Ask Me Anything with Keven Coates

Login to ask your questions and Keven will reply on October 25th!

Hi Keven, do you have thermal design guidelines and best practices you can share for PCB layout?

Hi Keven. Our customers often have issues with heat dissipation. What are the common methods for dssipating heat would you recommend to them?

Hi Keven. What would you say the primary cause of heat generation is? What do you think designers should watch out for?

How do you calculate thermal resistance

Hi Keven! Can you explain the importance of thermal vias in PCB design?

What is the role of a heat sink in heat management, and how do you choose the right one? How does the choice of PCB material impact heat dissipation?

Can you discuss thermal relief patterns in SMT components?

Hello Keven! What are the considerations for thermal management in high-power applications, such as power amplifiers or processors?

I have another question. Can you explain how simulation tools can be used to optimize heat management?

Any recommendations for component placement and trace routing for heat dissipation?

Thanks so much for your question! Can you be more specific about the power levels and situation you are facing? Is this specifically for SMD PCB heat management?

Hi Keven!

Yes, this is specific to SMD

There are 2 big causes of heat on PCBs, one is power components (caused by internal resistance) like MOSFETs, transistors, etc. and the other is gate switching.

Inside processors there are millions, maybe billions of gates that make up the logic of the processor. Each gate has a small amount of capacitance. If a million gates are switching on or off every clock cycle, 4 billion times a second (4 GHz), there is obviously some power draw and heat generated.

As far as what to watch out for, this goes back to the key of heat management which is to spread out the heat. All heat management is about spreading out the heat so that it may be transferred to the air more efficiently. All heat has to eventually make it to the air, so spreading the heat is key.

What to watch out for? Isolating heat. This is the opposite of spreading the heat. If you place your LDO regulators (for example) on tiny copper pads, the heat will be isolated and not able to spread efficiently. On the other hand, if you place your LDO on vastly oversized pads (a large amount of copper) that same heat will be spread out and most of it can be transferred to the air. This is the key to heat management.

Yes, great question! As I wrote “thebalancedbliss.blo”, the key to heat management is to spread out the heat, so all my recommendations are about doing that in practical and low cost ways.

  1. The first tip for heat management is to try not to generate heat in the first place. Buck regulators, for example, are more expensive than LDO regulators, but may reduce the amount of heat in the system enough to save you money overall (because heat management can be expensive).
  2. Anytime you have a heat generating component, allocate some space for it on your PCB. Larger pads, traces, etc. (all copper area) are all a great way to spread the heat so that it can be dissipated to the air. This means large pads for the tabs on LDO regulators, thick trace widths to pins, etc.
  3. 2oz copper is another great way to spread the heat. 2oz copper spreads heat much better than thinner copper, but obviously you’ll have to make sure you can use it on your PCB due to the larger trace/space requirement for the thicker copper.
  4. Thermal vias are another great way to spread the heat. If you can couple your MOSFET, LDO, or LED to a ground plane, power plane, or copper area on the other side of the PCB, you’ve just increased your copper/heatsink area and spread out the heat.
  5. Larger components are also helpful. If you have the choice between a 2mm x 2mm MOSFET and a 5mm x 5mm MOSFET, chose the larger one since it’s already spreading the heat much better. You can even use multiple MOSFETs to spread the heat further, and while this is more expensive, it may be cheaper overall if it avoids a heat sink.
  6. If you are spreading the heat through copper area on the PCB, avoid corners. Corners limit how much you can use the PCB copper to spread heat.
    I’ll go over all these in great detail in my class on Jan. 24th.
    Thanks for this question!

Thanks for your question! I think this is essentially the same question asked by apekshak, so please read the answers I wrote there, and if you have any other questions, feel free to ask during this hour.

Simple resistor type thermal equations are easy to understand as long as you see them as steady state estimations.

Imagine the source of the heat, usually a silicon junction inside a MOSFET, (for example). From there to the outside of the package is a resistance, we call this theta JC (the resistance from the junction to the case) and so on until you get to the air (the final destination of all heat).

To calculate the thermal resistance of say, a PCB copper area or heatsink you would add up the thermal resistances that you know (like the junction to case resistance, etc.) and measure the input heat and output heat, then subtract the ambient temp and calculate.

For example, let’s say you have a MOSFET on a heat sink with a theta JC of 1 degree C/Watt. To calculate the heatsink resistance (theta CA, which would combine the resistance from the case to the heatsink and the resistance from the heatsink to the ambient), you’d heat the MOSFET with 1W (or any power level) of electrical heat, measure the case temperature, and work backwards.

If you measure 51 degrees C. then you subtract ambient (25C) = 26C of temp rise. Then you subtract the junction to case resistance (1 degree C/W) = 25C and you’ve got your answer. 25 degrees C/W.

Thanks for the question!

Sure, I would recommend anything that spreads out the heat.

For example, if you plan on using PCB copper to cool your components, don’t put them in the corner where the area is limited by the board edge, put it close to the middle where the heat can more easily spread.

As far as trace routing, it’s not so much about the routing as it is the trace widths. Wider traces take heat away from components (by spreading it out), so wide traces on power resistors, MOSFETs, etc. are a big help.

Obviously airflow affects cooling as well, so if your airflow is greater in one area, put the hot components there.

Thanks for the question!

Simulation tools are a great asset to complex heating problems. They are only estimations as nothing is completely accurate, but they can help with situations where board airflow is variable across the board, and ambient heating causes an unknown airflow, especially where more than one component is heating things up and air can travel in many directions.

For simple situations where just a few discrete heat sources are present, software is not needed, but for situations where you’re trying to do something complex, like use the aluminum case to cool components, they can be a life saver.

How you use them depends greatly on the tool.

I hope this answers your question. Thanks!

Thermal reliefs are kind of a mixed bag, right? On one hand, you want to isolate the pad from the surround copper so that rework is easier, but on the other hand you want the component to be as cool as possible, which means minimizing the relief (or no relief at all) because thermal reliefs reduce heat spreading.

It’s not so much about the pattern or design of the relief, but the percentage of copper from the pad to the surrounding area.

You could get into some tweaking like doing more open area on the outside of the pad in a TQFP to encourage proper melting of the solder closer to the part, but I’m not sure anyone has done a lot of studies on that.

For heat, you want the thermal relief to be as minimal as possible. No thermal relief would be best, but your rework people may be upset with this. Board pre-heaters can make rework possible in these situations.

The answer to what’s best is a compromise between rework and heat spreading. Only you can choose what works for your design.