Defining the Layer Stackup

After project synchronization, we are ready to start the development of the printed circuit board. One of the first stages is defining a PCB Stackup. At this stage, we will define the internal design of the PCB that starts with deciding how many metal layers are needed, the PCB thickness, via types, and impedance profiles. During this stage, we need to ask ourselves "will we be able to form an impedance structure with this set of layers?”. If we are able to check with the manufacturer about dielectrics and metallic materials, information about impedance requirements can be found in application design guidelines. With Altium Designer, you don't have to spend a lot of time calculating the impedance profiles and selecting the width and gaps of the conductors and planes. You only need to specify the target impedance; the Layer Stack Manager will automatically select these parameters for you. After that, when working with the rules, you can select the necessary profile for the group of circuits in a few mouse clicks. Let's start forming a PCB layer set!

Stackup Configuration

We need to form a layer set for our PCB. Open Kame_FMU.PcbDoc, press O then select Layer Stack Manager. The Layer Stack Manager editor will open in the design space.

Tip: You can also run the Layer Stack Manager by selecting Design > Layer Stack Manager from the main menus.

**Fig. 1** - Launching the Layer Stack Manager

**Fig. 2** - The Layer Stack Manager editor

Currently, the PCB stackup contains two metal layers (Top and Bottom) and a default dielectric layer (FR-4) between them. Our drone’s PCB should contain at least six layers: four signal layers and two plane layers with a total thickness of 1.6 mm. Enable the Stack Symmetry option in the Properties panel. When this option is activated, the Layer Stack Manager will automatically align the top and bottom halves of the stackup. Right-click over the Top Layer then select Insert layer below > Plane.

Inserting a Plane layer below the Top Layer — **Fig. 3** - Inserting a **Plane** layer below the **Top Layer**

Four layers were added to the PCB stackup (two metal plane layers and two prepreg layers). Using the Stack Symmetry option has automatically balanced the layer set.

Layer Stack Manager automatically added a layer to the bottom half to provide stack symmetry. — **Fig. 4** - Layer Stack Manager automatically added a layer to the bottom half to provide stack symmetry

The next step is to add two more signal layers in our stackup. Right-click over Layer 2 then select Insert layer above > Signal to add a signal layer above Layer 2. Since the Stack Symmetry option was enabled, we now have a full 6-layer stackup.

**Fig. 5** - Created PCB Stackup: four signal and two plane layers

This set of layers still needs additional configuration. We need to define the core dielectric layers as well as the correct weight for the metal layers. Double-click on a value in the Weight column for the Top Layer. Use the drop-down menu to select 1/2oz. As you can see, the weight value for Bottom Layer has been changed automatically. Set the Weight to 1/2oz for all metal layers.

**Fig. 6** - PCB stackup with updated weights for all metal layers

The next step is to define the core dielectric layers. Double-click on Dielectric in the Type column for Dielectric 4. Use the drop-down to select Core as the type. Set the Thickness for this layer to 0.51mm.

**Fig. 7** - Core layers have been configured for the PCB stackup

There are three prepreg layers left to configure. All we need to do for these layers is set the thickness to 0.15mm. The total board thickness should be 1.597mm.

All materials of PCB stackup are configured — **Fig. 8** - All materials of the PCB stackup are configured

To aid readability, we will specify names for the internal metal layers. To rename a layer, double-click in the Name column then enter a new name and click Enter to save the layer name. Rename layers as follows:
Layer 2 -> GND2
Layer 3 -> L3
Layer 4 -> L4
Layer 5 -> GND5

Your stackup should now resemble the below figure.

Finished PCB Stackup — **Fig. 9** - The completed PCB Stackup

We are now done configuring the layers and materials. Save your Stackup document.

Impedance Profiles

The design of our printed circuit board has a USB interface that requires the placement of differential transmission lines with a 90 Ohm impedance. The Layer Stack Manager allows you to calculate the impedance of the transmission lines as quickly as possible by specifying the target impedance. When you specify the correct impedance value, Altium Designer will do the rest. After creating the impedance profile, it will become available in the rules editor and you can apply it to required tracks with mouse clicks. Let’s set the impedance profile for the differential pair.

Click on the Impedance tab at the bottom of the Layer Stack Manager to run the Impedance Profile Manager.

Fig. 10 - Add Impedance Profile

Click the Add Impedance Profile button. A standard impedance profile will appear, which needs to be configured.

Fig. 11 - Impedance Profile is added

Open the Properties panel. In the Impedance Profile region, define Type as Differential. Set the Target Impedance to 90 and specify the Target Tolerance as 5%. Notice that all values for Width and Trace Gap have been updated automatically in the Layer Stack Manager for all signal layers to match the specified target impedance.

Fig. 12 - Impedance Profile configuration

Tip: You also can add a short description of your impedance profile in the Description field of the Properties panel.

Save the Stackup document. That’s it! Impedance profiles have been automatically transferred to the PCB. Later, we will configure the width and gap rules for the differential pair with this profile. Close the Layer Stack Manager editor and open the Kame_FMU.PcbDoc to continue working with the PCB.

Good job! Article is now completed!

Mark as Completed Completed

article Previous

article Next

CAPTCHA

Was this article useful?
Yes No

Thank you Glad to hear it