Flyback Converter Module PCB Design Project

Click here to jump to the viewer embed and browse this project

If you have an electronic product that converts AC to a moderate voltage DC while also providing isolation, then most likely you're using a flyback converter. Flyback DC/DC converters give the large step-downs required in AC-connected systems that also require a DC output, but without a big hit to efficiency. In this project example, I'll show how to design a basic flyback converter module, both in schematics and in a PCB layout.

Flyback converters require a transformer, and the transformer you use will determine the level of step-down and current handling that the device can handle. A big part of flyback converter design is the transformer design and selection, which could force you to use a custom transformer. We'll see how this arises in this project. At the end of this article, you'll have a chance to download the design files and start using them in your own designs.

Getting Started With a Flyback Converter

The flyback converter design I will show in this project is meant to convert 120 V AC input down to a 3.3 V output. The primary controller that will be used to run the flyback converter is the UCC28881 from Texas Instruments.

At a basic level, the device we want to design includes three stages:

1. AC input, circuit protection, and rectification
2. Flyback converter switcher and transformer
3. Output interface and isolated feedback loop

The schematics shown below illustrates each of these three stages connected together to produce the 3V3 output. This system is expected to handle 1-2 A of current. This system is also going to maintain isolation provided by the transformer, which requires careful placement of all of the components.

AC Input

The input leading to our transformer contains circuit protection components and a bridge rectifier (BR1). The circuit protection provided here includes a fusible resistor, metal oxide varistor, and a small amount of capacitance. On the output side of the bridge rectifier, we have a TVS diode and some additional capacitance to reduce ripple from rectification.

The goal of this section is to rectify the input AC and provide a semi-stable DC output to the switcher section while also providing circuit protection. Here, I have not added EMI filtering, but this could be added with low-pass filtering and some chokes (see below). How you add those elements depends on whether you will keep the chassis connection after the AC input. For now, let's proceed with a line and neutral connection and omit the earth connection.

Switcher Circuit (UCC28881)

The switcher circuit is based on part number UCC28881, which is an open-drain switching controller that includes a feedback connection and supports a wide input voltage range. The snubber circuit (made up of C1, R1, D1) provides stability during switching so that large overshoot/undershoot during switching can be suppressed.

3V3 Output and Feedback

The output stage is shown in the image below. This shows how the output is rectified down to a DC output via D2 and finally stabilized with some capacitors. The output section includes some testpoints for manual probing if desired, as well as a terminal block to attach flying leads. Note that C8 is marked DNP and is optional; its placement can provide further stabilization if required and can easily be determined from a comparative measurement with a scope.

The feedback section uses an optocoupler and a precision shunt regulator to stabilize the power through the optocoupler. The resistor divider R3/R7 biases the REF pin on the LMV431AIMF regulator to 1.244 V. The additional passives provide filtering/stability when the system is biased ON and the LMV431AIMF also switches from OFF to ON. The R2/R4 voltage divider biases the optocoupler to the correct voltage and current, and it will only allow current flow when LMV431AIMF is biased ON.

Transformer Design and Selection

Flyback converters use a transformer and its primary side inductance in order to step up/down the input voltage and regulate the output voltage. They are switching regulators that use the primary side inductance as a typical buck converter would use a regular inductor. 

To properly size the transformer, we need to determine the required duty cycle, coil inductances, and peak currents. First, we need to determine the turns ratio for T1, which depends on the desired output voltage (Vout) and the diode forward voltage drop (Vdiode, measured on D2 above). This will also determine the duty cycle for the switcher:

If you have an off-the-shelf transformer that has a specified turns ratio, then the flyback voltage can be determined. Or, if you want your switcher to run at a specific duty cycle, then you can determine the flyback voltage and thus the required turns ratio.

Next, we can determine the required maximum switching given the maximum duty cycle capability and the target output current.

Next, to help size the transformer, there is a requirement on the peak current:

The challenge with designing the transformer for a flyback converter is finding a transformer that balances the form factor, inductance value, turns ratio, and current handling limit. Most transformers that you buy off-the-shelf will only hit 2 or 3 of these requirements. From what I have seen, most of these off-the-shelf transformers that offer the required turns ratio and current handling, but they won’t give the required form factor.

This means you may need to design a custom transformer or work with an assembler to build a custom transformer. There are core and bobbin components available that can be used to assemble a custom transformer that will hit your inductance and turns ratio specs in a specific form factor. You will need to carefully assemble a custom transformer or contract with a vendor to have the component assembled.

The design shown below will use a TDK core insert (PN: B66417G0000X149) and TDK coil former (PN: B66418W1008D001), which is a through-hole part that could allow for center tapping if desired. Based on the target output voltage of 3.3 V and a reasonable switching frequency of 62 kHz for the UCC28881, the required turns ratio is 69:4 and the primary inductance is 984 uH. The peak current handling does not need to be excessively large for a low-power flyback converter module, which allows a small wire diameter of 26 AWG for the windings. The expected peak primary current is 0.44 A.

PCB Layout

The PCB layout is shown in this section and it is relatively simple to understand the approach to this layout. The goal here is to illustrate how to maintain the isolation required for this DC/DC converter and how to implement this in a module form factor.

The initial placement is shown below, and the isolation boundary is marked using the dashed white line. All of the large through-hole components have been placed on the top layer, while the smaller SMD components have been placed on the bottom layer. The AC input will attach using flying leads that solder to plated holes (left side), and the 3.3 V output is taken from a 2-screw terminal block (right side).

The IC that is spanning across the isolation barrier is the optocoupler (U2). This feeds directly into the UCC28881 switcher (U1) and completes the feedback loop. The placement of the optocoupler is such that it ensures a consistent isolation gap near the middle of the PCB.

To start routing, I first set some clearances that ensure sufficiently large spacing between parts in the design according to the IPC-2221 standards. You can calculate these required clearances using the data shown in this article. The clearances I use assume a 120 V AC input on the primary side.

Next, the routing is completed with somewhat large traces to ensure sufficient current handling on the primary and secondary sides. Note that there is a decently large gap around the power input traces (line and neutral), which could be a region where noise is received/emitted. It may be desirable to use larger polygons as pours to limit noise generation and reception at low frequencies.

Now we can draw in the remaining polygons to provide ground for the output and the switcher. These are drawn out below. I have also cleaned up the silkscreen to prevent clearance errors and overlapping designators. The large sections of copper shown below both provide ground for the switcher to help ensure shielding, and it will provide current handling capability for BR1.

This completes all the routing and cleanup required for the design. The transformer is a switching element that could be rather noisy, and addressing this is one of the potential changes that could be implemented in the design.

To download the original project files, follow this link. These files are available under a CC license.

Rev. B: Preparing the Design for Manufacturing

At its most basic level, the design as shown above will be functional and show high efficiency. It has all the basic elements needed for the design to function as an AC-to-DC regulator module. Based on some of the potential improvements I devised, I decided to update the design to prepare it for manufacturing and add some EMI filtering components.

To improve the design before manufacturing a test PCB, 

• Added a Y-type capacitor across GND-P and GND
• Added a cutout between the transformer and optocoupler leads to clearly denote the isolation region
• Added an input low-pass filter to address conducted EMI (common-mode and differential-mode)
• Added an output filter to address conducted EMI (common-mode and differential-mode)

Regarding the first point, this is a typical way to bridge grounds in an isolated DC power supply as it helps control return paths for high frequency signal components originating from the switching waveform. If there is a problem with high frequency radiation from the 3V3 side, then a Y-type capacitor (usually about 1 nF) can help suppress that.

On the input side, we have the following component updates on the power stage. The two new caps across the Line and Neutral connections (C10 and C11) are X-type safety capacitors which will shunt high-frequency common-mode noise on the input power cable to ground (in this case, Earth ground). Finally, note the placement of the Y-type capacitor (C12); this is placed to link the secondary and primary ground, but it is the primary ground net AFTER the rectifier stage (net name PGND).

On the output side, I have added a combination differential and common-mode filter from Murata, part number BNX026H01L. This filter provides low-pass filtering for both types of noise with 5th order roll-off, providing 35 dB of insertion loss from 50 Hz to 1 GHz. Given the switching frequency in the design, the lowest order frequency in the switching waveform will be mildly attenuated, but all higher order harmonics will be heavily attenuated.

This completes the Rev. B design. To complete the PCB layout, I expended the board size along the length direction to make room for the input and output filters. These filters involve some large components and so the board no longer precisely occupies a brick form factor, but the module is still close to this size. The updated layout is shown below.

To further improve the design for EMI/EMC purposes, we could do the following:

• Place chokes on the input side if common-mode noise is a problem
• Add a chassis guard ring and connection to earth for a metalized enclosure
• Remove the input solder holes and add a standard receptacle for an AC plug
• Add an additional secondary tap and change the winding ratio to produce a dual rail module

The first point is important in general for EMC on input power stages. Creating a front-end EMI filter using an LC filter (pi filter) and placing chokes on the input will suppress common-mode noise coming from the AC line input. We could do the same on the output side so that we can eliminate common-mode radiation on the output wiring cable, but the output Murata filter essentially performs the same function as a common-mode choke.

To see a review of the Rev. B design as it is being prepared for manufacturing, watch this video on Altium Academy:

To download the updated (Rev B) project files, follow this link. These files are available under a CC license. You can also explore the Rev. B project files on my company website or in the Altium Viewer embed below.

Whenever you want to build stable and reliable power systems, use the complete set of PCB design features and world-class CAD tools in Altium Designer®. To implement collaboration in today’s cross-disciplinary environment, innovative companies are using the Altium 365™ platform to easily share design data and put projects into manufacturing.

We have only scratched the surface of what’s possible with Altium Designer on Altium 365. Start your free trial of Altium Designer + Altium 365 today.