Getting started with Maxim EE-Sim® OASIS Part 2: Schematic Capture & PCB LayoutFollow article
Designing a switch-mode PSU PCB layout, and getting ready for PCB manufacture.
Picking up from where we left off in Part 1, we now have a suitably designed and simulated SMPS that can take 9-30V, and output 5.1V at up to 2.5A. The next step is to capture the schematic in Designspark PCB and then produce a suitable PCB layout ready for manufacture.
The online Maxim EE-Sim DC-DC Converter Tool that we initially started the design in produces both a schematic that can be downloaded, and a Bill of Materials with the appropriate component choices. This gives us a convenient starting point to build upon.
You will notice that the design has now changed slightly to use a different switching controller, the MAX17576. This is because this part has a wider availability, and a slightly higher output current of 4A which could be utilised if the design was modified.
Once the Bill of Materials was downloaded, we found a number of 0402 size components, which are somewhat fiddly to solder by hand. We opted to change these to larger 0603 variants as the planned board size would be large enough to accommodate all the components. Any parts that were already 0603 or larger would be left alone.
Given we already had a schematic to base our design off, the schematic capture was a rather painless process, and consisted of redrawing the schematic, changing some component values, and adding some additional parts.
A new project was created in Designspark PCB, and then a blank schematic created within the project. This opens a completely blank canvas ready for adding components and connections.
We first started by adding the input capacitance for the power supply. The automatically generated schematic called for one 2.2uF 50V rated ceramic capacitor. This swapped out for a larger capacitance part rated for 10uF 50V (as a rule of thumb ceramic capacitors should have their working voltage derated by approximately 50%, which gives us enough headroom for our input voltage). We picked Samsung CL32B106KBJNNNFas a suitable replacement.
The datasheet for the MAX17576 clearly states that there is a distinction to be made between PGND and SGND, which is to be used for the compensation network and feedback components only; requiring the creation of schematic symbols for PGND and SGND. This is easily done by right-clicking on a placed “GND” component, selecting “Components and Symbols” then “Edit Component in Library”. In turn this opens the editing window for a component, and may give you a warning about the RS part number being missing or invalid - this can safely be ignored. The component can then be edited, we changed the terminal name and net class, and then saved back into the library under a different name.
As there is not an included component for the MAX17576 that we are using, this has to be downloaded from the online PCB Part Libraryand can then be imported into Designspark PCB. This is a painless process, as the online library has a schematic symbol and PCB footprint already created. Samacsys, the provider of the library, also has produced a free Library Loader utility which makes searching & loading parts a quick, streamlined process.
Once downloaded and installed, upon first launch the Library Loader tool provides clear instructions on how to configure the utility. It is a straightforward process, requiring nothing more than logging in, setting the appropriate PCB design tool, and specifying which library to store components in.
From then on, once “Download” is clicked on the RS PCB Part Library, the component is automatically imported into Designspark PCB and becomes selected on the cursor.
We added some additional parts to the designed schematic, mainly an input conditioning circuit and two LEDs for status monitoring.
At this point a new PCB was created in the project. The “New PCB Wizard” appears which guides you through the process of creating a blank PCB. We selected the “Double Sided (Metric)” technology file, as the design is not overly complex and would easily fit on a double sided PCB.
The next window asks you to specify the layers that should be included in the design. As we had already picked a suitable technology file to use, the default option of “Use Layers from Chosen Technology File” was left checked. After this, the next window asks you about PCB sizing. This was chosen to fit on top of a Raspberry Pi, dimensions of which can be found on Github.
Once this has been completed, and an appropriate name has been given to the board, we are presented with a blank PCB. From here on, components are placed on the PCB in roughly the right place, but not yet connected. It is particularly helpful to see if the manufacturer of your IC provides a reference design - in this case Maxim have produced the MAX17576EVKITB.
Once components were roughly in suitable positions, routing was started.
This was done following the reference design for the SMPS, which involves separation of SGND and PGND to keep noise away from the sensitive analogue inputs on the controller. This was done by drawing a pour for SGND, then creating a narrow keepout pour around this, then the PGND pour was completed on the top layer.
I found that certain track classes needed to have widths changed. For example, a net that was classed as a signal had a width of 0.5mm, which is far too wide to connect to the pads of the MAX17576. This can be changed by going to Settings > Design Technology > Track Styles, where the window below appears. The “Signal Nom.” and “Signal Min.” widths were reduced down to 0.25mm and 0.13mm.
Once the layout was completed, it was reviewed to ensure that everything looked OK, and everything that should be connected was indeed connected. We then proceeded with setting up for the manufacturing file outputs, which are often Gerber files. This was done by checking our chosen PCB manufacturer’s guidelines for input formats and settings. In this case, Eurocircuits require 6 digits of precision in the output, if the output units are set to imperial.
This can be done by going to Output > Manufacturing Plots (or pressing Shift+P), selecting the layer you wish to edit, heading to “Device Settings” and then editing the required fields. Your PCB manufacturer may suggest other settings that need to be changed, and they can be edited from this window.
Once all the correct settings have been inputted, the design is ready to be exported as Gerber files containing the manufacturing data. This can be verified to ensure the design looks correct by using tools either provided by your PCB manufacturer, or others such as https://gerber-viewer.ucamco.com/ - this is my preferred Gerber viewer. Once the design has been checked, it is time to send it off to your PCB manufacturer to be produced.
In part 3 of this series, we'll assemble and test the Raspberry Pi PSU to see if it meets the outputs of the simulation, and to ensure it can handle powering a Raspberry Pi reliably.