What is standard copper thickness for MCPCB?

[ftsolutions]

If you attach a larger copper pour to the thermal pad, it will help to some extent, if nothing else, to increase the surface area through which the heat is dissipated (which essentially increases the thermal transfer efficiency). This will be part of the thermal dissipation from the LED (some will be through the terminal pads of the LED). So, I do concur that it could help reduce the temperature of the LED to some extent if used to extend the area of the thermal pad. How much is unclear to me, but copper is an excellent thermal conductor. I think the design could be OK without it, but if you are going to pour the copper areas on the top side, they might as well be doing something useful by connecting to thermal pads, even by small area, and if it helps the individual LED run a few degrees cooler than that will only help the longevity of the components. It will help to spread the small "point sources" of thermal energy into somewhat larger square area, which will in turn improve the rate of thermal transfer through dielectric to the aluminum substrate.

 

[FvM]

The discussion demonstrates well why it's a bad habit to split related questions of one design over multiple threads. At the end you're jumping back and force between information given in one or the other places.

I believe that a better layout suggestion has been made by marce, which is however deviating from the Luxeon datasheet design.

If its a single sided design with metal clad PCB I fasten it to one of the other pads just to increase the actual copper connected to the led.

You don't get an overall copper pour rather than individual heat sink areas for one or two LEDs. The solutions also gets rid of possible dielectric strength limits.

 

[treez]

If so, then you can probably go back to using ordinary 1206 or 2010 O-ohm resistors as well.

I must admit, chip resistors just seem terribly delicate to me, like small pieces of bathroom wall tiling. Do you believe that SMD chip resistors may fracture when mounted on MCPCB due to the differences in thermal coefficient of expansion between the aluminium of the MCPCB and the material of the chip resistor?

Are there any cheap jumpers which are like bits of bent metal strip and can handle expansion/contraction of the underlying aluminium of the MCPCB?

Only if I could not accomplish this for some reason would I resort to having to do the "inside-out" jumpering here on this layout.

Thanks again, i will put the jumpes into the other lines and not the ground?

 

[ftsolutions]

>>>The discussion demonstrates well why it's a bad habit to split related questions of one design over multiple threads. At the end you're jumping back and force between information given in one or the other places.
I completely agree, I tired of trying to keep track of the multiple parallel paths on these and didn't always notice what others had replied on some of them. It is best practice to keep related things together, in my opinion!

I must admit, chip resistors just seem terribly delicate to me, like small pieces of bathroom wall tiling. Do you believe that SMD chip resistors may fracture when mounted on MCPCB due to the differences in thermal coefficient of expansion between the aluminium of the MCPCB and the material of the chip resistor?

Are there any cheap jumpers which are like bits of bent metal strip and can handle expansion/contraction of the underlying aluminium of the MCPCB?

Thanks again, i will put the jumpes into the other lines and not the ground?

Chip resistors are most frequently used on these types of boards - the good thing with metal substrate is that if the heat sources are anywhere near to reasonably placed, the entire assembly tends to warm up/cool down more evenly than boards that incorporate FR4 into their stackup. I just avoid trying to use tiny parts on them as they are certainly more fragile, have less solder joint area, and are like trying to solder/desolder grains of sand to the bottom of a copper frying pan when it comes to assembling these. So, the smallest parts I have used on commercial/industrial products with these type of constructions are 0603, and I usually use 0805 or above. Power handling issues can also come into the choice. If the soldering is properly done and the board is decently heatsinked, all should be OK as far as SMD chip resistors go.

As to SMD LED thermal pads - any increase in their area will help to improve lowering the junction temperature of the LEDs. How much we don't know without sophisticated modeling. It may be good to add some copper and connect to nearby thermal pads as Marce suggests to help in this manner, but not necessarily tie all the thermal pads to the largest area pours you have as far as solderability goes. More surface area = good for heat transfer, but if it makes it to hard to get reliable solder paste reflow under the parts because of so much thermal mass/heat transfer, the poor solder connection at the pad could undo the benefit of having the huge area for heat dissipation. I think I would add some extra copper to connect to these pads, but not go to tying every thermal pad to the largest copper pour I can make. Again, these dielectrics (at least those I have used) transfer heat VERY well. Dielectric strength of the HT Bergquist material is quite good - it holds up well with large motor voltages and in one of my designs, 250V DC with surface contamination by industrial ink solvents was not a problem. I suspect other vendors have materials of similar characteristics.

If you cannot reorganize your trace routing/component rotation to facilitate what I proposed in previous post, I think the routing is still OK from thermal perspective. I am just trying to get you to think about how to improve on it, make it more reliable/cleaner, if your application constraints will allow. With IMS boards (or any boards) having a clean layout with fewer jumps often forces one to think more carefully of best part placement, trace widths, etc and other improvements might also be noticed. Fewer jumpers will also mean fewer potential parts that can fail, and by removing jumpers from the return leg which must pass the most current, you also help to address the power dissipation issue by having jumpers that feed only 1 or 2 of the strings at a time. If you have other constraints and cannot make these routing suggestions work, the thing won't blow up - but these are the sorts of things that any good layout designer should do for any type of PCB design. I get paid alot of money for my design work, and people expect me to provide the best possible design to the constraints that I am given to work with.