Author Topic: First Complex PCB Design  (Read 11353 times)

0 Members and 1 Guest are viewing this topic.

Offline logictomTopic starter

  • Supporter
  • ****
  • Posts: 336
  • Country: au
First Complex PCB Design
« on: June 21, 2011, 05:12:56 pm »
I've created some basic single and double layer PCBs in the past using through hole parts but I'm now faced with designing a PCB with SMD parts and a jump in complexity.

When designing a PCB when should the decision be made about how many layers to use and what are the deciding factors?
I'm designing a board with an Arm processor and small size is a must so I'm wondering should I just start out with 4 layers? Is it easy to design with 2 and then switch to 4 layer on?

What size smd parts should I start with and what are the trade off's between using different sizes?

The processor I'm looking at is a QFN64 with a centre VSS pad, should I bring this through to another layer with one or multiple vias, how many should I use?

Thanks as always :)
 

Offline sacherjj

  • Frequent Contributor
  • **
  • Posts: 993
  • Country: us
Re: First Complex PCB Design
« Reply #1 on: June 21, 2011, 05:22:11 pm »
If many of your traces will be power or ground, you immediately drop in complexity by using a VCC and Ground layer in the center of a 4 layer board. 

If you are going to hand solder the parts, make sure you try some 0402s before you work with them.  They are doable, but not "fun".  I've just recently gotten into SMD and did my first 0402 this weekend.  I now have some good tweezers on order.

I found using solder paste and the hot air iron made it pretty painless, with the exception of getting the 0402s in place.  The solder paste will pool and draw itself along the solder mask towards the pad and help self center parts.  The occasional tombstone is just pushed down while both sides of the solder is molten.  The biggest issue is clearing solder bridging from using too much solder.
 

Offline Neilm

  • Super Contributor
  • ***
  • Posts: 1551
  • Country: gb
Re: First Complex PCB Design
« Reply #2 on: June 21, 2011, 07:27:33 pm »
Firstly, is this for work or for fun? If it is for work and what you are doing will go on sale then I would without hesitation say go for at least a 4 layer board. This is because any product on sale has to meet EMC regulations and I have found that it is much easier to meet this when you have power and ground layers.

If it is for fun / home use I would consider it and judge how much it will cost for a 2 layer board vs a 4 layer board. Then I would choose a four layer board, especially given the package you are looking at using.

Noise on traces can and will cause problems with a processor. Many problems are caused by poorly routed boards both with the signal tracks and supply tracks.

Don't try to design for 2 layers then switch to 4 layers. You will find that you will have made a large number of compromises and will then end up having to rip up and reroute later.

I would suggest going to http://www.compliance-club.com/ and looking through the articles from Keith Armstrong (Registration is required to look at them but it is free). I have a copy of his book on EMC layout tricks for EMC. It is a valuable book that explains what to do for good layout techniques and why they work without burying you in maths. See this for your question on how many vias.

I would generally recommend components at 0603, they are a little fiddly but OK with a good pair of tweezers - I don't even use magnifiers with these. Don't try to hand place 0102s - it doesn't work.

Yours

Neil


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
 

Offline Zero999

  • Super Contributor
  • ***
  • Posts: 19672
  • Country: gb
  • 0999
Re: First Complex PCB Design
« Reply #3 on: June 21, 2011, 10:21:17 pm »
Yes, put the power planes in the middle and the traces on either side because it makes debugging and rectifying errors possible. Having two power planes closely sandwiches on top of one-another is good for EMC because they will form a parasitic capacitor with as much as a couple of 100pF which improves supply decoupling and large copper planes have a lower inductance than long thin traces.
 

Offline logictomTopic starter

  • Supporter
  • ****
  • Posts: 336
  • Country: au
Re: First Complex PCB Design
« Reply #4 on: June 22, 2011, 09:30:23 am »
Thanks for the suggestions, it's my project for uni and what it to be something I can take to interviews and the likes so will go for the 4 layer, see how much I can stretch their budget :)

Thanks for the link Neilm, will definitely check that out and pop into the library for that book or any other EMC books.

Going for 4 layers is it best to go signal - gnd - power - signal or signal - power - gnd - signal, does it make much of a difference or should I keep the gnd layer closest to the layer with the majority of signals?
 

Offline jahonen

  • Super Contributor
  • ***
  • Posts: 1054
  • Country: fi
Re: First Complex PCB Design
« Reply #5 on: June 22, 2011, 09:42:36 am »
Going for 4 layers is it best to go signal - gnd - power - signal or signal - power - gnd - signal, does it make much of a difference or should I keep the gnd layer closest to the layer with the majority of signals?

Keep the gnd plane adjacent your most critical (high edge rate or interference sensitive) signals. There are some cases where the power rail is the reference but those are usually very rare (PECL logic).

Regards,
Janne
 

Offline Zero999

  • Super Contributor
  • ***
  • Posts: 19672
  • Country: gb
  • 0999
Re: First Complex PCB Design
« Reply #6 on: June 22, 2011, 04:21:26 pm »
What difference does it make whether you've got the ground plane or VDD plane adjacent the a signal containing high frequency harmonics? If you've got good decoupling, at AC the ground and power plane are the same thing since they're connected together with a very low AC impedance. I wouldn't worry about this too much, just put the +V/0V power planes in the middle on a four layer board and you shouldn't have any problems.
 

Offline jahonen

  • Super Contributor
  • ***
  • Posts: 1054
  • Country: fi
Re: First Complex PCB Design
« Reply #7 on: June 22, 2011, 06:48:02 pm »
What difference does it make whether you've got the ground plane or VDD plane adjacent the a signal containing high frequency harmonics? If you've got good decoupling, at AC the ground and power plane are the same thing since they're connected together with a very low AC impedance. I wouldn't worry about this too much, just put the +V/0V power planes in the middle on a four layer board and you shouldn't have any problems.

The recommendation to not to switch routing layers is from Howard Johnson's book High-Speed Digital Design (can't recommend that one enough!), where he recommends not to do that. The planes are still far enough to create quite big discontinuity in return path (remember that return current is mostly concentrated as near as the signal as it can, which is natural energy minimum for stored magnetic field = minimum inductance). Any imbalance of currents will manifest itself as common mode current, which shows up as EMI.

Adding a capacitor near the via, one improves the global VCC decoupling, and provides required return path. And it should be noted that the path of the return current is just as important as the signal current, however, it is usually unfortunately neglected. My measurements using a near-field probe shows that vias show up as high near-field points (not radiating, however). Situation changes if one has 6 or more layers. Then it is possible to change the signal on opposite side of same reference plane.

However, to be honest, it usually is not a big deal if there are no wide "fast" buses on board, like SDRAM or DDR. But it does not hurt to go "by the book" as much as possible, anyway (no added cost). I usually do not bother with extra decoupling caps, but I'll try to avoid swapping layers especially on clock traces.

Regards,
Janne
 

Offline Neilm

  • Super Contributor
  • ***
  • Posts: 1551
  • Country: gb
Re: First Complex PCB Design
« Reply #8 on: June 22, 2011, 06:53:13 pm »
Going for 4 layers is it best to go signal - gnd - power - signal or signal - power - gnd - signal, does it make much of a difference or should I keep the gnd layer closest to the layer with the majority of signals?

There are advantages of having specific stack ups but it usually only matters with VERY high frequencies (in order of GHz).

Neil
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
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf