If you are new to rigid-flex designs—or have never done a rigid-flex PWB layout—you might wonder how it is similar to and different from hardboard design. In previous columns, I’ve discussed cost drivers in rigid-flex boards and applications where rigid-flex designs will outperform all other packaging methods, which more than justifies the increased cost. In this column, I’ll address critical items you need to know to successfully create a stable and robust rigidflex design.
Gerber files, artwork, and other aspects of communicating your rigid-flex design to a fabricator are very similar to what you would provide your fabricator for a hard board. Some folks don’t realize that the flex layers extend all the way through the rigid section on a rigid-flex board. This is why rigid-flex boards provide such a high degree of reliability in highshock, or high-vibration, environments.
The flex layers are integrated right into the board, just like a layer of 0.004” core in a rigid board.
A typical fabrication package will look similar to a hardboard design. The Gerber files, drill files, and design guidelines and recommendations will be very much alike. Where they differ is in controlled impedance requirements, material layups, detailed fabrication drawings, and special design rules around the rigid-to-flex transition areas.
Thus, a typical rigid-flex fabrication package will look comparable to a hardboard design package. Impedance Considerations Controlled impedance traces have become more prolific in digital and high-speed circuit designs. The software and test vehicles to provide this level of control have progressed in step with the demand as well. The dielectric materials in the flexible sections are different than hardboards and generally provide better electrical performance.
The coverlayers and bondplys also offer better electrical performance. These materials have varying dielectric constant (Dk) values and should be modeled in software that is designed to predict how each of the dielectrics, reference planes, and circuits relate to one another. Trying to do this in a rigid-flex design using free online impedance calculators will almost always return false values.
There are just too many interactions to use single-value calculators. Additionally, some of the material suppliers give global DK values when they can be different at different signal speeds in reality.
The best path forward is to purchase the software, which is available as a standalone product for an annual license fee and is often included and built into some of the more popular CAD PWB layout tools. The software is not cheap, but it is far more accurate than the free online tools.
Whether you decide to purchase the software or not, it is always wise to involve your fabricator at the start of your design to either predict the impedances you desire, or to double check your work if you used your own software. Your fabricator does impedance modeling dozens of times a day and has modeled impedance circuits for many years. They will have a material library with Dk values for the different material constructions and will know all of the impedance values for every thickness of every
dielectric they use. For each impedance value that you want to be modeled, tell your fabricator the value you desire, the type or characteristic of differential, on what layer(s), what speed the signal is at, what layer(s) the reference plane(s) are on, and any mechanical considerations (e.g., the board cannot be thicker than 0.062”, etc.). There are two important differences to keep in mind with impedance modeling of rigidflex circuit boards. The first is that the values, trace widths, and spacings will be different in the flex sections than in the rigid sections. Your fabricator should provide you with a model showing both calculations whenever you have impedance-controlled circuits in both the flexible sections and the rigid sections of the board. As a designer, this will require you to neck down the circuits to their correct geometries and spacing. The neckdown should occur 0.050” or more into the rigid board to prevent stress on the circuits at the neckdown area and the flex-to-rigid transition area.
You should also note that the number of impedance values can quickly multiply with rigid-flex designs. Each value often needs modeling and testing in the flex and rigid sections of the board. Because of this and the fact that each value needs to be tested in the impedance coupons that are built into your part’s production panels, the size of the coupons can grow very large, very quickly. The larger the impedance coupons on the panel, the fewer number of parts that your fabricator can fit on the panel, which ultimately increases your cost. Thus, it is wise to specify only those circuits that you truly need to be tested on your print. You and your fabricator can model all the values you want through the whole PWB, but just put on the print the values you truly need.
If you modeled the impedances as previously described, you are approximately 90% of the way towards a material layup. The report will give you the material cross-section with copper thicknesses, dielectric thicknesses, Dk values, etc. If you don’t have any impedance values to model, or you just need a straightforward material layup, ask your fabricator for their recommendations. Here is what they will want from you to get started:
• The overall number of layers in the rigid section(s): rigid sections can have differing amounts of layers of circuitry, but they should all end up the same thickness
• Desired copper thicknesses in the rigid section(s): innerlayers and outer layers with plating
• Number of layers in the flexible section(s)
• Desired copper thickness in flexible section(s)
• If there are more than three layers in the flex section, do you want them bonded together or loose-leaf?
• The desired overall thickness of the rigid board(s): over laminate, plating, or solder mask?
• Materials desired (FR-4, polyimide, etc.)
• Final finish
• Special requirements (UL, RoHS, REACH, lead-free and halogen-free assembly, etc.)
With this, your fabricator should be able to provide you with a suitable material layup as a starting point, which you can refine from there. Also, remember that many of the most popular laminates available on the market do not have a corresponding no-flow prepreg. Rigid-flex manufacturers have to use no-flow prepreg to keep the uncured resin from flowing onto the flexible areas of the board during lamination.
Your fabricator can recommend laminates with corresponding no-flow prepregs that will meet your requirements. Another good starting point for material layups is our Valu Build brochure. Valu Builds offer simple, stable, and robust material layups for rigid-flex that are also very economical.
They are ideal for someone who is just starting rigid-flex, looking for a good entry point, and seeking the lowest cost in a rigid-flex design.
Board designers and their fabricators often see the print as a list of requirements, which it surely is. But much more than that, the print communicates to the fabricator what your desires are as the designer. Without that communication, the fabricator isn’t always sure what you want. This is especially true for rigid-flex designs. Gerber files show your data and what you desire for holes, etc., but often it is not possible to tell where the rigid-to-flex transition areas are in the Gerber layers. This is where a detailed print—often much more so than an equivalent hardboard design—shows your fabricator precisely what you want.
Any dimensions across the flexible portions of the board should be referenced dimensions only. The flexible areas will expand and contract with temperature and humidity changes, so dimensions across the flexible portions of the board should be for reference only.
Rigid-to-Flex Transition Area
Design rules change around the flex-to-rigid transition area. There is a keep-out area on both sides of the rigid-to-flex transition line, particularly on the rigid side of that line. The keep-out area varies by the fabricator, but most fabricators will want you to keep all pads, traces, and vias a certain distance away from that line. In our case, we want all traces and the edge of pads at least 0.025” from the line and the edge of all drilled holes more than 0.050” from that line.
The reason is due mostly to cut-back coverlayer manufacturing (sometimes referred to as bikini processing). In high-reliability rigid-flex design and manufacturing, the coverlayer and bondply do not extend all the way through the rigid part of the board. They will typically extend 0.025” to 0.100” into the hard boards, but that also varies by the fabricator. The reason for using cut-back coverlayer is that the acrylic adhesive used to bond the coverlayer has a relatively high Z-axis coefficient of thermal expansion (CTE) rate—much higher than the surrounding laminates. During thermal cycling—think of RoHS and lead-free assembly temperatures—the expansion can put too much pressure on the vias and cause them to crack. Also, the acrylic adhesive does not drill, prep for plating, or plate well. Overall, it is not desirable in the rigid sections of your board.
There are times when it is not possible to use the cut-back coverlayer technique, and you must use full-sheet coverlayer/bondply.
However, whenever possible, use cut-back coverlayers and bondplys to provide the highest package reliability possible. Because of cut-back coverlayer, the edge at the flex-torigid transition area can have a slight radius to it. Any circuits or plated features in this area will struggle to image faithfully and will suffer yield loss.
For the same reason, the edge of the drilled via needs to be kept back from that transition line. If the vias are drilled partially through coverlayer and bondply and partially through prepreg, they will not yield—which typically shows as plating defects and opens at electrical test. It is the edge of the drilled hole that is critical and not the finished via size. If you call out a 0.012” finished hole on your design, fabricators usually drill that at 0.006” larger than the finished via size to accommodate plating thicknesses. If you put the edge of the finished via on the edge of the keep-out area, the drill itself will be drilling within the keep-out area.
It is wise to involve and consult your fabricator as to what their keep-out limitations are in the rigid-to-flex transition areas of the board, which can often vary by design. These are not absolute rules, just recommendations to get the best design with the highest yields and lowest overall cost possible.
1. Printed Circuits’ Valu Build Brochure.
Bob Burns is national sales and marketing manager for Printed Circuits Inc.