Large Via on VQFN-20 thermal pad PCB layout. Problems for me?

[rbm]

Hi,

Wanted an opinion about providing a large via on a thermal pad for a VQFN-20 package, whether it would adversely negatively affect the thermal conducting nature of the pad and cause soldering problems.

The package is a TI TPS7A470x series 36-V, 1-A LDO Voltage Regulator which will be used to convert 11V - 14V input into 5V at 120mA max current draw. The worst case power dissipation in the unit will therefore be (14-5)*.12 = 1.08W. Worst case ambient temperature will be 35°C.  The PCB is 2.5" x 1.5" giving 3.75 sq. in. of 1 oz. copper on the bottom.

As shown in the first picture below, TI recommends thermal vias on the PCB layout to conduct excess heat away from the package and on to the bottom layer of a 2-layer board.  I am providing such vias but the middle one is larger, as shown in the second picture from the Eagle layout, so that I can hand solder the VQFN's thermal pad from the rear of the board with a soldering iron.  I am hand soldering the SMD components rather than using an air soldering station or reflow oven because I lack these tools.

[Ian.M]

If you fill it with solder and sweat on a square of thin copper sheet on the back as a heat spreader, that should be significantly better than the recommended thermal via size/pattern as you've got *SO* much more metal CSA. that it will compensate for the solder only beiing about 15% as thermally conductive as copper.   Even without the solder fill, if the package has an adequate internal heat spreader its probably better just because it has more through-copper nearer the edges of the the thermal pad due to the increased circumfrance of the center hole.

See https://www.electronics-cooling.com/2006/08/thermal-conductivity-of-solders/
For comparison, pure copper is approx. 400 W/(m K), electroplated copper can be as low as 300 W/(m K)

[DerekG]

I am hand soldering the SMD components rather than using an air soldering station or reflow oven because I lack these tools.

My advice would be to use a through hole regulator as you are hand soldering anyway. As you are only dissipating around 1W, you will find that an existing TO-220 (or TO-263 etc) that will handle the power without having to add an extra heatsink.

A through hole regulator is also likely to cost less than the proposed part above (along with using less real estate on your board).

If height is a problem, bend the through hole regulator so it is parallel with the PCB. If you want some copper to dissipate more heat, place a plated hole on the board & open up the solder mask on the top side. Screwing up a nut & screw is likely to take you less time than hand soldering the heat dissipation pad as you describe above.

[Ian.M]

Yes, unless there is a severe space or board area constraint forcing you to a small footprint low profile solution like a QFN package, a LM7805 would probably make more sense, either TO-220 through hole or D2PAK SMD.   However if you bolt a TO-220 one down to a PCB for better heatsinking a spring washer is essential (not a serrated washer) to maintain contact pressure as FR4 tends to cold flow under compression loads.

[rbm]

Thanks Ian and Derek.

I'm actually redesigning the layout, moving away from a three-pin regulator to this VQFN package.  Below is a picture of the current design:



There were two reasons for the redesign:

• The high efficiency TO220 style regulator from Rohm that I was using in the design became NLA and all stock disappeared from my suppliers.  I couldn't find a replacement from another manufacturer with the physical characteristics of the Rohm.
• I'm currently out of onhand stock of boards and regulators and I have a pending circuit update to apply, so it is an opportune time to change.

There are board size and height constraints that don't allow me any room for the regulator to lay completely flat against the board or stand upright. The cost of the TPS7A4700 I'm considering is very low because I have a whole reel of them that I bought from a surplus supplier.  My anticipated run of boards will not exhaust my current stock, so they are effectively a couple cents per unit.  I have had issues in the past with linear TO220 regulators in this operating environment shutting down from excessive temperature even though the power being dissipated was low.  I've not had that problem with the switching regulators.

Before I commit to this design, I'll run some stress tests on the circuit.  I have a VQFN-20 prototyping board coming in the Post.

I might just go back to a TO220 based three-pin regulator design as both of you suggest if I can re-work the board layout.

[Ian.M]

I assume the Rohm regulator is a switching one and is the glossy black three pin Hybrid in the middle.

Errr . . . . . I just googled the TPS7A4700 datasheet and confirmed its a fairly ordinary linear LDO.   Neglecting the few mA difference in their ground pin currents, its dissipation will be pretty much identical to a 'jellybean' 7805.  I doubt it will do any better unless its got a significantly higher Tj_max thermal limit or you give it a LOT more copper area.  Finding space to go to a D2PAK three pin regulator with a close spaced ring of thermal Vias through to a ground plane round the edge of the pad for its tab would probably do more for dumping heat than changing to your QFN regulator.   You should also squeeze as much copper in topside round the tab as you can.   OTOH its certainly worth doing a test PCB if the QFN regulators are essentially 'free' and you've got the time to experiment if they can do the job and assess what the extra labour costs would be.   

My experiences with 78xx regulators are they tend to die Hi-Z if run on the ragged edge of thermal limiting for an extended period.   If the tab's too hot to touch you need to add heatsinking or reduce the dissipation by whatever means possible.

It *MAY* be worth a few degrees to go to matte black soldermask in the hope of getting better IR heat transfer, but that's highly dependent on the IR emissivity of the actual mask used, and the wall emissivity and wall temperature of the enclosure.

Worst case you may have to bite the bullet (for the design pain) and go to a switching regulator with external inductor.

[KL27x]

You are dropping minimum of 6-9V. The LDO only needs a third of a volt of overhead at this level of current.

A linear regulator is essentially a variable resistor with feedback. And in this circuit, the minimum value of that variable resistance is exactly 50R = (11V-5V)/0.120A. You could put up to a 45 ohm series resistor rated for 2/3W between the power rail of the car and Vin on your LDO, and still get a minimum Vin of over 5.5V at 120mA max draw. When you do this, the regulator has to drop only a small fraction of the total, when at max draw of 120mA. That is if you are using 11V as the minimum voltage of the vehicle when the engine is off; personally, I would go 10.5V. To allow copious room for error and tolerances, I might try 40R 1W resistor.

This will dissipate up to 2/3 of that 1W of heat in the series resistor when the engine is running (and even larger percentage of the total wattage when the engine is off), which you could strategically place away from your regulator.  A resistor can typically run up to 200C, sustained/indefinitely, which means it can operate at a higher differential to ambient which means you can effectively get that level of dissipation with less copper/heatsinking. With a thru hole part, you can achieve this largely through ambient air cooling, with relatively smaller amount of heat back dissipated by the PCB other than what is transferred through radiation and through conduction via the resistor leads. In addition, a resistor has a positive temp coefficient to prevent runaway failure, and it can be strategically placed anywhere you want on the PCB to keep it away from the regulator and other high temperature and/or temp-sensitive silicon.

The series resistor might induce oscillation/instability of the Vout, particularly because this is a LOW DO regulator. But it depends on your load and power supply and is not necessarily going to be a problem; if it is a problem, more low ESR input caps in parallel might be all it takes. A voltage regulator is designed to give a stable Vout despite change to Vin and/or load. Using it as a power resistor is fine when you have excess capacity. If you are cutting it close, might as well separate the two functions and leave the regulator to only disspate closer to the minimal amount of heat that it must to take care of the variable part of the equation.

Depending on how you want to look at it, you could also view this series resistor as increasing the output impedance (voltage sag under load) of your Vin rail in such a way that at max load the rail barely covers the overhead requirement of the voltage regulator.

[rbm]

Thanks for the suggestion to drop my input voltage to the circuit.  Unfortunately, that 12V going to the regulator to power the analog and digital circuitry is also feeding into an on-board switching transistor.  Therefore, I still need 12V to the board.  That would mean provisioning for a relatively large resistor onboard and I haven't the room. Remember I'm constrained with size and height in this application.

I'll probably go with a high efficiency switching regulator with a LM78* pinout.  that's worked in the past and all I need to do is re-arrange the components on the board to accommodate the slightly larger Recom device that will substitute for the discontinued Rohm device. 

[PCB.Wiz]

Wanted an opinion about providing a large via on a thermal pad for a VQFN-20 package, whether it would adversely negatively affect the thermal conducting nature of the pad and cause soldering problems.

The large via would be fine.... solder is better thermally than fibreglass.

The package is a TI TPS7A470x series 36-V, 1-A LDO Voltage Regulator which will be used to convert 11V - 14V input into 5V at 120mA max current draw. The worst case power dissipation in the unit will therefore be (14-5)*.12 = 1.08W. Worst case ambient temperature will be 35°C.  The PCB is 2.5" x 1.5" giving 3.75 sq. in. of 1 oz. copper on the bottom.

That's a bigger problem - if you were using a switching regulator, and need to manage 1.08W in a linear unit, that's quite a lot of power into a small PCB area, which seems already constrained.

I'll probably go with a high efficiency switching regulator with a LM78* pinout.  that's worked in the past and all I need to do is re-arrange the components on the board to accommodate the slightly larger Recom device that will substitute for the discontinued Rohm device. 

That's sounding better - you might want to also allow for some other vendors similar to recom (eg CUI), to give you some supply options.

[montemcguire]

Thanks for the suggestion to drop my input voltage to the circuit.  Unfortunately, that 12V going to the regulator to power the analog and digital circuitry is also feeding into an on-board switching transistor.  Therefore, I still need 12V to the board.  That would mean provisioning for a relatively large resistor onboard and I haven't the room. Remember I'm constrained with size and height in this application.

Rather than a resistor, you could use a zener diode or a string of conventional diodes to soak up excess voltage. The benefit compared to a resistor is that an SMD diode will have a nice footprint that can thermally connect well to PCB copper, and because its voltage drop is less dependent on current, it will not mess up the input regulation over a wider range of regulator load currents.

I'll probably go with a high efficiency switching regulator with a LM78* pinout.  that's worked in the past and all I need to do is re-arrange the components on the board to accommodate the slightly larger Recom device that will substitute for the discontinued Rohm device.

I haven't used these TI regulators specifically, but they are some of the few modern regulators that have extremely low noise (about 40x less than an LM317 at 5V), low output impedance, high PSRR, and are also available with a negative complement. So, I say use them and just deal with the dissipation in some way. Ian.M's idea of using a good bit of copper shim on the back side of the PCB is a good one, as is the simpler idea of just laying out a large enough area of foil on the PCB side opposite the regulator. In the TPS7A470x datasheet, figure 27 shows the mounted theta-j-a parameter vs. PCB foil area, and with only 1 square inch of foil, you get about 60 degrees C per watt, which will be within the safe operating area, and somewhat away from thermal shutdown. I'd try to use more foil, but if you have a ground plane, the DAP can be directly attached to that, yielding a lot more copper area. Additional stitching vias that connect the bottom side DAP ground foil to a top ground pour will also help to sink away heat from the bottom foil to the top side. I think in practice that these parts are not impossible to use, and possibly also with an input zener or conventional diodes to reduce the regulator drop, you can make them work thermally and enjoy their super high performance and modern convenience features.