I am wondering what are the advantages and disadvantages of using thick copper in the PCB stackups.
One advantages is obvious that thick copper layers can carry and is rated for higher current for the same trace width. For example, 70 um (2 oz) can carry more current then 35 um (1 oz) and 18 um (1//2 oz) for a give trace width.
How it goes with heat dissipation ? Consider a hot component on the PCB. When the objective is to spread the heat on copper layer then which copper is better, thick copper or thin copper ? I guess thick is better the same way as in case of heat sink. The bigger heat sink can absorb or disperse more heat then smaller heat sink. Is that true that thicker copper layer can also disperse more heat then thinner copper ?
What are the disadvantages of using thick copper layers ?
Thick copper helps in that it lowers overall resistance. The benefit is greatest when using DC voltages. When you add the AC component to a signal, the signals start to travel towards the surface of the copper which is called skin effect. As far as heat dissipation…it still is related to copper resistance. Surface area is almost identical for differing copper weights so heat dissipation is not different due to surface area. More copper thickness has less resistance will help minimize heat generation due to resistance of the copper.
Disadvantages: higher fab cost and trace/space minimums are higher for higher copper weights (think etch and plating requirements increase as the copper thickness increases). That means that if you need fine pitch devices, that tends to limit heavy copper on that layer unless the fab shop process supports multiple copper thicknesses on the same layer (think zones of heavy copper and zones of thinner copper for fine pitch components). More etch and plating time also tends to deform the object shapes which make up the layer. This is not usually a big deal but it does become more pronounced as the copper becomes thicker. Copper edges tend to become more trapezoidal.
if you double the copper thickness, from 1/2 oz to 1oz, then you also double the heat flow, by Fourier`s Law of heat conduction Rate of heat flow - Wikipedia , so if you increase from 1/2 oz to 2oz you will have 4 times more heat flow and heat spread into a solid PCB ground plane. With HDI of say 1+n+1 or up to 3+n+3 you can simply put a few solid 2oz GND plane in the middle to improve heat spreading. at 2oz you need to have at least 7 mil clearance to prevent under etching. I would not use anything above 2oz because it is non standard and very difficult to etch. Most standard PCB capability stables assume 1/2 oz copper, so 3 mil line / 3 mil space minimum on inner layers assumes only 1/2 oz. As you increase the copper by 1 mil, you increase the clearance by 1mil. So 3/3 at 1/2 oz becomes 4/4 on 1oz and 6/6 on 2oz etc.
I am using this four layer stack up. Kindly have a look in the attached picture and let me know if that make sense and is manufacturable.
In the four layer board, the copper on top and bottom are 2 oz (70 um). The inner layers are 1 oz (35 um).
The core is thick and is 38 mil. The total thickness is 60.1 mil.
The dielectric thickness between the top and inner layer 1 is 6 mil. The same is true for the dielectric thickness between the inner layer 2 and the bottom.
The Stackup is possible, if the design requires 2Oz on outer layers and 1 Oz on inner layers it can be done.
Some more things regarding the stackup.
Er of 4.7 for a FR4 material is a bit too high. you will see it within 3.2 - 4.2 for a FR4 material depending on the Material taken and the Prepreg/Core construction. 3.8 or 3.6 can be typical value.
All PCB Material manufacturer might not have the 38 Mil Core and the thickness may vary slightly. same goes for the 6 Mil Dielectric, in the final build it might be slightly different.
But close by thickness can be achieved.
The biggest disadvantages of thick copper are mostly sourcing related (i.e. cost and availability) and weight related (heavier finished product). Your thermal characteristics should be better, and thicker copper becomes more resistant to CTE concerns.
Thick copper PCBs offer several advantages, but they also present challenges. Manufacturing heavy copper boards is more complex and expensive due to specialized etching and plating processes. The additional copper increases the weight of the PCB, which can be a drawback in weight-sensitive applications such as aerospace or portable electronics. Moreover, thicker copper layers are more susceptible to thermal expansion and contraction, potentially leading to warping or cracking over time. The increased thickness may also limit the number of PCB layers, restricting design complexity, while reducing flexibility, which could be an issue in applications that require bendability. Additionally, sourcing heavy copper PCBs can be difficult, as not all manufacturers have the necessary capabilities, and the specialized processes involved can lead to longer production times.
There are some good points already mentioned. Here are some additional points to consider:
Thicker copper requires longer etching times, which can lead to side etching and result in a “foot” shape with a smaller width on top than on the bottom.
Multiple high resin content prepreg layers are needed to fill the etched spaces, which can lead to several issues such as inadequate prepreg can cause voids, while excessive prepreg can lead to thickness and dielectric issues. High resin flow can cause inner layer shifts and mis-registration. Resin-rich areas may develop cracks due to lack of reinforcement and higher CTE, leading to reliability issues at higher temperatures.
Drilling through thick copper requires parameters similar to drilling a thick copper plate, leading to increased drill bit wear and careful debris removal.
Applying sufficient solder mask to cover thick copper patterns is challenging and often requires multiple printings, which can still result in voiding and undercut issues.
For very thick copper (10 ounces or higher), applying resin to trace gaps is necessary to prevent excessive resin filling and voiding risks.
Large copper planes, if not properly grounded, can act as antennas and lead to significant EMI problems. This is particularly the case with poorly grounded, thin, and elongated copper traces on the outer layers. Furthermore, connecting copper planes to the main ground often requires more vias, which can limit routing space and design flexibility.
When copper is connected directly to component pins, it can dissipate heat too quickly during soldering, making rework or desoldering much more difficult. This can be an issue during repairs or modifications.
yes this is very easy to manufacture, you get into trouble when your dielectric (core or pre-preg) is less than 3.5 mils = 0.0035 inch thick. With only 4 layers you may have electrical problems, going to 6 layers and adding more GND planes will improve electrical performance.
in material datasheet, you have CTE xy and CTE z axis, for maximum via hole reliability you want your CTE z to be as close to copper as possible, ie: 17 ppm / deg C. so if you have lots of thick copper, on average the CTE z is getting closer to 17. The CTE z of most dielectric is around 40 ppm / deg C up to Tg of 180 C, above Tg it goes even higher 1% etc. That means during SMT oven reflow, when your board is in the oven to melt the solder, the PCB expands in Z axis, this puts force on the vias, pulling them apart, and possibly causing cracks. When the board cools down, the via may make contact again, but it will be intermittent and fail in vibration or thermal cycling later on. If your application is low power (less than 20 watts) and low speed ( less than 100 MHz) I would simply use 1 oz for power and ground planes, and 1/2 oz for signals. So in your case, your inner core of 38 mils will be a 1oz over 1 oz core, and your top layer 1 and bottom layer 4 will be 1/2 oz foil lamination, plated up by 1.5 mils as the thru via walls are formed, Hope this helps.
