Any tips for 4-layer boards?

[Byte_Butcher]

Well... In the "old days" I used to build projects with through-hole parts on "vectorboard" (or perfboard, or punchboard, or whatever other names it goes by).
That worked for me for prototyping projects for about 30 years.
And if I made a mistake I could unsolder something and "move it over there" and re-solder it...

Then one day I woke up to find that a lot of the "cool" new parts that I'd like to use are only available in surface mount packages. Sigh.

So I finally set myself up with enough equipment to do SMD's and I started laying out (and paying for ) boards for most of my projects. But small runs of boards are EXPENSIVE, so I've gotten pretty good at maximizing my board usage to get the most parts on the least amount of real estate. I've done quite a few pretty dense 2-layer boards with good success. (Don't ask about the RTC that got laid out "upside down" on one board... I felt really stupid with a magnifying glass and tweezers bending the leads on the IC's to point upwards so I could mount it upside down on the board. )

Anyway, now I've got a new project that needs to fit in a very tight space.

I've got 6 IC's including 16F887, an RTC and xtal, EEPROM, voltage regulator, digital pot, and IR detector. (mostly TQFN, TSSOP, and DPAK packages)
There's also 5 MOSFETS, 4 in DPAK and 1 in SOT223.
And there's a few diodes, a crystal, a 470uF electrolytic cap (big!), and a metric ****load of resistors and caps, mostly in 0603 packages.

All together there's 59 parts that live ON the board, plus connectors to connect a 2x16 LCD, several external sensing devices, and power and programming connectors.

The problem? It's all gotta fit on less than *5*square inches of real estate. I've got about 2" x 2.5" of space to work with.

I've banged my head against it for days now trying to make it fit on a 2 layer board, but I just can't quite get there. I'm using the smallest packages available (or that I can work with) but it just ain't gonna go on 2 layers in the space I've got to work with.
If I go to a 4 layer board it should work . It's tight... but it'll fit.

SO... Are there any special tips I should know about for laying out 4 layer boards? I've done plenty of 2 layer, and in theory 4 layer should be easier... But 4 layer is so much more expensive and I don't want to do something obviously stupid and wreck it.
I've got power and ground on the inner layers and all my signal stuff on the outers. Everything *looks* like it's OK, but I think I've got the fear in me because it's my first time. :

Any words of wisdom before I jump into the world of 4-layer and blow $120 for 6 boards that are only 5 square inches each?



steve

[mackrackit]

I do not have any good suggestions about a four layer, but if you have the height why not two two layer boards stacked?

[Pic_User]

Hi guys,

Sounds like you guys have come up with some good ideas for squeezing the most components into the least real-estate. What might work would be insulated jumpers in place of the added layers. Circuit board designers have a prejudice against jumpers, but I have used them to avoid additional layers. Just force the layout with two layers then rearrange for the least and shortest “air-wires”. The jumpers would replace the air-wires.

We want to see pictures of your projects! Past and future.

-Adam-

[ScaleRobotics]

When I need to pack the most parts per inch, I start populating the bottom side with a few of the parts I can't fit on the top. I never had to go to 4 layer.

[Ioannis]

Triple check. What else can I suggest?

What is your design program? In Eagle there are some tools that help to find shorts or unconnected parts.

Use these tools to make it easier for checking.

Photos would be great for this!

Good luck and keep us posted.

Ioannis

[Byte_Butcher]

Thanks Guys for all the good suggestions!

If this thing works well I hope to make a commercial product out of it, so ease of assembly and a minimum amount of "external" wiring that needs to be hand soldered is important.
I want 6 boards to build prototypes, and if all goes well I'll order 100 more for my second round. So it's not just a "one of" project. and It needs to be easy to assemble and reasonably "proffesional".

In the long run, I think that Ioannis had the most practical suggestion for this board.... Triple Check!! (I knew that anyway)

I don't think that a pair of stacked 2 layer boards saves any money on board costs (4-layer costs less than twice as much as 2 layer), but probably does add quite a bit to assembly time.

I already tried putting some parts on the backside of the board, but that didn't seem to help. The back is already dense with traces and parts on the back just eats up space where traces need to go and nothing is really gained. Besides, I dislike populating both sides on SMD boards because it's a bitch to keep parts from falling off the bottom when the board is in the oven and I don't relish the idea of soldering one side by hand. I know there's special glues available for that, but that takes more time so I'd rather not populate both sides if I can avoid it.

I'm not a big fan of jumpers and "air wires". I DO use them sometimes, but again, it means more hand soldering and possibility of problems. And I'm afraid I'd need many of them for this board. Besides, jumpers require through holes, which kills space on BOTH sides of a board.

I think I'm doomed to go with 4-layer boards on this one. It's OK. I need to learn to become proficient at 4-layer anyway since parts keep getting smaller and smaller, and 4-layer does have some advantages with noise immunity.

I use DIPTrace for my schematic layout, and if I want quite a few boards I use DIPTrace for the board layout also. However, if I just need a few small boards at the lowest possible cost, then I order them from ExpressPCB, which means I'm stuck using their irritating board layout software. (Love their board quality and prices, hate the layout software)

DIPTrace does have some good tools for verifying the integrity of networks and the like. And it IS possible (with a little work) to import the netlist from DIPTrace to ExpressPCB, so I'm pretty sure my board layout matches the schematic OK.

I tried Eagle for a few boards, but I just didn't like it much. It seemed difficult and non-intuitive to learn and I finally gave it up. DIPTrace is more compatible with my brain I think.

I worked on the board a bunch last night and I think I'm about done. I need to double check the footprints of a few items one more time, and also change the pad sizes where the LCD connects, but I think it's about ready to submit... I hope.

Here's a pic of the top copper layer and silkscreen. Keep in mind that the entire board is only 2.5" (63.5mm) tall.





Some of the patterns look a little "funny" because they are laid out to accept more than one package style. For example, Q's 2-5 can accept MOSFET's in either DPAK, or TO-220 (stood up)

Thanks for all the suggestions. I'm gonna go with the "triple check" method and hope for the best!


steve

[Melanie]

If you want to make a commercial product, bear in mind that a THOUSAND VIAS will still cost less than a four layer board (which is basically two two-layer boards glued together). The only reason I can ever think of going into multi-layers is either Screening or Power Dissipation purposes. With good CAD software (and a good PCB manufacturer) your track separation can be as little as 0.15mm and there should be no need for four layers.

(For those who don't know, a VIA is a tiny plated hole connecting two layers of a board.)

[Ioannis]

I have not any experience wit 4 layers so cannot say if they are more expensive that many vias or not. But if Melanie says so, I accept it as a fact.

So, indeed it looks dense enough but may be if you select other PIC pins thing can get easier.

For your checking, does your software have any tools? Like highlighting the electric connections or showing the shorts, etc?

Ioannis

[rsocor01]

Hi,

I have done many 2-layer SMD designs, but I have never done a 4-layer design. I agree with Melanie that the preferred way to go is to use many vias with 2-layer boards. There are many useful design tips in the next PDF document.

http://www.alternatezone.com/electro...torialRevA.pdf

I use pad2pad instead of expressPCB. Their software is very user friendly and it has features to check your design for flaws.

Also, there are ways for programing your chip on board without having to solder a connector for programming purposes. Well, keep us posted about your project.

Robert

[ronsimpson]

Steve,

Will U5 get hot? I usually use a larger pad as a heat sink.
Is there much power lost in Q2,3,4,5? I usually have a large collector pad on all layers. This works as a heat sink and carries the heat to the other side of the board.

U3,C12 spacing?

Often a LCD display needs a “pot” to set contrast.

Mounting holes?

When I do 4 layer boards I usually use one of the inter layers as ground.
The other inter layer may have large areas of +5, +3.3 and a hand full of hard to rout traces. I usually have signal traces on the outside.

If there are noise issues, I may have the outside layers as ground and power planes. This sandwiches the signal traces between planes of copper. (FCC issues)

Using ball-grid arrays I need two signal layers, power, ground, and two more signal layers.

ron

[Byte_Butcher]

Thanks to everyone for all the good advice!
I'd hoped to get my board design submitted last week, but I think I need to sit on it and think for a while longer first.
I've got other obligations this week and may not get to work on it for a few days now.


Melanie,
Using more vias instead of more layers sounds great! But I just couldn't get there.... I ended up with too many traces on the backside and carved up my ground plane and had problems with islanding and I *still* couldn't quite get it all to fit.
With 4 layers I can run traces on both outer layers with power and ground internal and it gets LOTS easier for this poor old boy...
I'm sure the problem is all about my lack of skill. I haven't done all that much board design and I've usually got plenty real estate to work with.


Ioannis,
Yes, I think I need to shuffle a few pins around. But some are pretty much fixed by function (many of the sensors need an ADC pin), and some pins are fixed by... habit (I use the same pins for the LCD on several projects so it's easier to remember what's what.)
Part of the problem is that the "core" of the circuit was stolen from a previous project, so the layout on that chunk might not be ideal for this project.

Anyway, I'm going to toss all the parts down on the board again and start over and see if I can cram it onto two layers.


Robert,
Thanks for the link to the PCB Design Tutorial. That was a worthy read and may provide some useful tips for me. Much appreciated!
Yeah, I know I can ditch the programming connector. I eliminated it on the 2 layer design (still couldn't make it all fit), but there was enough space after going to 4-layer that I snuck it back in again. If nothing else it brings those PIC pins out where I can use them If I want.


Ron,

The power dissipation on the voltage regulator and transistors should be fine. The regulator has already proven itself to not need any more heat sinking (in another project) and the power dissipation on the FET's is low, and the duty cycle is also low. Should be fine.
I did add an extra set of through holes for those parts so I can use T0-220 parts on a heatsink if I ever need to.

Yes indeed, got a contrast pot for the LCD. It's digital (U4) so the user can have some control over it without needing to access the board with a screwdriver.
Got a single big ugly mounting hole right above Q3.

You use BGA parts? Wow. Way too scary for me still.


Anyway, I appreciate all of the good advice you folks have given,and later this week I'm going to try and do a better job on layout and see if it'll all cram onto 2 layers.
You folks have inspired (or shamed) me into trying harder.


steve

[Ioannis]

Can you get rid off of the U4 and replace the function with some PWM from the PIC itself?

Ioannis

[Byte_Butcher]

Can you get rid off of the U4 and replace the function with some PWM from the PIC itself?

Ioannis

Mmmmm.... I don't know. The contrast pin for the LCD wants to be on the "wiper" of a 10K pot with the other legs connected to Vdd and Vss.

I'm not sure what would happen if I fed it from a filtered PWM output... ?

U4 actually eats up about the same amount of real estate as the 10K pot that it replaced on my original design, but it adds easy user adjustment.

Actually, I've been working on it some today and I'm starting to think I just might get the whole thing on 2 layer now that I've got a bit better layout.

We'll see....



steve

[Melanie]

http://www.picbasic.co.uk/forum/show...=Easy+Contrast

Actually, six years on from that post I standardised with 1K5 for R1 and 470R for R2... works well...

[Byte_Butcher]

http://www.picbasic.co.uk/forum/show...=Easy+Contrast

Actually, six years on from that post I standardised with 1K5 for R1 and 470R for R2... works well...

Errrr.... seriously? It's that easy?

Melanie, you never fail to amaze me.

No need for a filter cap even? Any benefit to using one?
Any restrictions on the max/min PWM frequency?

Thanks VERY much for that tidbit. That's excellent.

Ahhh rats... now what am I going to do with all those digital pots I've got in stock?


steve

[Melanie]

Here's the HPWM code I use to drive Contrast...

SetLCDContrast:
	DataA=Contrast*40
	HPWM 2,DataA,1000
	Return

DataA is a byte variable. Contrast is a User software selectable value between 1 and 5. The factory default is 2.

A Capacitor is a waste of real-estate. Your eye can't distinguish 30Hz (TV picture frame rate) let alone 1kHz as used above... your LCD probably can't switch that fast either. How fast is your LCD monitor... 3mS? - mine's closer to 9.

As always, try it on a breadboard with your chosen LCD before you commit to PCB... I've used it sucessfully on dozens of different PowerTip and Tri-T LCD's without problems.

If you have a couple of PWM channels, use the other one for the Backlight... same code... do a Search for Easy Backlight.

[Byte_Butcher]

Thank you Melanie, that's great!

I'll give it a try as soon as I get a chance. It saves some expense, and a bit of real estate, and 1 PIC pin compared to the digital pot method. Very nice!

I'm already using the other PWM channel to drive a MOSFET for the backlight. I figured out how to do that several projects ago.

I'll give your circuit a test to make sure it works with my LCD before I commit to a run of boards, but it sounds like a very happy thing for my project.

Thanks ever so much for your help!



steve

[Byte_Butcher]

Well I just tried Melanie's "Easy Contrast" circuit and it works great!
I tried with and without a filter cap and there's no visible difference.
I ended up using 2K and 1K resistors because I had some laying within arms reach and it gives good control.

That's cheaper and uses less real estate than a trimpot, and it gives the user control that I was going to use a digital pot to achieve. With only 2 resistors.

Most Excellent! Thanks Melanie!


steve

[Byte_Butcher]

Well, I shuffled a bunch of stuff around, made a few circuit changes, and presto!
It all fits on 2-layers now.

5 IC's
19 Capacitors
28 Resistors
5 Transistors
4 Diodes
1 Crystal,
1 LED
+ connectors and wires to the outside world.... power supply, sensors, LCD, etc.

All on a board that's about 2.5" high and less than 2" wide.

Thanks to everyone that provided suggestions and insight. Much appreciated.


steve

[Ioannis]

Thats great news! Now, how are you going to solder components?

Ioannis

[Byte_Butcher]

Thats great news! Now, how are you going to solder components?

I've got some good stout radiator solder and a propane torch.

Actually, I'm modestly well setup to do SMD boards. I have a homemade reflow oven (modified toaster oven) and a cheap hot air rework station.
I've done quite a few small SMD boards but nothing quite as tight as the current one.

Here's a basic PIC controller board with RTC and EEPROM on board. Various versions of it lounge around on my bench, being test beds for assorted projects...





Since this latest board has up to 63 parts on less than 5 square inches, I'll definitely cough up the extra $$ to have silkscreen and soldermask on this one.

I'm glad it all went on 2 layers. I was willing to go to 4, but cheaper is better...


steve

[TinkersALot]

Outside of reading temperatures, that is? Just seems like a pretty beefy processor to read/display temperatures, so am merely curious.

[Byte_Butcher]

Outside of reading temperatures, that is? Just seems like a pretty beefy processor to read/display temperatures, so am merely curious.

Nahhh, you're missing the point!
It's not about displaying temperature.... It's a learning platform!
(that photo looks like it was a learning test for the MCP9800)

It's a board that holds a $3 PIC that has lots of I/O .
It has space for additional EEPROM if you feel like doing some data logging. It's got provisions for a DS1302 RTC if you need real time (to go with your data logging, or whatever?) (if you don't need that junk, don't load it)

It's got a connector to connect to an LCD display so you can... display stuff.
It's got an onboard MOSFET to control the brightness of the LCD backlight.

It's got all the excess I/O ins brought out where they can be used to play with all kinds of sensors or... stuff.

That board is not just about reading/displaying temperature. It's useful for all kinds of tasks!

That circuit board, fully loaded with all the options RTC, EEPROM, Onboard voltage regulator, LCD connector, etc costs about $15.

It's a learning tool for a PIC. What would you like to learn today?



steve

[TinkersALot]

Before anything else: Congratulations and Nice Job! This does look like it was a great learning experience -- especially with regard to re-arranging some parts and getting it to route into two layers. Interesting thread to read as well.

Don't mean to be thick-skulled about the purpose of your efforts. It is a neat board and project.

[Byte_Butcher]

Before anything else: Congratulations and Nice Job! This does look like it was a great learning experience -- especially with regard to re-arranging some parts and getting it to route into two layers.

It was actually a very good learning experience for me.
One of the best things I got from it was learning to use the "rats nest" feature on my PCB software.
The Rats Nest always freaked me out so I left it turned off.
After reading the tutorial that Robert posted the link to, I went ahead and turned the rats nest on... and learned to use it.
It really DOES help a lot in getting the parts laid out better and minimizing the amount of traces that have to wander all the way across the board.

Anyway, I should have boards here by the end of next week to test.
Hopefully there aren't too many mistakes...


steve

[Byte_Butcher]

UPS brought my boards yesterday!
I think I'm starting to really enjoy working with surface mount devices...
There's a certain pleasure in being able to put 63 parts (only 61 loaded in this photo), plus room for connections to the outside world (LCD display, sensors, power, etc) on only 4.5 square inches (29 sq cm) of real estate.

I loaded it up and ran it through the oven last night. Dunno if it WORKS yet, but it *looks* OK so far.



Here's a close up of the solder job. It's hard to resist the temptation to put too much solder on the pads. Just the tiniest bit is plenty. These look pretty good.



Big fun!

steve

[rsocor01]

Very nice!!!

Where did you buy your stencil from?

Robert

[Byte_Butcher]

Mmmm... if you mean a solder paste stencil, I've never used one. Yet...

For the small runs of boards I do, I apply paste by hand with a pointy tool under a magnifying lens. It took me less than 10 minutes to apply solder paste to all the pads on that board. (that includes going to the fridge and back for another beer). I'm hoping to be doing some larger runs of boards soon, so paste masks will become a necessity for me sooner or later (I hope).

I'd love to hear folks experiences with getting stencils made (cheaply)...


steve

[dhouston]

I've done them manually as you do and I've used a stencil. The thickness of the stencil controls the amount of paste applied. The stencil is preferred but for small parts and small quantities I still use manual methods. Here's a good source for stencils.

• http://www.quickstencil.com/prototype-stencil-kit.aspx

I've also seen less expensive mylar stencils but have not tried them.

• http://www.pololu.com/catalog/product/446

[rsocor01]

Wow, I didn't know you could make it without a stencil. But you are right, for a prototype why spending more money. I might try it in the future.

I have soldered 44-lead TQFP pics like the one you have in your pictures and I usually get my plastic stencils from www.ohararp.com. They are inexpensive and do the job. I have also tried pololu.com that was mentioned by dhouston. But for a bigger production I would recomend you panelizing your boards and using www.stencilsunlimited.com.

Robert

[Byte_Butcher]

Thanks Dave and Robert for the links!

I've bought from stencilsunlimited before.. that's where I got my solder paste and flux.

I took a quick look at the ohararp, pololo, and quickstencil sites and they got bookmarked for future reference. Sooner or later stencils will become a necessity for me.

Sure does make me drool to look at all the fancy laser cutters for making stencils, the PCB routers for making boards, and all the fancy reflow ovens and pick & place machines that are available now. All I need is a bunch of money. sigh...


steve