I want to know the concept of plating in pcb aand what is its significance? while simulating through hyperlynx do we need to take care of Plating thickness while stac up editing.
Such as SnPb plating over copper trace on outside layer will impact at very high frequency due to it's conductivity and roughness, merely Hyperlynx can't
do this type of analysis. There are some method or tool to assit this type of analysis. Recent papers discuss it in detail, also it have be dicussed in Designcons.
For copper plating, you don't need to care of it if you have set the stackup with correct finished copper thiness.
In a PCB manufacturing process, there are two main type of plating
1. Copper Plating (Electroless Copper Plating followed by Electro Plating)
2. Final Finish Plating
For the first one you need to consider the finished Cu in external layers (Assuming that you only through holes vias from primary to secondary side). Per IPC-6012, the barrel plating thickness varies from class to class. If you have a minimum barrel thickness of X mils minimum, then your external layer Cu will be base Cu + 1.3 to 1.44 of X.
The final finish generally won’t be added to trace. Most of the suppliers go with SMOBC (Solder Mask over bare Cu) with HASL or Fused tin Lead. There are cases where the Solder mask may apply over ENIG. This thickness will be few micro inches.
yes. I just anwsed the question in high speed side, and you explained the question in manufacturing side
So i can conclude that in stack up we have to consider only finished thickness in outer layer (Top & Bottom) i.e. 1 OZ or may be 1/2 OZ of copper.We do not have to worry about plating & Soldermask thickness in stack up for Hyperlynx simulation.
normally, 1/2oz or 1oz copper thinkness only have 1.5% around variation to calculated Impedence value, and soldmask also have 1.5% around effect . because it's very difficut to precisely calculate out the effect of sourface finishing material and it only take noticible effect on 20Ghz above, so don't warry
lot of thanks to both of you for your kind reply.
Yu is correct, Impedance won’t have a big variation will be within 10% in the finished PCB. But when you go for PI the finished Cu thickness will help in getting the optimum thickness.
Retrieving data ...