1
\$\begingroup\$

In cases when a 4-layer board is space limited, and there's a lot signal traces in the whole board, "power plane layers" is not very usefull to distribute power rails. Because it is used only to draw solid regions in a negative format. Therefore it is very hard to place some signal traces along the power plane.

I've been thinking, what's the difference to use a "signal-layer" instead of "power plane layer" which offer the capability of non negative format? You can also draw as solid region as you want but you are still able to put a few traces that they are difficult to stand on the external layers due to complexity.

\$\endgroup\$
  • \$\begingroup\$ In the olden days of uploading gerber files over 14.4 kbaud modems, a negative plane layer transmitted a lot quicker than a polygon pour. Probably also took a lot less time on the photoplotter. Nowadays neither of these considerations has much weight. \$\endgroup\$ – The Photon May 18 '17 at 19:32
4
\$\begingroup\$

While there's a lot of good answers already, I felt I should add some distinctions to "when should you use which, generally" and "when should you move from the ideal, because Altium."

Normally Power Plane layers offer a nice and well defined inherent separation of rules and restrictions. As came up before, it allows programs to assume solid copper in complex analysis. It's also more space efficient when defining large copper areas. In some cases manufacturers can use more reliable negative-defined processes, though these are somewhat outdated and inverting a plot is negligible work anyway.
When you send a plane definition layer the entire supply chain assumes high levels of copper coverage, which is key in getting impedance control right at the least amount of cost.

However...

There are programs, amongst which Altium, in which you cannot always set vital parameters on your plane layers, that you can set on signal layers and/or for copper pours.

For one example, Altium removes via pads by default on power plane layers, without any option to force it to place them anyway. This is all well and good if you're designing a power-supply or an audio amplifier (a manufacturer that needs them for processing stability will just add a 0.05mm ring anyway). But if you're designing signalling for high MHz and GHz ranges you may actually want full control over all bits of your signal path, including the way vias couple on plane layers. Similarly you cannot easily force the program to pull back a power plane from cut-outs or edges by a configurable distance.

This leads me to the advice, rather than just condoning, to always consider signal layers instead of plane layers in Altium specifically (not as a general argument!), unless you need trace impedance analysis or other plane-tied features.
But if you're working professionally enough to want full analysis of done designs, you are likely to be in a domain of frequencies that someone should arrange a license for a tool like ANSYS or Microwave Studio, which works fine for signal layers as reference plane.

\$\endgroup\$
1
\$\begingroup\$

The plane feature is good if you have arrangements that are best drawn in negative. Splits are handled nicely, for example, and highlight when the net is selected.

If you must run signal traces you might find it easier to do polygon pours on the layer in question for the power regions.

\$\endgroup\$
1
\$\begingroup\$

The way I route my power planes is using signal-layer and draw power planes with polygon pours. If you want to add a section for signals or put two or more power planes in the same layer, its as simple as drawing another pour.

The only layer that I have as a power plane layer is a ground layer because this one is going to be solid and will almost never have traces running through it.

I've been thinking, what's the difference to use a "signal-layer" instead of "power plane layer" which offer the capability of non negative format?

The difference is if the plane is going to be mostly solid on that layer, then use a power plane layer otherwise use a signal layer.

\$\endgroup\$
  • \$\begingroup\$ These are all good answers. I would like to add another quirk unique to Altium: unless things have changed in recent versions, plane layers are used for microstrip impedance calculations when doing impedance-driven routing, whereas polygons on signal layers aren't. So, you may have to do your impedance width calculation manually if you use a polygon on a signal layer as a reference plane. \$\endgroup\$ – Peter May 18 '17 at 22:25
1
\$\begingroup\$

While I don't know the complete list, here's one example. Altium can calculate trace impedance only when the trace is next to a plane.

At the same time, if you don't have to use Altium features that rely on designated plane layers, then your approach is just fine. I've done this used it with OrCAD: designated inner layers as routing layers, then used copper pours for ground and power planes.

related
Can I lay traces on internal layers of 4 layer PCB?

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.