<img height="1" width="1" style="display:none" src="https://www.facebook.com/tr?id=140460429997534&amp;ev=PageView&amp;noscript=1">

EMI Shielding Methods for Flex & Rigid-Flex PCB Designs - Q&A

Epec Engineered Technologies
Written by Epec Engineered Technologies
Posted on September 9, 2021 at 12:09 PM

At the conclusion of our webinar, EMI Shielding Methods for Flex & Rigid-Flex PCB Designs, we had several questions submitted to our presenter, Paul Tome, Product Manager of Flex & Rigid-Flex Circuits at Epec. We have compiled these questions into a readable format on our blog.

Q&A From Our Live PCB Webinar

Quick Links:

Watch the Recording Below:

Free Download: Top 6 Flexible Circuit Board Design Checks

Question: Are there other shielding materials available?

Answer: This actually ties in with discussions that we've had with customers very recently, specifically copper or aluminum foils, conducted tapes, sputtered metals, and the simple answer for that is yes, but not for flex and rigid-flex applications. They're just not part of the industry's demand for flex and rigid-flex PCBs. Sputtering metals is a very unique process, and at the end of the day, we just haven't seen any application that has ultimately demanded that that can't be solved by the three methodologies that we discussed today.

Question: Can a shielding film or silver ink be used for current carrying requirements?

Answer: The most common being a ground return circuit. And per the materials manufacturer's specifications, the answer to that is no, it should not be used as a ground return. The material itself was never designed and/or rated to carry any current, and you need to keep in mind that the electrical connection between the shielding film is an electrically conductive adhesive. It is not a soldered or copper-plated connection, so that can create some issues..

Question: Can ferrites be used on flexible circuits?

Answer: In general, yes. Not overly common, but I have in prior history manufactured flexible circuits that ultimately have a ferrite inserted onto them. Some of the concerns: it may create some assembly issues because in most cases the flex will need to be threaded through and/or wrapped around the ferrite. And you'll need to do this first before any connectors or components are attached because typically the opening of the ferrite isn't going to be large enough to accommodate anything more than the thickness of the flex. So, under those circumstances, it might force the flex to be hand-assembled, which is always, you know, in a small quantity run, it can be considered. In larger volumes, it’s definitely not the preferred solution. In general, we find that adding a ferrite to a flex circuit works best if the flex is a ZIF connector design, where there's no additional connector required. So, you'll have at least ZIF contact fingers on one end of the flex circuit, which will allow you to thread it through the ferrite without compromising the assembly process.

Question: This goes back to the controlled impedance design question and why aren’t silver ink and shielding films recommended?

Answer: As I touched upon before, one of the biggest challenges is achieving the correct dielectric thickness between the signal layer and the shield layer, which is now also required to act as a reference plane. You need to accomplish that thickness by the coverlay. Coverlays are typically on the thinner side, half-mil, 1-mil thickness is the two most common thicknesses for coverlay, which is not going to be enough for. It's not going to be thick enough for your dielectric thickness to hit your impedance values. You can laminate multiple coverlays to get to that thickness, but you're now adding cost and thickness again. But the biggest concern then becomes now, with this added thickness of coverlay, either the silver ink or the shielding adhesive needs to penetrate down into this cavity that you've created in order to access the ground net, and the adhesive is only so thick, and it can only accommodate a certain amount of thickness in the coverlay before it just can't make proper connection to the ground. And as I also mentioned, because of the characteristics of the material, and the inconsistencies of it in relation to copper, your controlled impedance tolerance is going to increase, in some cases, beyond what the design is going to allow you to utilize. You're going to be easily up into the plus or minus 15% to 20% range now on your controlled impedance.

Question: How do I know if I require shielding?

Answer: This is a very, very common question that a lot of customers come to us. We'll get involved at an early design stage, in many cases, a conceptual one. And at that point in time, the customer is unsure as to what their shielding requirements may or may not be. They're either unknown or they have to be defined. And what we do in the majority of cases at the prototype stage as part of one order, we'll supply parts with and without shielding films under one part number and under only one tooling charge, and that'll give our customers the opportunity to evaluate the designs both with and without the shielding, and then make an informed decision moving forward in the production as to whether or not shielding in specifically required for their design.

Question: How does the thickness of the film affect the 50x to 100x bend radius for continuous flexing environments?

Answer: The added thickness of the shielding film becomes part of the overall thickness of the flex circuit which then is used to define the minimum reliable bend radius for a dynamic flex application. The advantage of shielding films is that they allow for a much thinner construction and in turn a tighter bend radius. While the shielding film is inherently more flexible than a copper layer this is not factored by IPC 2223 flex design standards when calculating the minimum bend radius. Only the total thickness of the design is used.

Question: What is the common rule-of-thumb for bend radius of flex circuit given copper layer shielding?

Answer: Once copper shielding is added to the design the total flex layer count will increase by two layers. The recommended minimum bend is a function of the total thickness of the flexible area. In general, the min. bend radiuses are as follows:

  • 3-layer flex: 20x finished thickness
  • 4-layer flex: 30X finished thickness

Question: The ZIF connector can be noisy. What is your recommendation to shield? Also, any information on double-sided EMI film?

Answer: While we do see many designs that utilize “standard” ZIF connectors, we agree that they can be a source of EMI emissions. There are ZIF connectors that do include shielding however we seldomly see them used. In general, any shielded connector system that can be attached to a rigid PCB can be utilized on a flex circuit to meet your EMI requirements. All EMI shielding films are designed for external use on a flex circuit as such they are defined as a single-sided material. Due to the slip properties of the external most insulation layer, no other materials can be effectively laminated to a shielding film. For an internal flex layer shielding requirements, between two signal layers as an example, a copper shielding layer will need to be used.

Question: Do you have a single slide showing relative cost, flexibility, and performance (shielding effectiveness) between the 3 methods discussed?

Answer: A single slide is a challenge and currently not available as there are a large number of variables from design to design. In general, from feedback from our customers, we see shielding films being as effective as a solid copper plane solution. We have not had a single report of ineffective EMI performance after 1000s of applications. Flexibility is significantly improved on average by 50%, due to the significant reduction in the flex thickness. Cost for a shielded flex design is on average 25% less than that of a comparable copper layer shielded design. Data on the silver ink method has not been tracked for a number of years due to the almost complete lack of demand that we see in the industry.

Question: Do you ever mix shielding methods? (e.g. copper layer on one side for impedance matching and shielding film on the other side).

Answer: Yes, we do see designs that utilize both shielding film on one side and a copper plane on the other. However, these designs are non-impedance-controlled as the EMI shielding film is not well suited for achieving impedance control. We do see 3-layer controlled impedance stripline configurations that use power and ground nets as the reference planes and then require additional shielding external of the power and ground planes.

Question: What is it about the other materials that limits the usefulness for controlled impedance designs? Are they just significantly less conductive than copper at RF/microwave frequencies?

Answer: Material conductivity does have a negative impact as both shielding films and silver ink are far less conductive than copper. There are also additional mechanical issues that create limitations: coverlay thicknesses need to be increased significantly to achieve the required dielectric spacing to achieve the impedance values. Coverlays of the required thickness are not commonly used in the industry as reduced flex thickness is a standard requirement to meet bend requirements. Thicker coverlays are also not readily available or stocked. To overcome this a multiple coverlay lamination construction would be required. Both shielding films and silver ink require selective openings in the coverlay to expose and access the ground net. With the thicker coverlay, these openings become relatively deep which in some cases does not allow the shielding film’s conductive adhesive to extrude down into the openings and create an effective electrical connection to the ground.

Question: When designing a flex board in EDA tools how do I include shielding films in my design?

Answer: We’ve seen this as a challenge for customers as most if not all EDA/CAD tools do not have design provisions for shielding films. If modeling the performance of the design is necessary, the shield films can be represented as added external solid copper planes. To specify the shielding films in a production data set, we most often see customers define them as mechanical layers or as additional coverlay layers. Either the mechanical layer or additional coverlay solution is based on standard soldermask design parameters. We then take those files and update them to meet the technical and manufacturability requirements of the shielding film and submit them back to the customer for review/approval and to update the data set. A drawing note is also be included identifying the shielding film requirement(s).

Question: How does silver ink affect impedance?

Answer: “If” the silver ink can be used the impedance tolerance will increase to 15-20 % due to the material properties and limitations in the manufacturing process. An additional issue is that thicker coverlays are needed to achieve the required dielectric spacing to meet the impedance values. Coverlays of the required thickness are not commonly used in the industry as reduced flex thickness is a standard requirement to meet bend requirements. Thicker coverlays are also not readily available or stocked. To overcome this a multiple coverlay lamination construction would be required. Because of the above items, we have not seen a design with controlled impedance specify silver ink reference planes in over 15 years.

Question: Are these methods mostly used to limit emissions or for susceptibility?

Answer: A shielding requirement, independent of the shielding method used, serves both to limit the EMI emissions of a flex circuit and to limit the flex circuit’s susceptibility to absorb EMI emissions. Emitting EMI could negatively meet EMI standards while absorbing EMI could negatively impact the performance of the flex circuit itself.

Topics: Flex & Rigid-Flex PCB's

Download our Flex & Rigid-Flex Circuits Design Guide

Leave a Comment

Subscribe to our blog Subscribe to our blog

Recent Posts

Quote Your PCB's Online

InstantPCBQuote - Online Quote and Ordering Solution for Rigid PCB's

Register today and start to quote and order your circuit boards online, 24/7.

Start Quoting Now

Need Help with A Project?

Request Design Support

Our team of engineers are here to help you with all your product needs.

Request Design Support