what to do with (for all of 3 minutes).

Other thing is, smaller pads lift easier, so be gentle when your soldering them,

[Richard Head]

If you go smaller than 0805 you can't fit a track between the pads. This is assuming an 8 thou minimum track width and track spacing. This could be a problem, depending on your layout.

[nctnico]

You can still fit a track between the pads of a 0603 but it depends on the position of the pads. If a board is going to be hand soldered I'd stick to 0603 or larger. Soldering 0402 is doable but it takes more time.

[uncle_bob]

If you go smaller than 0805 you can't fit a track between the pads. This is assuming an 8 thou minimum track width and track spacing. This could be a problem, depending on your layout.

Hi

You can fit several tracks if you use 2 mil traces and 2 mil spacing

Getting a via in the pad of the part (or not) will also vary depending on your design rules and if you even do that sort of thing or not (some do, many don't).

If you are already placing 0.3 mm pitch BGA's on an everyday basis, going to 01005 SMD's may not be a big deal. If a 1 mm pitch part is "tight" for you, then 01005 will be an issue.

If parts get stored in open bags on a shelf out in the un-heated warehouse for years at your location, SMD may not be for you. If everything, no matter what it is, automatically goes into nitrogen purged dry boxes, as soon as it hits the loading dock ... not a problem.

If you are used to wandering around the shop floor in sneakers and no blue smock, don't go to SMD. Get your ESD program set up first. Heal straps, conductive flooring, conductive work surfaces are needed. Small parts *are* ESD sensitive.

It all *is* very highly dependent on what you consider normal and what sort of things you are already doing. An industrial control environment that looks at anything under 8 AWG as "hookup wire" does not have the same focus or needs as a military radar outfit.

Bob

[Richard Head]

The board house I use can only do 8 thou min width and 8 thou min spacing with min hole size of 0.4mm. Below that they insist on bare board testing, at your own risk.

[Siwastaja]

The board house I use can only do 8 thou min width and 8 thou min spacing with min hole size of 0.4mm. Below that they insist on bare board testing, at your own risk.

Maybe you should consider changing your board house, because literally the cheapest manufacturers in the world (according to pcbshopper.com) offer 6/6 mils with 0.3mm hole as a standard service. I have used them with good results. Use almost anything beyond the cheapest Chinese, and you'll easily get down to 4/4 or 3/3 mils. Haven't seen 8/8mils spec in a few years anymore, not even in the cheap places.

[Richard Head]

You may be right. The board specs are limiting how dense a layout I can produce.
It's a pity since they are good in all other respects. Thanks for the feedback.

[uncle_bob]

You may be right. The board specs are limiting how dense a layout I can produce.
It's a pity since they are good in all other respects. Thanks for the feedback.

Hi

There are a *lot* of places that will do much better than 8/8 as limits. You do not take a quality / delivery / price hit when you move up to 6/6. You might see a small impact at 4/4.

Bob

[Rerouter]

Also if your cad package supports it, do fillets on your smaller via's, it relaxes the risk of a breakout if the registration is wonky,

[gauravmp]

Hi,

I'm wondering what the ramifications would be if I were to move from using say an 0805 or 0603 chip to say an 0402 or 0201?

Could someone tell me what factors I should be considering? I'm designing a board that's densely populated and would want to swap out these chips with very small ones. And I'm ok with soldering so I'm looking for other concerns.

Thanks.

Hi

Well, it depends a bit on what sort of part you are talking about. Resistors have one set of issues. Capacitors have another set of concerns. Stuff like inductors and ferrite beads are less common, but they also have issues. It also depends a bit on the frequency range. If this is a microwave design, you will have a different set of concerns than on a MCU board with a bunch of LED's. A full and complete answer to all the possible ramifications could take a day or more to type in.

What sort of parts are you working with and what kind of design is it?

Bob

Hi Bob,

I'm sorry I didn't respond to you. I'm working with high speed ADCs and Amplifiers on the board. So the board runs at about 120MHz. And I'm trying to reduce the population density by going with small resistors and capacitors.

Thanks

[uncle_bob]

Hi Bob,

I'm sorry I didn't respond to you. I'm working with high speed ADCs and Amplifiers on the board. So the board runs at about 120MHz. And I'm trying to reduce the population density by going with small resistors and capacitors.

Thanks

Hi

For very regular things (like line terminations) you can go with multiple resistors in one package. They can be a bit easier to deal with. For capacitors, be very careful to watch the dielectric.

Bob

[gauravmp]

Thanks
I'll check that out

[TiN]

Also beware large-capacitance 0402's caps. Many of them are not really 0402, but actually bit bigger. This can be an issue in tight layouts, where you designed PCB and spacing to fit regular 0402 component, and get bigger capacitors shorting each other.

[uncle_bob]

Hi

Ok, as you try to pack more capacitance in a given sized package, you change the dielectric material. No big surprise there, people have been doing that for at least the last 80 years. What is a little less obvious is that there are always tradeoffs. The higher the density the worse a dielectric material it is. What happens:

1) Delta C vs V goes up ( = it's not really Q = CV anymore)
2) They become microphonic ( = it's a microphone !!)
3) The loss tangent goes up / Q goes down
4) The maximum useful frequency comes down
5) The ESR goes up
6) The insulation resistance comes (mega ohms microfarads) down
7) They likely become easier to crack / fracture
The layer thickness goes down ( = they may short out more often)
9) The change in capacitance versus temperature goes up (maybe way up)

That's just the first few items on the list ... there are a lot more. I would avoid anything looser than an X7R if possible for bypass. Never use anything but an NPO in an RF circuit.

Bob

[Richard Head]

All good advice. Unfortunately I find it difficult to get NP0 above about 1nF.

[uncle_bob]

All good advice. Unfortunately I find it difficult to get NP0 above about 1nF.

Hi

It's just a matter of package size. You can find 100 nf if you look around a bit. The major distributors do have them in stock. It's not going to be in an 0402 and they will not be penny a piece sort of prices. If you want bigger than that, it does start to get a bit more difficult.

Bob