Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Why this kind of power planes/copper pour in PCB design

Status
Not open for further replies.

sac1991

Member level 2
Joined
Jan 21, 2017
Messages
52
Helped
7
Reputation
14
Reaction score
7
Trophy points
8
Activity points
409
pcb.jpeg

Today I found a damaged power supply PCB. Why are those copper pours have solder mask removed in that particular manner.

I could also observe a white layer(may be silk screen layer) on top of many tracks(at the edges on figure). Can anyone explain why this kind of pcb design was done.
 

These ribs/bumps on the power planes are usually done to increase:
- conductivity of copperplane (less powerdissipation, solder is cheaper than choosing higher Cu layer thickness)
- thermal capacitance & surface of copperplane (better cooling of components)

For me, the "white layer" looks like a kind of cheap shielding for sensitive long traces.
We used such a design in Low-cost-products. The paint usually contains some graphite/metallic particles. This is cheaper/faster than optimizing the layout or adding additional components for filtering.
 
In spite of the probable reasons justifying such a style, I would intuitively say that the performance of a dashed track finishing would be intermediate if compared to a fully filled one, or another totally covered therefore not sure of the usefulness on this case. As for temperature performance, while actually increasing conductivity, on the other hand the solder is intrinsically less electrically conductive than copper, and so would be in some way a thermal barrier to the track just below. Another curious aspect in the above layout is that the direction of the stripes is orthogonal to the largest dimension of the plate, ie, the supposed electric path is not aligned with the addition of solder at copper surface.
 
These ribs/bumps on the power planes are usually done to increase:
- conductivity of copperplane (less powerdissipation, solder is cheaper than choosing higher Cu layer thickness)
- thermal capacitance & surface of copperplane (better cooling of components)

For me, the "white layer" looks like a kind of cheap shielding for sensitive long traces.
We used such a design in Low-cost-products. The paint usually contains some graphite/metallic particles. This is cheaper/faster than optimizing the layout or adding additional components for filtering.

Never heard of that. What's the name of the white stuff?

And why remove the mask in stripes rather than remove it entirely?

Like andre said, I also don't understand the direction of the stripes.
 

For better conductivity entire mask could be removed and solder can be placed. But the direction and shape of the mask makes me curios, there might be some good technical reason behind it.
 

Hi,

The conductivity of solder is much lower than copper, thus you need relatively thick and full area solder plating to get a considerable decrease in overall resistance.

I don't think it's a useful and reliable method to increase conductivity.

What reliable solder thickness one can expect?
And how much in % will this increase overall conductivity?

Klaus
 

Both solutions seen in the OP picture, solder mesh on trace and Silkscreen cover, are cheap and weak solutions for technical problems. Often seen in cheap powersupplies, to save money. And sometimes implementation is even done wrong.

Solder mesh:
Weak workaround for using thicker copper core/plating. For wave soldering, you cannot remove the SR completely, as this will give undefined solder thickness & some drops/tears on the trace. It will also increase risk of bending if both layers are not weighted equally. Therefore this is done as a mesh.
In the OP picture, this is even done wrong, as the mesh should follow the current flow. They mainly only have the outer surrounding shape, the inner crossings are 90° to current flow, therefore somehow ineffective.

Silkscreen cover:
Besides standard silkscreen, there are a lot of different materials with special properties available. See https://www.dupont.com/products-and...rials/brands/screen-printed-inks-for-pcb.html
In the OP picture, it could be also normal silkscreen, covering some traces, to increase insulation resistance, if the pcb is too close to housing.

I fully agree to all of you that both solutions are not "best practice" for proper pcb design.
I'm just waiting when we will see PCBs with SCO / STH on CEM1 again :laugh:
 
Completely removing the soldermask and flooding it with solder would give practically no control over the final distribution of the solder after reflow, which could lead to various issues such as local stress points during ramp down.

The direction of the tracks was likely chosen to be along the minor dimension of the PCB in order to improve flexibility.
 

The direction of the tracks was likely chosen to be along the minor dimension of the PCB in order to improve flexibility.

Perhaps, but isn't the mechanical flexion on the PCB a feature to be avoided ?
 

Perhaps, but isn't the mechanical flexion on the PCB a feature to be avoided ?
I meant that it would be able to tolerate more flexing without cracks in the solder blobs, or delamination of the copper pours.
 
Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top