Getting Your Layer Stack Right the First Time: A Guide for Every Engineer
Are you taking enough time to plan your layer stackup? If you’re like most designers, then you’re probably just figuring out how many layers you need and leaving the rest up to your manufacturer. But consider this, an improperly planned layer stackup can lead to nasty issues like excess heat, crosstalk, and impedance mismatching. So if one of these problems might be plaguing your design project, then this is one step in your workflow that is better left in your domain of expertise. Ready for a new perspective on managing your layer stackup? Let’s take a look at how to get your layer stack done right the first time, every time.
The Layer Stacks of Yesterday and Today
Gone are the days of PCBs just being single-layer boards with no vias, clock speeds of around 100 kHz, and basic through-hole components. These days, you’ll find PCBs with as many as 50 layers, with components on both sides of your board, and even some nestled in between layers. And those days of KHz signals speeds are now in the 28+ Gb/S range. Point being, as the technology in our PCBs advances, so does the importance of planning out a solid layer stackup before you ever begin your design.
The layer stackup might seem deceptively simple at first glance. After all, isn’t it just describing the basic construction on a PCB with its various layers? While the stuckup might be a simple visual cross-section of your PCB, what it manages to achieve for your design is vital. Did you know that it can:
- Help you to minimize radiation and prevent your circuit from being affected by external noise source?
- Help you to reduce crosstalk and impedance issues on your high-speed PCB layouts?
- Help you to balance Signal Integrity (SI) issues with the needs for low cost and efficient manufacturing methods?
And most important of all, did you know that a properly planned layer stack is one of the most valuable tools in your toolbox for enhancing the Electromagnetic Compatibility (EMC) of your design? So before you go off calculating impedances, or matching trace lengths to minimize electromagnetic interference (EMI) on your board, what you need to do is start with a properly planned layer stack.
Without a plan for what materials you intend to use, and in what order they’re arranged, you might find yourself dealing with symptoms like poor electrical performance, increased emissions, and even timing glitches. All of these and more can be solved when you make an effort to get your layer stack done right the first time.
What Kind of Layer Stack Do You Need?
The answer to that question ultimately depends on the specifics requirements of your design. These days manufactured PCBs are broken down into two general categories: single-layer and multilayer PCBs. But what’s in the details?
Single-layer PCBs are ideal for the most basic devices and include either one or two copper layers (Top and Bottom) for you to lay down components and traces on. While these boards won’t be a focus for this blog, it’s good to know that they still exist, and are usable until you hit a frequency range of 25MHz.
More layers afford you a lot more than more space to route. Once your frequency needs have climbed, you’ll start to live in the world of multilayer PCBs. These types of boards take advantage of multiple cores, which consist of a symmetrically balanced structure of alternating copper layers and insulating prepreg material. Check out the image below to get a visual on how this all comes together in an 8-layer PCB.
But why would you ever want to use a multilayer PCB in the first place? Here are a few solid reasons:
- It’s a well-known fact that a four-layer board will produce 15 dB less radiation than a two-layer board with all other variables being consistent.
- There’s also the huge benefit of designing in a multi-board environment that can contain dedicated planes for ground, signal, power, etc.
- Boards with multiple planes will also allow the routing of traces in either a microstrip or stripline configuration. These can help to carefully control impedance and emitted radiation better than a single-layer board even could.
When you opt for a multi-layer PCB, you’re also getting the benefits of multiple ground power planes, which can help to reduce impedance and ground noise in every design. Still not sure if you need a multi-layer PCB?
Use our general rule of thumb – if your frequency range is going to be above 10 – 15 MHz, then multi-player boards will be needed to get the job done.
Planning Your Stackup
When planning your layer stack, most designers just consider the amount of players they need, and little else. However, there are a lot more variables to consider when planning a robust set of layers, including:
- How many layers your design requires
- How much spacing you need between each layer
- How the layers are going to be structured and organized
- How many power/ground planes your design requires
When deciding how many layers your design requires, the details go even deeper with a new set of constraints to consider like:
- The number of signals that need to be routed
- The frequency of your signals
- The type of FCC emission requirements that your board has to meet, Class A or Class B.
- The type of enclosure your board will call home, whether that’s shielded or unshielded.
By considering not just one but all of these variables, you can go about determining how many layers your design will require. You can also use the table below to estimate the number of layers based on your board’s pin density:
|Pin Density (Pitch)||# of Signal Layers||# of Board Layers|
|0.6 – 1.0||2||4|
|0.4 – 0.6||4||6|
|0.3 – 0.4||6||8|
|0.2 – 0.3||8||12|
You can also use the equation below to figure out how many routing layers you’ll need:
Here, M is the number of routing layers you’ll need in total, which is determined by the number of netlists, N, multiplied by the average pitch, Pavg, divided by the board length and board height, lh.
Arranging Your Layers
Once you’ve determined how many layers your design requires, you can then go about organizing them in a logical structure. When doing this, you’ll want to consider both the distribution of your signal layers and also the distribution of your power/ground layers. With these considerations in mind, here are some general principles to follow when arranging your layers:
- A signal layer always needs to be arranged adjacent to a ground plane. This will give the return signal an efficient path of travel from source to sink.
- Your signal layer needs to be next to an internal power layer. This will provide shielding benefits from any emitted radiation.
- For high speed designs, designate a layer for these signals located between planes. These planes will act as a shield to minimize radiation.
- Always place a ground layer between two adjacent signal layers. Doing this will lessen the chance of crosstalk affecting your signal transmissions.
- Consider taking advantage of multiple ground planes if possible. This will lower the overall ground impedance of your board and reduce common-mode radiation.
One thing to keep in mind when doing this process is that designers will often have to make a compromise when deciding between close signal/plane coupling or close power plane/ground plane coupling. Under normal PCB manufacturing methods, there’s usually just not enough inter-plane capacitance between adjacent power and ground planes to provide ample decoupling below 500 MHz.
Because of this limitation, you’ll likely want to op for tight coupling between your signal and return plane. Coupling between a signal layer and its return plane produces way more advantages in proper signal timing and reduced emissions than what you lose by not closely coupling your power planes.
Layer Stack Templates
While your layer stack is uniquely yours, it can never hurt to follow an example template from your manufacturer. Listed below you’ll find layer stack examples to help guide your planning process for four, six, and eight-layer boards.
Four layer stackup
In this stack, we have high speed signals placed on the top layer with an efficient return path on Layer 2 (Ground Plane). The high speed signals on the bottom layer are referencing the power planes on Layer 3, and this will require placing stitching capacitors between the power plane and ground plane.
In this stack, it’s recommended to route your high speed signals on your top layer. That way the signals have a direct path to ground. But if your design calls for high speed signal routing on the bottom layer, you can simply swap Layers 2 and 3 to make that possible.
Six layer stackup
In this stack high speed signals routed on the top layer have a reference plane on Layer 2. Stitching capacitors will be needed on this layer to reference the power plane to the ground plane.
Unlike the four-layer stock, this one is designed to have high speed signals routed on the bottom layer as it has an immediate reference to ground in Layer 5. Layers 3-4 is where you’ll do all of your low speed signal routing, which has a reference plane on Layers 2 and 5.
Eight layer stackup
In this stack, the high speed signals on the top layer are referenced with the Layer 2 ground plane. You’ll also find Layer 3 using the same ground plane as its reference point. When using this stack and routing on Layer 3, you’ll definitely need some stitching capacitors between the power and ground planes.
You can also use Layer 6 when you need to route high speed signals with critical impedance control requirements. This layer will produce less EMI problems because it’s shielded by two ground planes.
Documenting Your Layer Stackup
Once you’ve defined and arranged your layer stackup, the last thing you’ll need to worry about is documentation for your fabricator. This is an important step, as one of the most common defects in the PCB fabrication process is the misordering of layers.
Aside from just generating Gerber files for each layer in your design, there are several strategies you can take to clearly document your stackup for manufacturing, including:
Adding a README file
While your PCB software will output unique files for each layer in your PCB, how those layers fit together in a complete layer stack is up to you to communicate. To do this, simply submit a README file that details the orders of your layers and their associated files names to your manufacturer like in the example shown below:
Numbering layers on your copper
Within your design tool, we also recommend placing a layer number directly on each copper layer. This is a clear visual indicator for your fabricator that it’s a layer number. When your PCB is viewed from its primary side profile, this numbering sequence will be shown for each layer on your board, making it easy to see layer numbers at a glance. To see this feature, you’ll want to add a solder mask relief of 100 mils around each layer number.
Adding stacking stripes on your copper
While numbering your layers is useful, it doesn’t fully communicate how your layer stack will be arranged in physical form. To address this concern, you can add what’s called a stacking stripe to the edge of each layer on your board.
To do this, locate the primary side of your board and add a 200 mils x 50 mils box that protrudes off the side on your first layer. Then repeat this process on each subsequent layer, shifting the stripe over 200-250 mils for each layer.
By the time you’re done, you’ll have a set of stacking stripes that step down nicely and show how each layer is arranged in order. This will help to provide a quick visual inspection for QA, and will also give your fabricator an indication that they’re assembling your layer stack right the first time.
Get Your Layer Stack Right
There’s no reason to skimp on the process of carefully planning your layer stackup at the beginning of your design process. While many designers are just fine with defining their layer count and leaving the rest to their manufacturer, doing so leaves a lot to chance when considering future issues like radiation, crosstalk, and signal integrity. You know your design best, so doesn’t it just makes sense to be in control of your layer stack? By carefully planning your layer stack right the first time, you’ll be putting together the first line of defense to ensure that your board meets Electromagnetic Compatibility (EMC) requirements.
Ready to define a multilayer stack for your next electronics design? Subscribe to Autodesk EAGLE today!