I continue to be surprised by the number of designers who have yet to understand the importance of a ground plane. Think back to your basic electromagnetics classes, and you'll see why a large ground plane is important in multi-layer planar structures like PCBs. The ground plane acts as a form of shielding, confining electric fields in certain regions of the PCB stack-up, and it is simply convenient for routing and placing ground connections on components.
If you're one of the many designers who understand the importance and often the necessity of a ground plane, your PCB design software makes it very easy to create planes in a layer stack-up. This article will show how it works, as well as how to set this up in Altium Designer.
All commercial PCB design software defines two types of layers in a PCB stack-up: signal layers and plane layers. The distinction actually has nothing to do with how the layers are traditionally used, and in fact, a signal layer can be used to define a ground plane. The distinction arises in manufacturing outputs in terms of how photoplots of signal and plane layers are displayed in CAM software.
The distinction is clearly seen in Gerber exports from a PCB layout file, as shown below.
Image signal layer and plane layer from Gerbers
Now back to the original question: how do you make a ground plane in your PCB stack-up?
A plane layer in a PCB stack-up is intended to be completely filled with copper, with the only absence being removal around the board edge and vias passing through the plane. The signal layer could also have complete copper fill, which basically makes it a plane layer, but it will look like a regular signal layer with a positive display in a Gerber output. This leads to two ways to define a plane layer:
Both options allow you to design multiple large rails into the same layer, or to use the entire layer as a single plane. We'll look at all the options below.
In Altium Designer, you can assign signal or plane layers in the Layer Stack Manager. The first thing to do when creating an internal plane is to add a design layer specifically for the plane. In the picture below, you can see that two layers have been added as internal planes in the Layer Stack Manager, which is found in the “Design” pulldown menu. They have been named “GND” and “PWR” respectively and occupy layers 2 and 3. Note that planes can also be used on outer layers, such as the stackup I discuss in this article.
Creating Internal Plane layers using Altium Designer’s Layer Stack Manager
Once you have set everything up, you are ready to assign a net name to the plane layer. Open the PCB Editor, and navigate to the internal plane layer. Double-click the colored region and a net assignment dialog will appear. Select the relevant net from the dropdown menu, and you are finished. Any vias or through-hole pins that also connect to this net will automatically connect to the internal plane.
An example of via connections to a net can be found in the left panel of the picture below. Note that the pins and vias do not have any visible connections yet to the plane. This is because the net name has not been assigned. You can also see on the left side of the connection menu that pops up when you double-click on that layer within the layout session. This same menu is used to name both single and split planes.
In the drop-down menu on the left side of the picture above we have selected “GND” as the net name that we want for this internal plane. This way it will match the GND net of the pins that you can see in the picture.
Once a net name has been selected, vias and through-holes are directly connected to the plane. If the relief connect rule is enabled in the PcbDoc, the pins will have thermal pad connections applied automatically as shown in the right side of the picture. Remember that this is a negative plane, so the metal of the thermal spokes and the plane area are represented by the darker color.
If you designate a signal layer in the PCB stack-up, then you can turn it into a plane by drawing in a copper pour with the drawing tools in your PCB design software. Draw out the plane manually in the copper layer with the drawing tools and assign that region of copper to the appropriate net.
Now we’ll create a positive plane or a “Polygon Pour”. On the left side of the picture below you can see that this signal layer does not have any metal on it yet. To create the polygon pour you can either use the pulldown menu command “Place > Polygon Pour”, or you can click on the polygon icon in the active bar at the top of the session window.
While in the polygon pour mode, you will click where you want to place a vertex of the plane that you are creating. If you make a mistake simply use your backspace key to remove the last placed vertex. Once you are finished, right-click in the workspace to exit the polygon pour mode. On the right side of the picture above, you will see the plane that you created assumes the color of the layer that you are working on. You will note though that there aren’t any connections yet to the pins and vias in this plane layer.
Creating a Polygon Pour in Altium Designer
Once the polygon is placed in the PCB layout, it needs to be assigned to a net; select the polygon you just created and go to the Properties panel. As you can see in the picture below, you will have a list of nets that can be assigned to the polygon. Again, we have selected the GND net.
Assigning the net name to the polygon pour
There are other options and values that you can set up in this panel for your polygon. As you can see above, there are options for copper islands, arcs, and nets as well as setting your plane up as a solid pour or hatched.
While the polygon is still selected you will next need to re-pour the plane in order to force the connections between the polygon and any nearby objects assigned to the same net; this is required any time you modify a polygon. To do this, right-click on the selected polygon in the PCB Editor window and select Polygon Actions -> Repour Selected. You can also use the T + G + A hotkey to repour all polygons.
Re-pouring the polygon pour to connect the net
When repouring a polygon over any vias, SMD pads, or through-hole pads, the design rules engine will enforce a connection style between the polygon and the pad. In the image below you can see that the polygon (shown in red) is now connected directly to the vias and through-hole pad with a thermal relief. Once the polygon is repoured on this layer, the thermal relief spoke connection will be visible.
A completed polygon pour ground plane in Altium Designer
If you determine you do not need an entire layer filled with copper to form a plane, you can split the layer into multiple rails by drawing different polygons. While not recommended for ground, it is very common with power rails. One practice that is common in designs that require digital power rails or high-current DC rails is to use large sections of copper pour and place them on the same layer. This layer, for example, would be your power layer, and all the rails would have to share space on this layer. This is a common approach in 6-layer stack-ups or in less-dense 4-layer stack-ups. Follow the steps above to implement this type of design.
An alternative to drawing multiple polygons onto a signal layer is to draw splits in a plane layer to form multiple rails. While you should be careful of the signal integrity and power integrity consequences of doing this, skilled designers who split planes into different rails can achieve a very convenient way to route power into groups of components or circuits. Doing this on a plane layer involves manually drawing out the split regions on the plane layer, then assigning a net name to each rail formed after the split.
In Altium Designer, you can place any configuration of lines, arcs, tracks, and fills in an internal plane to define a split and create multiple rails. The easiest way to draw split plane is to use the Place -> Line command and manually draw out the boundary of the new rail in the plane layer. Once this is drawn, the new rail can be assigned to a net using the same process shown above for a uniform plane. Once this is complete, the split plane regions can be selected individually, such as is shown in the image below.