Newbie Question: Calculating correct via for power traces.

[JoeN]

I am trying to design a motor controller.  It has an external dual H-bridge using 8 N-channel MOSFETs in D2PAK .  I am doing it in Diptrace and plan to sent it to OSH Park.  The PCB will be 1 oz copper, 2 layer.  I am using 12 mil tracks for logic and power to logic circuits (low power non-driver logic).  I am using 30 mil tracks for power traces between the motor and the MOSFETs and power supply.  A PCB track calculator says this is good for 2A with a 10 degree C temperature rise.  I could go bigger on the traces but I want to keep the board as small as possible for this first shot - trying to pack this into 5 square inches.

Right now my vias are 13 mils outer and 6 mils inner.  I think DipTrace chose this for me.  This has always worked for me before for logic.  Should it be increased in some way for those 30 mil power traces?  How do I figure that one out?  The one calculator I found for this just confuses me.

Thanks for any advice!

[tszaboo]

This looks wrong. There is no bypassing on the power input, the powerpad on the U1 driver(?) doesnt have any vias, so no cooling, the voltage regulator has minimal footprint, so no cooling, your mosfets have no cooling, 2A is a little bit too much for 2.54mm headers. Traces are all over the place, 90 degrees traces. You have enough place to triple/quadruple the traces on the power section, dont be lazy. You can use ten via, it will cost you the same as if you use one.

[JoeN]

This looks wrong. There is no bypassing on the power input, the powerpad on the U1 driver(?) doesnt have any vias, so no cooling, the voltage regulator has minimal footprint, so no cooling, your mosfets have no cooling, 2A is a little bit too much for 2.54mm headers. Traces are all over the place, 90 degrees traces. You have enough place to triple/quadruple the traces on the power section, dont be lazy. You can use ten via, it will cost you the same as if you use one.

There are through holes for a 2200uF/16V electrolytic cap to the right of the barrel jack in the top left.  It isn't labeled.  I had to smash it to move the pads around a bit and it lost the label.  God knows if this is the right value, it's only a guess.  There are smaller bypassing caps all over the place, the big cap is meant for the power section up top.

I wonder how to via stitch the powerpad.  Thanks for the advice there.   I will try to figure it out.  Also, thanks for bringing my attention to it.  It is supposed to be connected to ground and is not.  I thought I had done that.

That regulator is providing 5V for the microcontroller and the microcontroller is providing 3.3V to the QFN.  I don't see it getting very warm.  But now that I think about it, it may be completely unwise to hang the driver IC off the microcontroller so I think I should put a dedicated regulator on there.  But what do you suggest here?  What do you mean by footprint - just give it more space on the PCB?  Or make some of the copper larger and via stitch that too?

90 degree traces are bad?  Should I break those down to 45?  Does it really matter for logic traces?

2A is a little bit too much for 2.54mm headers?  I don't understand.  The current comes in the DC barrel jack, top left corner, out the 5mm headers which are rated for 20A.  (http://www.taydaelectronics.com/connectors-sockets/terminal-blocks/pluggable/4-pin-male-plug-in-type-terminal-block-5mm-5ehdrc.html).  Am I overrating the barrel jack?  I don't know what the recommendation on that is, I got those as no-name no-datasheet parts.

How to cool MOSFETs with respect to the PCB?  My brilliant idea was just to throw a heat sink on them if necessary.  With through-hole ones I know the normal idea is to stand them up and tie bind the heat sink onto the metal in the rear.  What is recommended for SMT?  Is this a place where you put copper on both sides and via stitch it?

And what about the vias anyway?  Are they too small or are they actually right for the larger traces?

Thanks for any more suggestions!

[T3sl4co1l]

Schematic?

At 2A, the choice of MOSFET seems strange.  You can get SOT-23s that'll handle that with aplomb... though you might want a power package (SOT-89, -223 or SO-8 range) to have a couple microseconds leeway before they poof, in case of poof-inducing conditions.  Shouldn't need to bring out D/2PAKs until 12V/10A+ range, I think?

Trace width is OK but as long as you have the space, you can always go bigger.  More important though is to have lots of extra copper area on the tabs.  As shown, you'll get about a watt of dissipation in each transistor before magic smoke.  Yes, the datasheet says 200W or something stupid like that, and yes they lie.  You don't get much heat out of a PCB, but you can at least dissipate 2, maybe 3W safely with up to 2 in^2 of copper pour per transistor (up to maybe 4W and 4 in^2 if you splurge for 2oz copper).

Minimum via size is a manufacturing issue.  Ask the board shop.  They should have it on their website.  Standard minimum is 8 mil hole, 5 mil annular ring (= 18 mil pad).  Cheap fabs will either upsize them anyway, or charge more for teensy holes -- a practical "I don't need anything special" minimum is 12 mil hole, 30 mil pad (that's almost a full 10 mil annular ring -- their drilling can be total shit and you'll still get a good ring around the hole).

Likewise, trace width/space minimum is around 6 or 7 mil for most fabs.  I go with 10 or even 12 or 15 for "I don't need anything special" rules.  It's worth following, even if you break the rule in some places by necessity (like that damn part you can only find in 0.5mm pitch TQFP).  More clearance in more places is less chance for electrical failures.  And don't count on cheap fabs to do thorough electrical testing -- you get what you pay for.  Ultimately, you're responsible for your own vigilance...

Clearance should go up by about 10 mil per 50V, so line operated stuff needs 30-50 mil clearance.  (Protip: that's for "transient limited", functional insulation -- the stuff between traces on the line side.  Line-to-ground or line-to-something-the-user-can-touch isolation needs to be much wider, often assisted with actual slots cut right through the board.)

And definitely do pour grounded copper around everything you can.  This greatly reduces loop inductances, and shields signals from each other and from outside influences.  Stitch it with vias at least every inch, staggered either side of traces, on peninsulas, floating areas, etc.  Examine closely the negative space around traces, top and bottom; try to get as much top-to-bottom overlap as possible, and stitch around "holes" where you can't get ground to reach.  Ideally, every trace always runs above or below a solid piece of ground.

If you have free space on the back side, put heat dissipation pours there, too.  Now, your circuit will necessarily have pads that aren't grounded, so you can't go connecting them with ground plane (which would be the easiest), but you can still make the pours expand into most of the nearby area, and stitch them to the top side pours.

Tim

[tszaboo]

There are through holes for a 2200uF/16V electrolytic cap to the right of the barrel jack in the top left.  It isn't labeled.  I had to smash it to move the pads around a bit and it lost the label.  God knows if this is the right value, it's only a guess.  There are smaller bypassing caps all over the place, the big cap is meant for the power section up top.

OK, that is good. You might want to run the traces through the capacitor, and after that to the rest of the circuit.

I wonder how to via stitch the powerpad.  Thanks for the advice there.   I will try to figure it out.  Also, thanks for bringing my attention to it.  It is supposed to be connected to ground and is not.  I thought I had done that.

I think it is enough to put some 3x3/4x4 0.3mm/0.4mm vias under that package. Make sure it is not covered by soldermask

That regulator is providing 5V for the microcontroller and the microcontroller is providing 3.3V to the QFN.  I don't see it getting very warm.  But now that I think about it, it may be completely unwise to hang the driver IC off the microcontroller so I think I should put a dedicated regulator on there.  But what do you suggest here?  What do you mean by footprint - just give it more space on the PCB?  Or make some of the copper larger and via stitch that too?

I would use a separate regulator indeed. And yes, more copper.

90 degree traces are bad?  Should I break those down to 45?  Does it really matter for logic traces?

135 degrees, if you think about it.

2A is a little bit too much for 2.54mm headers?  I don't understand.  The current comes in the DC barrel jack, top left corner, out the 5mm headers which are rated for 20A.  (http://www.taydaelectronics.com/connectors-sockets/terminal-blocks/pluggable/4-pin-male-plug-in-type-terminal-block-5mm-5ehdrc.html).  Am I overrating the barrel jack?  I don't know what the recommendation on that is, I got those as no-name no-datasheet parts.

Sorry, those seemed smaller. Those terminal posts are OK for 2A.

How to cool MOSFETs with respect to the PCB?  My brilliant idea was just to throw a heat sink on them if necessary.  With through-hole ones I know the normal idea is to stand them up and tie bind the heat sink onto the metal in the rear.  What is recommended for SMT?  Is this a place where you put copper on both sides and via stitch it?

More copper, that will definitely help. You can realistically dissipate 3-4W on this with more copper before it gets warm, should be OK.

And what about the vias anyway?  Are they too small or are they actually right for the larger traces?

Thanks for any more suggestions!

They look small to me.
You are welcome.

[JoeN]

With respect to the topic of thermal relief that has come up, I want to run what I have done so far by you.  It doesn't look like DipTrace has any automated via stitching or patterns that have thermal relief.  All the parts with power pads are top layer only, at least that is how they come out by default.  So I copied the TO252-3/10x6.6x2.28 part and modified it in this was:  1.  I changed pad 3 which is the big guy to "through hole" which makes copper appear on both sides.  I made it about 50% larger.  Now, there are no vias in the pattern editor so I made a bunch of plated through holes.  At least they come plated from my manufacturer.  I don't see an option for that.  Here is the before part:



Here is the frankenpart:



Here is the preliminary board:



Will this work?  It seems sketchy to me.  But, if it will work I will add this to the regulator and driver power pad as well.  Will my fabricator hate me?

[T3sl4co1l]

It's a start; do you have any copper pour on the backside too?

Shouldn't have to embed vias in the footprint, unless it throws an error on via-in-pad and you can't make an exception.

Via-in-pad is undesirable for reflow soldering (you're better off placing them around the periphery of the pad instead), but OK (or even better) for hand soldering.

Tim

[JoeN]

It's a start; do you have any copper pour on the backside too?
Tim

The copper pads on the bottom are exactly the same as the copper on the top.  The copper and therefore the MOSFET drains are not connected on the back.  I'm not sure how I could make it larger.  If it is larger then the copper will be connected which means the drains will be connected together.  For the drains of the four MOSFETs on the top of the two h-bridges they all connected to the same thing (the main voltage) this is OK.  For the other four, the bottom MOSFETs of the two bridges, it is not, the drains have to be electrically isolated from each other.

Shouldn't have to embed vias in the footprint, unless it throws an error on via-in-pad and you can't make an exception.

I realize I can make vias in the actual PCB layout.  But then, I have to do it for every part I want via stitching in and if I want to do this with another PCB design, I have to put vias into the PCB for that too.  Isn't it preferable to make a part with it built in and then you can lay out that part as many times as you wish?

Via-in-pad is undesirable for reflow soldering (you're better off placing them around the periphery of the pad instead), but OK (or even better) for hand soldering.

I was using adapter boards that I have seen with stitching as my guide, like this one below.  I use these.  They work fine for prototyping.



But just go around the edges?  On the ones above, just lay down the outermost ring of vias and forget the rest?  To prevent solder from flowing through?  I was probably going to build this by hand with a hot air gun anyway...

[EEVblog]

Get the Saturn PCB Toolkit calculator, it's awesome.
http://www.saturnpcb.com/pcb_toolkit.htm

[T3sl4co1l]

I realize I can make vias in the actual PCB layout.  But then, I have to do it for every part I want via stitching in and if I want to do this with another PCB design, I have to put vias into the PCB for that too.  Isn't it preferable to make a part with it built in and then you can lay out that part as many times as you wish?

What if you don't need vias?  What if you need a few in odd positions?

One of those either-or situations where you need to maintain more footprints, or always do it by hand.  YMMV, but most tools you can simply copy and paste vias, so it's easier repeating them than making and maintaining footprints.

I was using adapter boards that I have seen with stitching as my guide, like this one below.  I use these.  They work fine for prototyping.

[pic]

But just go around the edges?  On the ones above, just lay down the outermost ring of vias and forget the rest?  To prevent solder from flowing through?  I was probably going to build this by hand with a hot air gun anyway...

Those can't be done otherwise, for a few reasons:
- You can't connect to a buried pad with anything else
- It's for heat dissipation (usually), so you aren't getting the heat out any other way
- On a proto board, you'll probably be hand soldering it, so you need the vias to wick solder to do the job (or you can reflow, but in that case you can control the amount of excess solder).  Reliability probably doesn't matter either.
- On a production board, you use small vias (12 mils or less), which have less tendancy to wick solder.  You can also design in enough excess solder, and the right number of vias, with the intent that the excess solder wicks into them.  Otherwise, a flat build (no wicking) should use less than full pad area for solder.  This is usually shown on the footprint drawing.

There's no room for vias around the pad, or that would obstruct what routing area you might have, anyway.

Likewise, LGAs and BGAs have such density that you have no choice but to use a "dogbone" or ViP fanout.  Especially for these, you want to avoid ViP unless you're going to use a capped or filled via process (added steps = added expense).  (Tenting isn't good enough, especially double side tenting, because the hollow via will inevitably trap gas.)

So it's different for pads that have accessibility around them.  You can place vias very near (even tangent with, but not inside) the pad, tented or otherwise (preferably tented so they don't steal solder), and don't have to worry about wicking or gas bubbles.  Place a copper polygon around pad and vias, top and bottom.

There's little point in using vias if you aren't going to put copper on the bottom.  In that case, just leave as much extra copper on the top as you can.

Tim