Outer vs. Inner copper thickness

[metebalci]

I was looking at the gerber files of an ST Nucleo board and then checked also jlcpcb (https://jlcpcb.com/help/article/364-multi-layer-pcb-standard-laminated-structures) and it writes the outer and inner copper thickness is different even if both are 1oz. What is the reason for this, impedance control or different processes during the manufacturing ?

[thm_w]

1oz is the thickness, its not going to vary unless specified as another number. Usually inner would be 0.5oz.
Can you paste here exactly what you read?

You can see on their site: https://jlcpcb.com/quote/pcbOrderFaq/Copper%20Weight

[exe]

What is the reason for this

Cutting costs Other pcb manufacturers don't have that, but they are also more expensive .

[tszaboo]

HASL for example. Pure copper is very easy to corrode by touching it or even by air itself over time, so they plate it. After plating it's a different thickness.

[metebalci]

1oz is the thickness, its not going to vary unless specified as another number. Usually inner would be 0.5oz.
Can you paste here exactly what you read?

You can see on their site: https://jlcpcb.com/quote/pcbOrderFaq/Copper%20Weight

This is what is ordered but it seems like the final thickness is different. I understand the final could be different but I wonder why inner and outer is different from each.

For jlcpcb, from https://jlcpcb.com/help/article/364-multi-layer-pcb-standard-laminated-structures, which says outer is 1.6mil, inner is 1.2mil, both 1oz.



This is from the gerber files I mentioned of NUCLEO-G474RE board. Here the inner layers are 35um but outer is 42um.

[metebalci]

HASL for example. Pure copper is very easy to corrode by touching it or even by air itself over time, so they plate it. After plating it's a different thickness.

I saw things about processing allowance (IPC-4562 if I am not wrong), so I guess some changes are supposed to happen but is the surface finish included in the final copper thickness ? I thought HASL is quite thick, comparable to trace thickness not a few micrometers.

[metebalci]

What is the reason for this

Cutting costs Other pcb manufacturers don't have that, but they are also more expensive .

I forgot where I saw but I think you are right about the final thickness if the aim is 35um, they can start with more copper. However, it does not answer why outer layer has more copper. I mean, assuming both outer and inner uses 1oz, if the same amount of copper is put on the layers, and then etched, they should be same.

I found the page: https://www.eurocircuits.com/tolerances-on-copper-thickness/ . I guess due to cleaning or plating or something like that there can be a difference.

[wraper]

You cannot do outer and inner layers of the same thickness unless using copper foils of different thickness to reach the same final thickness. Unless pcb has blind or burred vias, inner layers are not electroplated unlike outer layers that are electroplated together with vias.

[tszaboo]

You cannot do outer and inner layers of the same thickness unless using copper foils of different thickness to reach the same final thickness. Unless pcb has blind or burred vias, inner layers are not electroplated unlike outer layers that are electroplated together with vias.

Via plating... I really should't write anything technical at midnight 

[mikeselectricstuff]

The initial plating process to create vias also plates the outer sufraces, increasing thickness.

[wraper]

Also thick copper on inner layers is problematic as it causes problems with PCB flatness and layer bonding.

[exe]

why outer layer has more copper.

I'd say current capacity. For power application 1oz is often not enough, let alone 0.5oz.

[metebalci]

Thanks all, then it is due to via plating.

This made me wonder another thing, if lets say the starting copper foil is 35um, and it is decreased to 30um during processing for some reason, but with plating it is increased to 40um. Doesnt it mean the copper at a via has a thickness of 10um ? And it is OK because the surface area of via is more than the trace, basically creating a thin but wider trace ?

[thm_w]

Thanks all, then it is due to via plating.

This made me wonder another thing, if lets say the starting copper foil is 35um, and it is decreased to 30um during processing for some reason, but with plating it is increased to 40um. Doesnt it mean the copper at a via has a thickness of 10um ? And it is OK because the surface area of via is more than the trace, basically creating a thin but wider trace ?

They start at 0.5oz (18um) and plate to 1oz (35um) total.
So the via would be 18um thickness, roughly.

I don't think there is much loss during processing.