4 Replies Latest reply on Feb 24, 2014 7:46 AM by wolferm

    Designing a PCB with thermal relief

    harry-stone

      We have a new PCB that has 10 layers. There are plenty of gnd and power planes. I have had to do some modifications to this board, including removing and replacing components. I have plenty of experience with soldering and I believe this is one of the hardest boards to work on. What I am asking is what techniques, tips, etc. I can use when designing a circuit board that would give thermal relief and not be as difficult if the need for hand soldering is needed.

       

      Thanks

        • 1. Re: Designing a PCB with thermal relief
          RLS2004

          The notes below are from a web forum (Probably TomH at pcbl):

           

          Total cumulative copper web for all layers in any plated through hole should not exceed 4.0 mm for 1 oz copper or 2.0 mm for 2 oz copper.

           

          It means that if you have a 12 layer board and 4 GND planes, the accumulative spoke width on all 4 GND layers should not exceed 4 mm for 1 oz copper or 2mm for 2 oz copper. If you violate this rule you will get "Cold Solder Joints".

           

          (Removing the part also gets difficult! Hope this helps).

          RLS

          • 2. Re: Designing a PCB with thermal relief
            sabitha.jamal

            Hello

             

                   But if we are using the spokes on extreme bottom layers the solder results will be good 

             

            Thanks and Regards

            Sabitha

            • 3. Re: Designing a PCB with thermal relief
              harry-stone

              Can you explain the accumulative spoke width. Does this mean the total spoke width for each via cannot exceed 4mm for 1 oz and 2mm for 2 oz of copper.

              I have a spoke width that is 0.381mm per spoke. Do you multiply that by four spokes, and if that number is below 4 mm for layers with 1 oz and under 2mm for 2oz you are designing within this thermal relief rule.

              Thanks

              HS

              • 4. Re: Designing a PCB with thermal relief
                wolferm

                I believe the answer "total acumulative on all layers" pretty much covers it.

                In other words on any one thru hole pin that requires soldering if you have a 1oz copper bd and have 4 duplicate plane layers that this thermal pin will connect to

                then that is 4 spokes X 4 layers equals 16, then take the 4mm divided by 16 equals .25mm or approx 10mil width for each spoke width max.

                To be clear on terms, you state spokes for vias and not part holes, if these really are just vias you are concerned with why aren't you just making then solid connections and no thermals.

                vias usually do not need thermal relief at ll unless ou are trying to solder wires or smeting to them.