Beyond Design: Stackup Planning and the Fabrication Process


Reading time ( words)

Editor's Note: This article originally appeared in the April 2012 issue of The PCB Magazine.

Back in 1987, when I first started working on high-speed designs, the PCB stackup did not seem that important. If a board would not route, I simply added another couple of signal layers--problem solved. But that was running at a maximum frequency of 166 MHz, which at the time seemed fast.

Times have changed. Now, multi GB/s designs are becoming the norm and the stackup configuration, characteristic and differential impedance control are crucial to the performance and reliability of the product.

Rick Almeida of Downstream Technologies, Inc. pointed out in his article, What to Look Forward to in 2012 (The PCB Magazine, January 2012) that “The growing importance of stackup design and analysis will be recognized. Today, there is a growing need to plan and design the stackup properly, as well as optimize it for better overall performance and communicate and document stackup information between engineering and fabrication.”

I have previously written on the topic as well, but perhaps some designers are not quite at this level yet. Therefore, let’s look at some basic stackup configurations and briefly cover what is required for the fabrication process.

Dielectric Materials

Before starting a PCB design, we need to plan the PCB stackup and ensure that the selected substrate materials are available from our chosen fabrication--a step that is regularly missed. Changing the stackup towards the end of the design process could mean changing trace widths and clearances to achieve the correct impedance, which could create a lot of unnecessary work.

If we use the same materials that the fab shop stocks to build our stackup, then the impedance will be more accurate. If we just choose a convenient number, for core thickness, for example, then this may be up to 3% different off from what is available; hence, the impedance will vary by 3%.

The most widely used dielectric material is FR-4 and may be in the form of core or prepreg (pre-impregnated) material. Isola’s top selling materials are FR406 and FR408. While FR406 sets the industry standard for basic multilayer PCB fabrication, FR408 is a high-performance FR-4 epoxy dielectric for improved signal performance. Its low dielectric constant and low dissipation factor make it an ideal candidate for broadband circuit designs requiring fast signal speeds or improved signal integrity. Also, the high glass transition temperature makes it compatible with ROHS compliant components and most FR-4 processes. Figure 1 illustrates the available core materials in the default Dielectric Library Editor of the ICD Stackup Planner (download here).

The core material is a thin dielectric (cured fibreglass epoxy resin) with copper foil bonded to both sides. For instance: Isola's FR406/8 materials include 2, 2.5, 3, 4, 5, 6, 7, 8, 10, 12, 14, 18, 20, 21, 28, 31, 36, 39, 47, 59, 93 and 125 mil cores. The copper thickness is typically ½ to 2 oz (17 to 70 um). If you look at the datasheets from Isola (or any other manufacturer) these sizes are not very clear, so it is best to contact your fab shop for details on the materials they stock.

 

Figure 1: Isola FR406 and FR408 dielectric materials. (Click image to enlarge.)

The prepreg material is a thin sheet of fibreglass impregnated with uncured epoxy resin which hardens when heated and pressed during the PCB fabrication process. Isola’s FR406/8 materials include 1.4, 2.5, 2.9, 3.8, 4.5, and 6.5 mil prepregs that may be combined to achieve the desired prepreg thickness. These are the final thicknesses after processing.

The most common stackup, known as the foil method, is to have prepreg with copper foils bonded to the outside on the outermost layers (top and bottom), then core alternating with prepreg throughout the substrate. An alternate stackup is called the capped method, which is the opposite of the foil method and was used by old-school military contractors, but may still be fabricated today.

The total substrate thickness is generally 62 mils (1.6 mm) but may vary according to the application: 20, 31, 40, 47, 62, 93 and 125 mils are other not-so-typical thicknesses. Obviously, as the layer count increases the total board thickness increases. Twelve layers is the limit for 62 mil substrates. The configuration of the PCB stackup depends on many factors, but whatever the requirements, one should ensure that the following rules are followed in order to avoid a possible debacle:

  • All signal layers should be adjacent to and closely coupled to a reference plane, creating a clear return path and eliminating broadside crosstalk.
  • There is good interplane capacitance to reduce inductance at high frequencies.
  • High-speed signals should be routed between the planes to reduce radiation.
  • The substrate should be symmetrical with an even number of layers, which prevents the PCB from warping during manufacture and reflow.
  • The stackup should accommodate a number of different technologies.
  • Cost (the boss’s most important design parameter) should also be addressed.

It is not always possible to configure the stackup to have both tight coupling of the planes and tight coupling of the signal layers to the planes, as this depends on the number of layers and the available materials. Four- and six-layer boards typically have this issue. Fortunately, the lower layer count boards are generally used for designs below 100 MHz so the interplane capacitance may not be as important at these frequencies.

Figure 2: Four-layer board. (Click image to enlarge.)

In the four-layer board (Figure 2) the signal layers are < 10 mils from the plane, which helps reduce crosstalk, and the single-ended (Zo) and differential impedances (Zdiff) are 54 and 101, respectively. A good range of impedance (Zo) is from 50 to 60 ohms. Keep in mind that lower impedance will increase the dI/dt and dramatically increase the current drawn (not good for the PDN); higher impedance will emit more EMI and also make the design more susceptible to outside interference.

Figure 3: Four-layer board with dielectric materials. (Click image to enlarge.)

To communicate our intent to the PCB fab shop, we need to produce documentation detailing the required materials. In Figure 3, the centre core of 39 mils thickness has been replaced by a core from the Dielectric Materials Library which fortunately is also 39 mils thick. Also, in order to get a total of 8 mils thickness of prepreg between layers 1 and 2, as well as between layers 3 and 4, two sheets of FR408 2116 material are used, each totaling 7.6 mils. As mentioned, we cannot always get the exact value and this is where the inaccuracy occurs. The impedance Zo drops by 1.6 ohms (2.8%) and Zdiff by 2.4 ohms (2.3%). And, the total board thickness reduces.

Figure 4: Six-layer board. (Click image to enlarge.)

The six-layer board in Figure 4 again has close coupling between the signal layers and the planes--reducing crosstalk. The bulk of the board thickness is again made up of the centre core material. Broadside coupling between signal layers is reduced by keeping signal layers 3 and 4 far apart, and close to the reference planes. Ideally, these signal layers should be routed diagonally (or at 45 degrees) to each other to minimize the coupling. Routing pairs should be layers 1 and 3 (GND reference) and 4 and 6 (VCC reference). High-speed signals should be routed on the stripline layers 3 and 4 to reduce EMI.

Figure 5: Six-layer board with dielectric materials.

Figure 5 illustrates the completed stackup with all the dielectric materials defined, ready for pasting into the PCB specification and sent off with the Gerber and NC Drill data to the fab shop for manufacture.

Please see my previous article “The Perfect Stackup for High-speed Design” for information on additional stackups.

Points to remember:

  • Control impedance to ensure performance and reliability of the product.
  • Keep the signal layers close to the planes to reduce crosstalk.
  • Avoid broadside coupling by separating the internal signal layers with bulk core material.
  • Combine prepreg and core materials from the datasheets, in the stackup, in place of the defaults to improve accuracy.
  • Ensure that the selected substrate materials are available from your chosen fab shop.

References:

  1. What to Look Forward to in 2012” by Rick Almeida, The PCB Magazine January 2012
  2. Electromagnetic Compatibility Engineering—Henry Ott
  3. “The Perfect Stackup for High-speed Design”, by Barry Olney, The PCB Magazine November 2011
  4. The ICD Stackup Planner and ICD PDN Planner can be downloaded from www.icd.com.au

Barry Olney is managing director of In-Circuit Design Pty Ltd. (ICD), Australia, a PCB design service bureau and board-level simulation specialist. Among others, ICD was awarded “Top 2005 Asian Distributor Marketing,” and “Top 2005 Worldwide Distributor Marketing” by Mentor Graphics, Board System Division. For more information, contact Barry Olney at +61 4123 14441 or e-mail at b.olney@icd.com.au.

Share



Warning: array_rand() expects parameter 1 to be array, null given in /home/iconnect/releases/20160311/public_html/elements/next_item.php on line 41

Suggested Items

Video from productronica 2017: Karel Tavernier on Ucamco's New Communic8tor

11/20/2017 | Pete Starkey, I-Connect007
European Editor Pete Starkey and Ucamco Managing Director Karel Tavernier discuss Ucamco’s cloud-based Communic8tor platform which facilitates two-way communication between the CAM engineer and the PCB designer, or any other party involved in the manufacturing process. This gives real-time access to image data and annotations, enabling queries to be resolved, changes to be approved, and a full communications history to be maintained.

Signal Integrity: The Experts Weigh In

11/14/2017 | The I-Connect007 Team
When we began planning the October issue on signal integrity, we arranged a conference call with a variety of industry experts. Mike Steinberger of SiSoft, Mark Thompson of Prototron Circuits, and Yogen and Sunny Patel of Candor Industries joined editors Andy Shaughnessy, Patty Goldman, Happy Holden and Publisher Barry Matties on the call for a spirited discussion about the challenges related to signal integrity and some of the tricks of the trade for helping ensure SI.

Nine Dot Connects: Good Design Instruction is a True Value-Add

11/09/2017 | Andy Shaughnessy, PCBDesign007
Nine Dot Connects has certainly blazed an interesting trail. The company started out as an Altium reseller, but in less than a decade, Nine Dot Connects has also become a design service bureau and a provider of PCB design instruction, training, and consulting services. I recently interviewed Paul Taubman, technical services director for Nine Dot Connects. We discussed the company’s expansion from VAR to service bureau and content provider, and the changing landscape of PCB design instruction.



Copyright © 2017 I-Connect007. All rights reserved.