-
- News
- Books
Featured Books
- design007 Magazine
Latest Issues
Current IssueLevel Up Your Design Skills
This month, our contributors discuss the PCB design classes available at IPC APEX EXPO 2024. As they explain, these courses cover everything from the basics of design through avoiding over-constraining high-speed boards, and so much more!
Opportunities and Challenges
In this issue, our expert contributors discuss the many opportunities and challenges in the PCB design community, and what can be done to grow the numbers of PCB designers—and design instructors.
Embedded Design Techniques
Our expert contributors provide the knowledge this month that designers need to be aware of to make intelligent, educated decisions about embedded design. Many design and manufacturing hurdles can trip up designers who are new to this technology.
- Articles
- Columns
Search Console
- Links
- Events
||| MENU - design007 Magazine
Seven Tips for Your Next Stackup Design
February 1, 2021 | Eric Bogatin, University of Colorado, BoulderEstimated reading time: 4 minutes
If interconnects were transparent, the stackup in your board would just be about how many layers you would need to route all the connections between components. In fact, some test boards that are strictly testing continuity and isolation do exactly this. Each layer is a dense packing of narrow signal traces connecting an array of pogo pin pads on the top side to an array of connectors to an ATE on the bottom side.
But rarely do we have the luxury of designing a board just for connectivity. When interconnects are not transparent, we must engineer them to reduce the noise they can generate. This is where design for signal integrity, power integrity and EMC—collectively high-speed digital engineering—are so important.
Seven Tips for Stackup
1. An important element in reducing the noise contributions from the interconnects comes from the stackup of the board and the layer assignments. The very first step is to engineer all signal layers with at least one adjacent plane as the return path. This will reduce the crosstalk between the signal-return paths: the microstrip traces on the outer layers and stripline traces on the inner layers.
2. The striplines can be either one signal layer between two planes or two signal layers between two planes. With two signal layers between two planes, there is the danger of excessive crosstalk if signals on adjacent layers are routed broadside to each other.
3. To avoid this problem, it is best to route the adjacent signal layers in dual stripline stackups orthogonally. One signal layer is routed in the x-direction, the other in the y-direction.
4. When interconnects must distribute 10 A of current or less, traces as wide as 200 mils can carry the 10 A of current in 1 oz copper with an acceptable temperature rise. But, with larger currents, like 20 A or more, it may be necessary to use wide planes to distribute the current from the power generators to the power consumers on a board. This is when some of the planes should be allocated as dedicated power planes.
The challenge is balancing the requirements of power distribution with the requirements for reduced crosstalk from signals changing return planes.
In principle, a signal line will see exactly the same characteristic impedance if the return plane is at ground potential or 12 V potential or anywhere in between. The problem with using a different voltage plane than ground to carry return current is when the signals change layers.
5. When a signal trace switches layers, we use a via to carry the signal current. If the return plane also changes, we will achieve the lowest crosstalk between all the signals switching layers when we also provide a via to carry the return current from the starting plane(s) to the final plane(s). This is a lowimpedance via shorting between the two different return planes. This is only possible if the return planes are the same voltage. If they are at different voltages, we can’t add a shorting via between them. This is a strong motivation to only use ground planes as the return planes for signals.
6. At best, if the two planes are a different voltage, we can add shorting vias between the two planes with a DC blocking capacitor between them. The loop inductance through a DC blocking capacitor can be as much as 5x higher impedance of a direct shorting via. It is a poor approximation to a shorting via, but the best we can do.
7. When signals change return planes and the planes are at different voltages, we run the risk of launching high bandwidth return currents into the cavity formed by the two planes. This is a source of long-range crosstalk and potentially a source of radiated emissions noise. One solution to reduce the noise in the power-ground cavity is by using very thin dielectric in these layers. This suggests that when power planes are used, they should be paired with closely spaced adjacent ground planes.
Once the order of the signal layers and planes is set, the dimensions can be calculated based on the line width of signal traces, the dielectric constant of the laminates used, and the target single-ended or differential impedance. This is where a 2D field solver comes in handy to define the cross section of microstrip traces, single layer stripline and dual layer strip line traces.
If you don’t follow these tips, it does not mean your board will not work. Unfortunately, there is no way of knowing if your stackup design will work or not unless you do a detailed analysis based on the driver models and 3D electromagnetic analysis of all the worst-case signal and power paths. Implementing these tips is about risk reduction.
They are part of a balanced diet of best stackup design practices, best signal routing design practices, and best power distribution design practices. And like all design guidelines, buyer beware. Always consider the best design practices, but also always do your own analysis.
This article appeared in the January 2021 issue of Design007 Magazine.
Suggested Items
Insulectro’s 'Storekeepers' Extend Their Welcome to Technology Village at IPC APEX EXPO
04/03/2024 | InsulectroInsulectro, the largest distributor of materials for use in the manufacture of PCBs and printed electronics, welcomes attendees to its TECHNOLOGY VILLAGE during this year’s IPC APEX EXPO at the Anaheim Convention Center, April 9-11, 2024.
ENNOVI Introduces a New Flexible Circuit Production Process for Low Voltage Connectivity in EV Battery Cell Contacting Systems
04/03/2024 | PRNewswireENNOVI, a mobility electrification solutions partner, introduces a more advanced and sustainable way of producing flexible circuits for low voltage signals in electric vehicle (EV) battery cell contacting systems.
Heavy Copper PCBs: Bridging the Gap Between Design and Fabrication, Part 1
04/01/2024 | Yash Sutariya, Saturn Electronics ServicesThey call me Sparky. This is due to my talent for getting shocked by a variety of voltages and because I cannot seem to keep my hands out of power control cabinets. While I do not have the time to throw the knife switch to the off position, that doesn’t stop me from sticking screwdrivers into the fuse boxes. In all honesty, I’m lucky to be alive. Fortunately, I also have a talent for building high-voltage heavy copper circuit boards. Since this is where I spend most of my time, I can guide you through some potential design for manufacturability (DFM) hazards you may encounter with heavy copper design.
Trouble in Your Tank: Supporting IC Substrates and Advanced Packaging, Part 5
03/19/2024 | Michael Carano -- Column: Trouble in Your TankDirect metallization systems based on conductive graphite or carbon dispersion are quickly gaining acceptance worldwide. Indeed, the environmental and productivity gains one can achieve with these processes are outstanding. In today’s highly competitive and litigious environment, direct metallization reduces costs associated with compliance, waste treatment, and legal issues related to chemical exposure. What makes these processes leaders in the direct metallization space?
AT&S Shines with Purest Copper on World Recycling Day
03/18/2024 | AT&SThe Styrian microelectronics specialist AT&S is taking World Recycling Day as an opportunity to review the progress that has been made in recent months at its sites around the world in terms of the efficient use of resources: