Hi guys, I just finished designing a PCB that should conduct up to 17A. I know the amperage is pretty high, but the PCB is designed solely for an electrical interface between transportation modules. Shouldn’t I edit the thickness of the copper layer, so that it can withstand the high amperage? How thick should the layers be? Thanks in advance?
Normally it is a parameter that you fill in on a web form when ordering the PCB’s.
I am not aware of a setting in KiCad related to this.
In 5.99 you can set copper thickness in the board stackup (and get it included in the job file) but your board house will ask about the discrepancy at best. Or they’ll just produce whatever you actually ordered (thicker copper is of course more expensive).
That aside, thicker copper will negatively affect constraints like copper-to-copper clearance, minimum trace width and such. Are you sure you’re actually
I might should have mentioned that the PCB does not include any traces: it conducts currents current through the surface area from one side to the other. You can see it in the attached photo. I am just worried about the thickness of the layer (as it contributes to the conductivity and efficiency of the interface). Would the manufacturer consider the amperage? or can one edit that on KiCad.
I also believe that my layout is as good as complete, the layer thickness is the last issue. Do you want to refer to something specific?
Nope. The manufacturer only cares for what copper thickness you tell them. They don’t care what your end use is.
That said, you may be able to get some advice from their technical support team with the proper questions. Just be sure to purchase from them to pay them for the technical support time. (Bonus of asking the manufacturer directly is they will be able to also tell you how they expect any potential thicker copper requirements to be communicated to them so they can bill you appropriately and provide a product that you are happy with.)
Can’t I adjust the thickness on KiCad? Or should I provide it in the order description/notice (assuming that’s the only way to do it)? If the latter is right how can I calculate the thickness depending on the amperage?
For most manufacturers you just give them a note telling the thickness or select it in a web order interface.
There’s no simple way to calculate the thickness. The temperature rises when the current rises, but how much the board actually heats depends on the external conditions. Chassis, air temperature and air flow etc. The produced heat must of course be conducted or radiated away lest the board burn.
KiCad has some kind of calculator.
One way to find out is to order some prototypes and test them with high current, then do some educated guess about whether the whole product can handle the heat under the conditions it will be used.
We hardly can help any more than this unless you give much more details about the product and how it will be used.
It can be a bit of Fun and, certainly frustrating (to get a grasp of it and results that make sense) but, a FEA (Finite Element Analysis) could be a self-vote of confidence.
If you had posted your file, I would have used it but I threw something at an FEA, just go give you the idea.
Results always depend on Good Input and, I have zero info about what materials you’ll have (FR4, ABS, Phenolic…etc). The copper is straight-forward enough… Geometry is important…
Anyway the point is that you can jimmy-up an analysis (look for my posts on Thermal Analysis).
Images below show a Semi-Circle of geom that has nothing similar to yours (about 100m Diameter, 36um of copper, ). FR4 (1.65mm) is sandwiched between Copper on Top/Bottom. Shows Displacement magnitude of 7.xx um).
Also, an image of a Heating Element embedded into FR4(just for another example) Temp&Displacement Magnitude
You can Google copper thickness for PCB and come up with the ‘Standard’ for it (it will list them in a usable way. I’ve posted them so, won’t repeat my effort.
Ahh… The football game started, gotta go!
The pcb will have a copper thickness that is generally either 1 or 2 ounce per square foot. 1 oz = 0.0014 inches thick.
Take a look at the tool Hermit referenced.
You will see that as current increases, so does temperature. You have to decide how much temp rise you can stand.
There is no direct equation of current to copper thickness.
You should always be mindful of traces that need to carry current but how you capture this information is down to where you are getting your card fabricated.
Fundamentally it is about cross sectional area: wider tracks = thinner copper for the same capability.
SaturnPCB toolsuite has a fantastic section on current capability (note: the calculator that comes with KiCad uses IPC-2221A, which is incorrect and you need a calculator that aligns with IPC-2152
So take 17A and assuming you want to limit self-heating to say … 5C
1oz copper -> 60mm wide track
2oz copper -> 30mm wide track
3oz copper -> 20mm wide track.
With a number of combinations of parallel tracking in between.
HOWEVER, this doesn’t actually answer your question as to how do you set the thickness. Typically you don’t in PCB tools, well not for information like this.
KiCad-6 does come with a stackup editor and this will give you an idea of overall thickness but this does not influence how wide a track should be, likewise this does not instruct the board fabricator as to the thickness.
So during your design you will need to settle on the thickness of the copper to manage your trackwidth while also considering etching limitation (3oz is ~ 0.25mm track and clearance, rules out SSOP devices). Once you have this settled on and you have a design with an acceptable amount of compromise its about how to request a 3oz PCB.
If you are using the online proto sites they pretty much come with standard weight and stackups so your early design needs to consider this - if a boardhouse only does 1oz then you will need wider or many traces etc.
Now if you are paying the extra for a custom stack up where you can have different weights on different layers (assuming you produce a balanced stackup to mitigate warping), its then down to communicating the information to the fabricator. I typically do two things
- add a stack of infomation to the Eco1.User layer
- Provide a fabrication pack
This is a 100A card I am presently working on
NOTE: that is IPC-2221A and this has been superceeded by IPC-2152, there are only a few tools that have been updated (ninja and saturn are two)
That is IPC-2221a and is not suitable.
IPC-2152 is based upon empirical curves and the calculators that do exist work based upon a best-fit and caveats upto 25A
Current itself isn’t so important, but the power is, which produces heat. In the end it’s about how much power the system can stand. If you add cooling with liquid nitrogen you can have smaller copper thickness and save some money
Exactly, the resultant temprise is what is key, the manifestation of power being dissipated.
A nearby plane can help act as a heatsink to keep the temperature rise to a minimum. The last thing you want is a PCB that starts to delaminate due to thermal expansion OR glassification of FR4
The key is time. How long is that current (ie power dissipation) occurring for? if it is for a second? well the thermal mass will help realise smaller cross-sectional area. Continuous? well that’s a different story. Fault current? are they other means to interrupt the power
I think you miss my point, which is to point out that Thickness and Current are related.
Wasn’t saying that’s the only consideration.
Commonsense should inform geek that Power is Power (and all that it relates to).
If you bury a Powerline in soil versus the same Powerline/Load, strung across two towers, naturally the Heating is going to be different.
That is to say, on a Hot day, sitting on my Harley with heads at 340F doesn’t seem too hot to my crotch at 70mph but, sitting at a Red-Light, waiting, I want to stand up.
I don’t think anyone missed any point. Nobody criticized your post. There just are different things to say and different ways to say them.
Just to stress this again (and yes I would say this is the criticism…)
Please do not advocate IPC-2221 calculators.
Replacing the conductor sizing charts that currently exist in IPC-2221 (which were based on data sets more than 50 years old), the new IPC-2152 standard provides guidance on how thermal conductivity, vias, power dissipation, printed board material and thickness, and most importantly, the presence of copper planes all factor into the relationship between current, conductor size, and temperature.
There was no equation. The IPC developed charts based upon empirical testing. People derived equations based upon the tables which are subjectively “good enough”…
The IPC updated this information based upon more updated testing.
As is all too often the case, the OP asked what I’m sure he thought was a simple question and the respondents gave a bit of useful information. This was followed by quibbling over standards and incompleteness of comments. That should have been a new thread, as the OP didn’t likely benefit.
I tried to give a brief comment that there was no simple lookup table of current vs. copper thickness, which I believe addressed the OP’s question.
Focus ladies and gentlemen. FOCUS