Fullscreen HTML5Med Res (??MB)HTML4

PIC n’Mix Mike Hibbett’s column for PIC project enlightenment and related topics Part 4: PIC18F Development Board I n the last PIC n’ Mix article (January 2021), we discussed the design requirements for a PIC18F development board, creating enough detail that we believed this month’s task of designing the schematic and layout of the board would be simple. Now, let’s put that to the test. Our goal this month is to take the highlevel schematic shown in Fig.1 and create the design for a PCB that we can have manufactured quickly and cheaply by a PCB supplier. We will go with JLCPCB based in China for this board, to test how easy their service is to use compared to our favourite supplier PCBWay. We will be designing this board in EagleCAD, which is now part of AutoDesk’s Fusion 360 product offering. The software is still available for free to hobbyists and small companies; and it has been our default PCB design tool for over a decade. We’re using it out of familiarity, but completely free CAD programs such as KiCAD would be just as suitable. Due to its continual development KiCAD has become a viable alternative to commercial programs, and we will one day move over to it. Not this month though! PCB design process The CAD design process for our board will follow a fairly standard process. We have already chosen our component technology – through hole, not surface mount – and thanks to the relatively slow speeds of the signals on the board, we know that a simple double-sided board, with components mounted on one side, will be acceptable. We don’t have any design constraints on the size of the PCB so we shouldn’t need complicated ‘tricks’ like components mounted on both sides, or a four-layer PCB to allow the components to be positioned close together. Space between components will be desirable for ease of assembly and access to pins/leads with test clips or probes. The final dimensions of the board will only become clear once we have placed our components roughly in their positions. 50 We start with a large outline for the board, iteratively place components, reduce the board dimensions and then move components again until the right balance of board size and component proximity is achieved. Component placement is a personal choice, as there are no specific design constraints, but it seems sensible to have power and the main I/O signals at the edge of the board and the CPU in the middle. Library of parts That’s the process but we’re getting a little ahead of ourselves. First, we need to create a schematic, and for that we need a library of components to choose from. There is a ‘chicken and egg’ situation here; while EagleCAD (in common with all CAD programs) comes with an extensive library of components, it is reasonable to expect that some of our desired components may not be present – requiring us to design the footprint, mechanical layout and schematic symbol for these missing parts. Creating library parts can be a tedious task, but a search on the Internet can often reveal downloadable libraries created by companies and other hobbyists. A simple Google search, such as ‘EagleCAD DC Barrel socket library’, can often be successful, but also note that libraries for many components are made available by some component suppliers such as Farnell, RS Components, Sparkfun and Adafruit. The process for creating a component library is complex as there are additional features that must be drawn, including the location of solder paste, silkscreen and solder mask. The mechanical dimensions must be accurate too, or you risk the component not fitting. So, finding and reusing a pre-existing library is highly desirable, and is one of the reasons we have stayed with EagleCAD over the years – it seems to be the most popular CAD program for downloadable libraries, although KiCAD is growing in popularity. Our preferred approach when an existing library cannot be found is to pick an existing component that uses the same physical package, copy it and modify it to the requirements of the new part. It’s quite possible we may need to do that for our choice of processor, at least. Let’s begin the journey by going back to our high-level schematic, shown in Fig.1, attacking each circuit subsystem in turn and identifying the required components. Once done, we can simply ‘bolt’ them together on the schematic, with perhaps an extra decoupling capacitor thrown in for good measure. Power supply We have already decided that we want to be able to support both 3.3V and 5V as the system voltage, since some sensors and servos run at the higher voltage. This could be achieved using two voltage regulators with a 0.1-inch jumper header to select between them, but to save cost we went with the LM317 – an adjustable output voltage linear regulator. This is a very simple low-cost regulator, available in easy-to-solder packages. It’s not an efficient regulator and will waste some energy as heat, but since we are not targeting battery power for this board that’s not much of an issue. Although the datasheet is difficult to read (there are many uses for this regulator) it boils down to the circuit shown in Fig.2, with decoupling capacitors on the input and output power pins. We replace the single resistor R2 with two resistors, and a jumper shorting one of them sets the desired output voltage. The jumper allows the ‘R2’ resistor to be switched between 390Ω and 720Ω, and a resistance of 240Ω for R1 giving the desired voltage. To connect power to the board we will allow for two options – a standard ‘barrel jack’ connector, common on mains ‘brick’ power supplies, and 0.1-inch header pins for quick wire connection. The barrel jack presents an interesting problem with the PCB design, which we will pick up on later. Practical Electronics | March | 2021 G P I O6 (U AR T2 ) G P I O4 (U AR T2 ) U S B G P I O7 (U AR T2 ) G P I O18 (P W M) S ervo G P I O19 (P W M) S ervo Op amp G P I O5 (U AR T2 ) G P I O8 W i-Fi G P I O9 Op amp G P I O10 G P I O11 I2 C G P I O2 9 (I 2 C1) P ower input G P I O3 0 (I 2 C1) G P I O12 (S P I 1) G P I O2 0 (P W M) S ervo G P I O13 (S P I 1) Micro-S D Media card G P I O12 (S P I 1) G P I O14 I2 C G P I O15 Additional power headers G P I O2 9 (I 2 C1) G P I O3 0 (I 2 C1) G P I O1 G P I O16 G P I O2 G P I O12 (S P I 1) FET FET G P I O3 S tatus L ED G P I O2 1 P OR TC0 G P I O2 2 P OR TC1 3 2 kHz crystal S P I G P I O12 (S P I 1) G P I O13 (S P I 1) G P I O14 (S P I 1) G P I O13 (S P I 1) G P I O14 (S P I 1) L CD MCL R G P I O2 3 G P I O2 4 S P I G P I O2 5 (ADC) G P I O12 (S P I 1) P OR TB 7 G P I O13 (S P I 1) P OR TB 6 Deb ug G P I O14 (S P I 1) G P I O2 6 (ADC) G P I O2 7 (ADC) G P I O2 8 (ADC) Fig.1. Our PIC Development Board’s high-level schematic (see PIC n’ Mix, January 2021). USB interconnection FET subsystem Next, we look at the USB serial interface, which will be based on the MCP2221A IC from Microchip. Despite the complexity of what it does, the support circuitry for this device, as shown in the data sheet, is very simple – just two capacitors – see Fig.3. We copy this directly. For the physical connection, USB connectors are only available in surfacemount format. They are very challenging to solder so we will use an off-theshelf USB connector breakout board that provides an easy-to-solder 0.1inch header interface, which we will connect to with a plug and socket arrangement. If you are looking to save costs, you could take a standard USB cable, cut the end off and solder the wires directly to header pins. We will tackle the FETs next. In the previous article we did not go into the details of how the FETs would be configured, which does leave some ambiguity. Will we use a high-side or low-side FET switch? By this we mean, will the FET be tied to the positive supply line, or the ground? We will take the simpler approach, which is to place the FET switch in the ground supply line. This has two benefits: the circuit will require N-channel FETs, which tend to have a lower resistance between drain and source resulting in a smaller-package FET that can sink a relatively large amount of current for its size. Second, the gate ‘on’ voltage level only needs to be a few volts above ground, so we can drive it directly from the CPU, reducing component count. L M3 17 V in I nput Now that choice has been made, our design decisions become: n What current do we want to be able to support? n What package are we willing to tolerate for the FET (TO92 or the larger TO220)? n Will the FET switch on with a digital signal from the microcontroller? V IN FET sub system D2 1N 4 001 V out V DD Adj ust R 1 1 2kΩ L DO 3 .3 V V U SB R 2 20kΩ Fig.2. Power supply schematic (from Microchip datasheet LM317). Practical Electronics | March | 2021 In D+ D– 1 2 TR 1 TN 2 106 R 5 240Ω P IC pin 8 5V (U S B b us) or ext ernal power supply Output HDR 4 P IC pin 9 Out HDR 5 R 7 1 Ω D3 1N 4 001 1 2 TR 2 TN 2 106 R 6 240Ω R 8 1 Ω U S B Tranceiver Fig.3 USB interface (from datasheet Microchip CP2221A). 0V Fig.4. FET subsystem (the power comes directly from the supply, not the regulator). 51 We decide to go with a TO92-packaged TN2106N3-G, from Microchip. It has a very low resistance, 0.35Ω; will turn on with a gate voltage of 2.2V; and can sink 1.2A continuously. This seems a reasonable compromise; FETs in the TO220 package can sink tens of amps, but supporting such a current drain would have introduced challenges to the rest of the PCB design. The basic building blocks for our FET drive circuit (we decided to add two such circuits in our design) are shown in Fig.4. This is a simple and standard configuration for low-side N-channel FETs. The resistor to ground is there to ensure that the FET does not turn on accidentally, should the I/O pin driving it be set as an input (not a problem if no load is connected to the FET, but could be problematic if one were.) The series resistor may come as a surprise – The gate input resistance on a FET is extremely high – in the order of 100MΩ. What possible effect could a 220Ω resistor have? The gate of a FET has a relatively high capacitance, and there can be a brief but high current surge as the gate voltage rises and charges the gate. A low-value series resistor is a simple and low-cost method to reduce that current peak down to a few tens of milliamps. As we do not intend to be switching the FET on and off at high frequencies, the resistor is an appropriate solution. If we were designing a switching power supply with a gatesignal switching speed of over 100kHz, then a dedicated high-current driver circuit would have been required. On a development board like this, the value of that series resistor is fairly unimportant, so we may change the value later to a common value used elsewhere, to reduce the number of component variants. As a final point, you can see in the FET circuit that we’ve added a reversebiased diode across the header. This is an optional component, designed to cater for any inductive loads you might be switching (such as motors or relays.) These loads generate a large back-EMF voltage spike when power is turned off, and the diode will conduct this energy safely to ground. The FETs have a ‘body’ diode within their construction, but if the inductive load is large (or you are passing a large current) a discrete diode will provide a more powerful sink for this voltage spike, preventing damage to the FET and the microcontroller. Component type count Reducing the number of different components used is an important step in the design of any electronic product; for example, having 50 components with 50 unique values on a PCB will 52 S Y S TEM_ V P ower supply CON 1 D1 1N 4 001 **C4 and C5 close to V DD pin of I C2 C6 close to V DD- 2 pin of I C2 S Y S TEM_ V 1 IN OU T 2 ADJ 3 I C1 L M3 17 R 1 240Ω R 14 240Ω C2 100nF R 2 0Ω JP 2 1*** C3 1µF HDR 1A 1 + 1 C1 10µF 3 5V HDR 1B + C4 ** 10µF 3 5V C5** 100nF C6 ** 100nF L ED2 G reen 1 2 R 3 0Ω G N D G N D U S B sub system ***Fitted 3 . 3 V N ot fitted 5V 1 11 HDR 3 * *Can fit a female header here C11 100nF C10 1µF 4 5 4 13 3 12 2 V DD U R X V SU B U TX R S T 5 6 10 S CL D+ D– G P 2 V SS 1 1 1 2 2 2 3 3 3 R C2 G N D HDR 9 HDR 10 HDR 15 1 2 2 3 3 4 4 R B 1 S Y S TEM_ V G N D HDR 11 R 10 4 7kΩ HDR 12 1 HDR 13 1 2 2 3 3 4 4 5 5 R C4 R C3 S Y S TEM_ V G N D G N D HDR 14 1 R B 0 S P I Exp ansion sub system R C5 7 I 2 C exp ansion sub system R C7 S Y S TEM_ V 3 8 G P 3 I C3 MCP 2 2 2 1A G N D R C6 2 G P 0 G P 1 1 S ervo sub system 9 S DA R 11 4 7kΩ Fig.8. Our PIC Development Board’s final schematic. result in a higher cost than if there were only 20 unique values – simply because buying more of one item will give a bigger volume pricing reduction. This is why you may see some unusual values chosen for certain components in product designs – a 5.6kΩ resistor used as a pull-up instead of the more typical 4.7kΩ, perhaps because elsewhere on the circuit a 5.6kΩ resistor was required for a very specific reason. Such is the life of a product design engineer! CPU subsystem The processor subsystem is next. This is surprisingly simple; a standard minimum circuit from the datasheet. A resistor-capacitor circuit on the MCLR pin to provide the normal power-on reset delay, plus a few capacitors on the two voltage rails. We have decided to add the (optional) low-frequency 32kHz crystal, as that enables us to experiment with very-low-current consumption application options. (The main internal Practical Electronics | March | 2021 S Y S TEM_ V Analogue sub system R 12 220kΩ HDR 19 1 FET sub system HDR 2 0 R 13 220kΩ 1 R 4 4 7kΩ 11 V DD R E0/ R D/ AN 5 V DD- 2 R E1/ W R / AN 6 R E2 / CS / AN 7 2 MCL R / V P P / R E3 R A0/ AN 0/ C12 I N 0 – 3 R A1/ AN 1/ C12 I N 1 – 4 5 6 7 14 13 3 3 3 4 3 5 3 6 3 7 3 8 3 9 4 0 12 3 1 R A2 / AN 2 / V RE F – / CV RE F / C2 I N + R D0/ P S P 0 R A3 / AN 3 / V RE F + / C1I N + R D1/ P S P 1 R A4 / T0CK I / C1O U T R D2 / P S P 2 R A5/ AN 4 / S S / HL V DI N / C2 O U T R D3 / P S P 3 OS C2 / CL K O U T / R A7 R D4 / P S P 4 OS C1/ CL K I N / R A7 R B 1/ I N T1/ AN 10/ C12 I N 3 – R C0/ T1OS O/ T13 CK I R C1/ T1OS I / CCP 2 R B 4 K B 10/ AN 11 R C2 / CCP 1/ P 1A R B 5/ B I 1/ P G M R C3 / S CK / S CL R B 6 /B I2 /P G C R C4 / S DI / S DA R B 7/ B I 3 / P G D R C5/ S DO R C6 / TX / CK R C7/ R X / DT V SS R 5 240Ω 8 JP 2 D3 1N 4 001 R 7 1 Ω 1 1 1 2 2 JP 2 3 JP 2 4 5 + 3 C7 100nF 19 2 0 R 6 240Ω R 9 240Ω 2 1 TR 2 TN 2 106 JP 2 9 I C4 b MCP 6 04 P JP 2 8 3 JP 1 2 2 3 3 2 9 C8 C9 12 pF 12 pF 2 6 3 3 1 1 2 2 2 2 3 3 3 3 1 HDR 3 6 2 3 2 5 2 1 2 5 JP 3 2 X 1 3 2 . 76 8 kHz 2 4 1 1 JP 18 2 7 JP 15 17 JP 1 3 0 16 2 6 7 R 8 1 Ω L ED1 G reen 3 JP I C4 a MCP 6 04 P 2 3 2 1 – 6 1 4 – 2 3 1 + 1 HDR 5 10 Op amp sub system 2 2 3 TR 1 TN 2 106 9 2 8 R D7/ P S P 7/ P 1D R B 3 / AN 9/ C12 I N 2 – / CCP 2 3 2 7 R D5/ P S P 5/ P 1B R B 2 / I N T2 / AN 8 2 2 2 2 R D6 / P S P 6 / P 1C R B 0/ I N T0/ FL T0/ AN 12 1 D2 1N 4 001 G N D 3 2 HDR 4 1 1 10 + 1 9 – 3 JP 3 0 I C4 c MCP 6 04 P 1 8 HDR 3 4 HDR 3 5 V SS I C2 P I C18 F4 7K 4 2 (Fit in S K T1, a 4 0-pinDI P ) MCL R HDR 17 HDR 18 1 2 3 3 4 4 5 5 6 6 7 7 8 8 R A0 R A1 R A2 R A3 R A4 R A5 R E0 R E1 R E2 S Y S TEM_ V G N D R A7 R A6 OS CO OS CI R C2 R C3 R D0 R D1 1 2 G N D CP U sub system R B 5 9 9 10 11 11 12 12 13 13 14 14 15 15 16 16 17 17 18 18 19 19 2 0 2 0 HDR 3 7 12 1 + 13 – 1 P G D P G C 10 G N D L CD sub system R B 4 R B 3 R D4 R B 2 R D5 R B 1 R D6 R B 0 TD7 S Y S TEM_ V R A4 G N D R A5 R D7 R A6 HDR 2 R D6 8 R D5 7 R D4 6 R C7 R C6 P G C R C5 P G D R C4 S Y S TEM_ V R D3 G N D R D2 MCL R oscillator can be turned off completely, while the processor wakes periodically timed by the very-low-power 32kHz crystal.) That requires just a crystal and two capacitors. We added a 10µF bypass capacitor on the supply rail out of habit, this may prove to be unnecessary but it’s good to have the option of one on the board. Finally, there’s an LED to one of the GPIO pins, as everyone loves a flashing LED. You can see the original application circuit recommended by Practical Electronics | March | 2021 5 4 R C4 R C5 S Y S TEM_ V G N D 3 R D0 3 R D1 4 5 S Y S TEM_ V 11 1 HDR 3 9 G nd HDR 8 2 4 5 6 7 8 G N D 3 R D2 R D3 R D4 6 7 8 R A7 R C3 R B 5 2 1 14 HDR 3 8 W i-Fi sub system HDR 16 1 I C4 d MCP 6 04 P S D media card sub system 9 HDR 6 7 10 11 12 13 2 1 6 3 5 2 4 1 R A1 R C5 R C4 R C3 S Y S TEM_ V G N D HDR 7 4 3 R A3 R A2 S Y S TEM_ V G N D 2 1 Microchip in Fig.5, and compare it with the final schematic in Fig.8. Analogue subsystem Extending the high-level design from last month, we decide to add an analogue subsystem. This will be two ‘trimmer’ style variable resistors, connected to the supply rails. This gives us two variable voltages, which can be connected to ADC inputs on the processor. Not only will this allow testing of ADC-software designs, but also it can provide a useful ‘user interface’ for some projects, such as setting an audio frequency or a delay time. Op amp subsystem This leaves us with the op amp circuit. Since it’s an analogue circuit on a digital board it caused the greatest amount of thought. We want it to be general purpose, but the range of circuit configurations for inverting and non-inverting 53 C2 V DD R 1 V DD R 2 V SS MCL R C1 P I C18 (L )Fxx V SS Recommended values C1, C2 100nF, 2 0V , ceramic R1 10kΩ R2 100Ω to 470Ω Fig.5. CPU subsystem (from Microchip datasheet 2607031). deep within the library part of the barrel jack, as can be seen in the PCB layout in Fig.6, is a routing profile. This calls for a very small routing drill, as the hole measures just 1mm wide. Thankfully, this is a normal process requirement for PCB suppliers, and the resulting PCB can be seen in Fig.7, with a perfectly created plated-through slot. You must mention the presence of this slot to your PCB supplier though, in case they miss it. We have no need to add bypass capacitors on the DC power input, as the voltage regulator circuit has that covered. You do not want to add too much capacitance on the power rails as at some point the input capacitance will cause large inrush currents when the supply is turned on, which can introduce its own unique set of problems, typically voltage spikes on the power lines. amplifiers is huge – even before you start to bring filters into the equation. In the end, we took the lazy (and most flexible) approach – we provide power to the op amp and added pads on the input and output pins to enable you to build up any configuration you (or we) choose in future articles. We gave this some more thought and came up with the idea of an ingenious (we hope) arrangement of solder pads that will make constructing various op amp circuits easy. A small prototyping area around the op amp, with three pads connected together, will allow for mounting resistors and capacitors around the op amps while minimising the number of wires. We settled on the MCP604 quad op amp IC, again from Microchip, to minimise the component count. Time will tell whether this prototyping layout idea works! The Servo motors, SD-Media, Wi-Fi and SPI/I2C interfaces are just 0.1-inch headers with no additional components required. When it comes to connectors, the multitude of headers on our board are simple to implement as these are standard parts available within the EagleCAD libraries. The DC barrel jack on the other hand presents something of a challenge if you have not used one before. The connections to the PCB are flat tabs rather than simple round pins, which cannot be created by drilling a hole. The flat tab connections will require a small slot to be milled out of the PCB. Buried So now for the more exotic parts: n DC Barrel Jack n Processor n Crystal n MCP2221A n LM317 n FET, TN2106 n Op amp MCP604 Fig.6. DC Barrel Jack PCB footprint, from EagleCAD library. Fig.7. DC Barrel Jack footprint on a real PCB – note the slots for the jack’s pads. 54 Finally, the schematic Now that we know the required components we are almost ready to start drawing the schematic. We still need to check whether the components we want are available within the EagleCAD standard libraries. We start by looking for the common components, which will certainly be already present within the library, which are: n 1/4W resistors in an axial 10mm pitch layout n 1/4W resistors in a radial layout (might save some board space) n Capacitors on a radial 0.1-inch pitch (low-value parts) n Capacitors on a radial 0.2-inch pitch (high-value tantalum or electrolytic devices) n Diodes, similar package to the resistors n Header pins, on a 0.1-inch pitch, various lengths n Standard, single-colour 5mm LED. To our delight the MCP604 and LM317 were already present in the library. The crystal was slightly harder to find (we like the cylindrical wire-ended ‘watch crystal’ format). Two parts were found in the library, but the package name did not match any part we could find on Farnell, our favourite component supplier. In the end, we temporarily placed one of the standard library crystals on our board, and carefully measured the dimensions of the holes and the silkscreen outline of the package, then compared these to the datasheet of parts on Farnell. We found a match and made a note of the Farnell part number and the library designator for the part. Despite an extensive collection of Microchip processors in the EagleCAD library, with over 17,000 processor variants and more being released each year, it was no surprise to find our particular device – the 40-pin DIL PIC18F47K42 – was not present. However, what we did find was a PIC18F43K20 in an identical package with an identical schematic symbol. We will simply rename the part when we drop it into the schematic. Again, it was no surprise to find that our choice of FET, the TN2106 in a TO92 package was not present. As an N-channel FET has a simple 3-pin construction, we chose the first N-channel FET already present in the library – a 2N3819. A quick look at the datasheet for this FET indicated that it would not be a suitable alternative to use directly, but the pinout is identical to the TN2106, so again we will just rename the part name when adding it to the schematic. That leaves the MCP2221A IC. A quick search on the Internet revealed a library created, and publicly available, on DIYmodules.org – thank you! The library file was downloaded and copied to our EagleCAD library directory. As with all third-party library files, we did a careful check of the component’s design, double checking pin connections and the dimension and positions of holes. It’s an important step, but thankfully reviewing someone else’s component design is a lot easier than creating your own! So, through a combination of luck and searching the Internet we have found all of our required parts. Armed with these and the circuit subsystems, we can start to draw the schematic, pulling in the components we have identified. We start with the power supply section, then the CPU subsystem, USB IC, op amp, FETs and finally the headers. The completed schematic is shown in Fig.8. Note how the schematic does not resemble a PCB layout of the components; instead, we keep the design in a logical block layout, as this simplifies reviewing the parts and the interconnections. Practical Electronics | March | 2021 Fig.9. Initial PCB design view. These correspond with the industry ‘default’ values and will therefore be the cheapest option available. There are many other options to choose from, but for PCBWay and JLCPCB, these other options can be left at their default. Five days after placing the order, the package of boards shown in Fig.12 arrived – at the same time as the components. Assembly and testing At the end of schematic design we switch to the PCB layout stage. EagleCAD creates an internal datafile called a ‘netlist’, which is a formal description of the parts used and the wiring connections between them. When the PCB editor opens for the first time, it shows the collection of parts on the left, with an outline for a default PCB, as shown on the right of Fig.9, which measures 160mm × 100mm. It’s clear that these parts will fit a PCB of this size, but the number of interconnections that we are required to manually route for signal connections looks daunting! The task becomes easier as you place components in their approximate intended positions. After a few hours we arrived at the component placement shown in Fig.10. Not too compact, yet we were able to reduce the board dimensions down to 150mm × 100mm. Notice how we improved the legibility of the PCB by adding helpful text and boxes to show some of the subsystems. These additions to the silkscreen content add no cost; it’s just a question of how much time you want to invest in adding and tweaking details. The routing of the signals themselves was a process of first connecting up all the power rails, using nice thick tracks, taking short routes between components. We spent an hour hand-routing the data signals, and then allowed the autorouter to finish of the final track routes. The end result, with the top layer shown in red and the bottom layer shown in blue can be seen in Fig.11. Note that we have placed holes in the corners of the board to allow for mounting the PCB. Plus, there is plenty of space on the underside for adhesive rubber feet to allow the board, once assembled, to rest nicely on a desk. Adhesive rubber feet can be found in DIY hardware stores. PCB type 2 layer Silkscreen Colour Green PCB thickness 1.6mm PCB finish Hot air surface levelling Now for the fun part – assembling the board. We assemble one subsystem at a time, testing each new subsystem as we proceed to simplify debugging. The boards will have had a simple electrical test after manufacture, so there should be no shorted traces or open circuits – any issues with the board after assembly will be caused by us! It’s worth noting at this point that it is rare for a PCB design to be successful on the first iteration. In our professional Fig.10. PCB component placement. PCB sourcing When sourcing the PCB from a supplier, we had some PCB parameters to choose from. The key points were: Practical Electronics | March | 2021 Fig.11. PCB track layout completed. 55 Fig.12. Real PCBs! experience over 35 years, this has never happened. ‘Unsuccessful’ has quite a broad range of definitions of course, ranging from ‘it catches fire when we apply power’ to ‘the font used on the silk screen text is incorrect’. What might be a failure for the likes of Apple may well be perfectly acceptable to us. Now is the time to find out! Visual inspection The first thing we do, before soldering a single component, is visually inspect the PCB. There is a fairly standard checklist: n Are the PCB dimensions acceptable? When designing a board, we sometimes need it to fit in an enclosure with precision. We check that the PCB has the correct outline and any slots cut as specified. This is not an issue for us, as we are not fitting the board into an enclosure, but it’s worth checking that the dimensions are correct, within tolerance, as it confirms the quality assurance of the manufacturing process. Errors in something as simple as the board outline could signal more concerning issues later on. Fig.13. Silkscreen print detail. 56 n Are all the silkscreen details pres- ent? This is something that you can get caught out on when designing a board. You may put text or graphics on a particular layer, but then forget to include that layer in the Gerber pack you send to the manufacturer (happened to us more than once!) n Are all the silkscreen details legible? It’s too easy to specify thin text or graphic details that look great on screen, but look terrible with the manufacturer’s process. It’s not an exact science and difficult to judge when you are looking at a perfectly rendered design in a CAD package. n Are all the holes and milling profiles aligned? It’s possible that the centre of the drill holes may not line up with the PCB pads, either because of poor manufacturing tolerance, or a misinterpretation of the CAD data (PCB tracks and drill positions are held in different files, in different data formats.) n Are all the holes and milling profiles suitable for use? Sometimes, component legs may be thicker than expected, and will not fit in the holes. Connectors with wide flat pins – like our DC power jack – require milling rather than drilling. Did the manufacturer spot this, and are the dimensions OK for your actual connector? Once these checks are complete, you can relax a little. When we examined our board, we spotted one small issue – the header pin interface HDR8, on the top right of the board, does not include the text ‘WiFi’, to indicate the module intended to connect to it. This is a very small point – people using this board will know the purpose of the connector, and the Wi-Fi module can fit on only one header – but it’s an annoying omission. The silk screen layer on the PCB is our ‘canvas’, and at no additional cost we can print whatever we want on it, so to miss printing something that is useful is regrettable. We will correct that in the final PCB design. Our smallest silkscreen print detail, shown in Fig.13, came out very clearly with all text visible, so that’s a plus point. Now we can look more closely at the manufacturing detail, with the aid of a magnifying glass. Are the drills nicely centred in the pad holes? By this we mean, is there a good amount of copper around any throughplated holes? How well is the solder-resist aligned with the pads? In our design, where all components are soldered manually, this is not an important point; but with surfacemount components, a poorly aligned solder resist print could mask parts of pads which should be clear. As you can see in Fig.14, there is an offset in the solder resists outline, but it is within the manufacturer’s stated tolerances and causes us no issues. Then a second issue was found – the holes for the MicroSD card holder have the card entry slot pointing inwards, not away from the PCB. While this will work OK, it is not what we had intended. That was a simple design error on our part, and rather surprising too, as it was a point we thought about during the design. Not sure how that slipped through, but that is why we prototype, check – and check again. Initial assembly and testing We build the power supply section first, perform a quick continuity check across the supply pins, then apply 9V DC input. We measured 5.3V without the header fitted, and 3.4V with it fitted. Current consumption (without any load at this stage) is 5.7mA, which is almost exactly the current through R1, R2 and R3 – as expected. We can now fit the power LED. Next, the CPU subsystem – just the minimal parts: the IC socket, the PIC debug header and the CPU. Using MPLAB IPE Fig.14. Solder resist layer (mis)alignment. Practical Electronics | March | 2021 www.poscope.com/epe Fig.15. At last! – we have a built PIC Development Board. It’s not yet fully tested, but so far it looks very promising. we connect to the MCU. After confirming the device can be read, we proceeded with fitting the remaining CPU subsystem components (MCLR pull-up, capacitors and the user LED) then checked the PIC could be read again. Current consumption rose to 16mA, due to the processor running ‘blank’ code. FETs next, followed by the USB IC and the op amp. A recheck of the current consumption shows no significant increase, so we finish off by installing all the 0.1-inch-pitch header pins, and the four header sockets for the Wi-Fi, USB and SD-Media interface boards. Now we can test a peripheral. We start with the easiest, a servo motor. The interface works, and with two plugged in we check current consumption. An extra 20mA at 5V, and no significant heat increase from the regulator, even without a heatsink fitted. The USB interface was a joy to test – we do not have a USB software stack to mess with, as the MCP2221A IC provides us with a UART interface to the processor. We simply enabled the UART interface in software, mapped the UART RX and TX signals to the correct pins (as shown on the silkscreen) and success. So easy, and cheaper than buying an FTDI USB-to-UART cable. The Wi-Fi interface was validated by routing the Wi-Fi’s UART interface through the processor and out to the USB serial interface, making the processor appear as a ‘pass-through’ wire. With a terminal program running on a PC, we were able to send AT commands to the ESP-01 module. Another subsystem ticked off. Testing the other subsystems – the Micro SD-Media interface, the analogue and op amp circuits – will have to wait until next time, but so far things are looking great for the first revision of the PIC18F development PCB. Practical Electronics | March | 2021 Summary In our next article we will cover the software side of testing, as this will introduce the MPLAB-X IDE, and the MCC Code Configurator tool, which simplifies the setup of the drivers for the various peripherals on the microcontroller. We will also present the parts list and PCB ordering details once validation has completed, so you can follow along with your own PIC Development Board hardware. - USB - Ethernet - Web server - Modbus - CNC (Mach3/4) - IO - PWM - Encoders - LCD - Analog inputs - Compact PLC NEW! 5-year collection 2015-2019 - up to 256 - up to 32 microsteps microsteps - 50 V / 6 A - 30 V / 2.5 A - USB configuration - Isolated PoScope Mega1+ PoScope Mega50 All 60 issues from Jan 2015 to Dec 2019 for just £35.95 PDF files ready for immediate download See page 6 for further details and other great back-issue offers. Purchase and download at: www.electronpublishing.com - up to 50MS/s - resolution up to 12bit - Lowest power consumption - Smallest and lightest - 7 in 1: Oscilloscope, FFT, X/Y, Recorder, Logic Analyzer, Protocol decoder, Signal generator 57