Fullscreen HTML5Med Res (??MB)HTML4

By Geoff Graham Professional PCB Assembly If you aren’t confident soldering small SMDs, don’t have time or don’t want to populate your boards with dozens or hundreds of components, there is another option. For a modest fee, you can have your boards professionally assembled using parts that you specify, and in many cases these components will cost just a pittance! O ur first article on the Second Generation Colour Maximite 2 computer (which you can see on page 26 of this issue) mentioned that you could have the PCB professionally assembled. This includes the PCB fabrication, supply of the components and the soldering of these components onto the board. So, how do you get that done? The process is remarkably cheap and easy, even if you only want a couple of boards assembled. For the home constructor, this is a boon as you can now ‘hire’ a machine to assemble a complex board that would be difficult, if not impossible, to put together yourself. You design your PCB using SMD parts as you would normally do, but instruct your PCB design software to generate two extra files: a Bill Of Materials (BOM) and a Component Placement List (CPL). With these files the fabricator has enough information to supply the components and solder them in their correct positions. For a relatively complicated PCB like the one used in the Second Generation Colour Maximite 2, this saves the effort involved in sourcing then tediously soldering over a hundred tiny components. Furthermore, for someone who is not comfortable soldering SMD components, this avoids that issue entirely. It is worth reflecting on how the times have changed. A little over ten years ago, a typical hobby project would be based on a single-sided PCB etched and drilled at home. Even Silicon Chip projects were based on PCBs The assembled prototype PCB for the Second Generation Colour Maximite 2, exactly as received from JLCPCB. It has about 100 components supplied and soldered, with only the large components (connectors, switch etc) to be fitted. siliconchip.com.au Australia's Australia’s electronics magazine August 2021  35 like that. Now, a fabricator will make you a four-layer PCB for the price of a hamburger and then populate it for the price of a six-pack of VB. How great is that? Designing the board Most PCB design software can generate BOM and CPL files. As an example, the designer of the Second Generation Colour Maximite 2 printed circuit board (Peter Mather in the UK) used DesignSpark. This is a free program from RS Components, and it did a great job. To fabricate the prototype Colour Maximite 2 board, we used a company called JLCPCB (https://jlcpcb.com/) in China. There are other companies (mainly in China; there are some in Australia too) who will do the same, so you are not restricted to JLCPCB. Still, we will use them as an example of how you go about getting your own boards populated. We have covered how to design PCBs before, so we will not go over that again. However, to get the fabricator to populate the board, you need to supply one more bit of information to the PCB design software. This is the unique part code assigned by the fabricator to each component. The fabricator needs these numbers to identify the components to load into their pickand-place machines. If you go into the JLCPCB website, there is a link at the top labelled “Resources”, and if you click on that you can then select “SMT Parts Library”. Then you can browse the various categories (Capacitors, Resistors etc) in their catalog, or you can search using a part code or a value. These are all surface mount components (JLCPCB can assemble some through-hole components by “hand soldering”, at an extra cost). When you select a component, it will list the part code used by the fabricator, which, in the case of JLCPCB, is called the “LCSC Part number”. You must then enter this part code into the properties of the component in the PCB design software. You can also search for parts (and find their numbers) at the LCSC website, which is a Chinese component supplier and the sister company of JLCPCB (http://lcsc.com). This is an example of the Bill Of Materials (BOM) file generated by DesignSpark. The fabricator uses this file to associate a component’s reference designator with their part code. An example of the Component Placement List (CPL) file, used by the pick-andplace robots to place the component on the PCB. It lists the part’s designator, the PCB coordinates of the centre of the component, which side of the board to place the part and the orientation (ie, rotation). 36  Silicon Chip Australia’s electronics magazine It’s important to know the capabilities of the manufacturer; JLCPCB’s can be found at https://jlcpcb.com/ smt-assembly For example, they can only perform PCB assembly on boards between 20 x 20mm and 250 x 250mm in size, with a quantity of no more than 50 PCBs. Parts selection There are a few tricks to selecting parts. If the part is not in their catalog or identified as “Not Stocked”, you will have to source and solder that part yourself after receiving the board. This is true of most non-SMD components, including connectors. But do not be put off if you cannot initially find the component that you need. It might be listed in a different package, different temperature specification etc. An extended search often will get you what you need; JLCPCB says that they stock over 80,000 components. As a last resort, it might be easier to redesign your circuit to use something that they do have in stock, for example, a regulator with a different footprint. If you plan to have the Second Generation Colour Maximite 2 board assembled during 2021, you will probably find that the ARM processor and the 32 megabit memory chips are out of stock. This is due to the current semiconductor shortage; all you can do is wait until they come back into stock, then get in quickly before they run out. JLCPCB lists components as being either “basic” or “extended”. Basic parts are always loaded on their pickand-place robots and are ready to be placed onto your PCB. This primarily applies to items like small resistors and capacitors. The extended components are the less common items that are stored in their warehouse. These must be retrieved and loaded on the pick-andplace robot specially for your build, so they attract an additional charge per item (generally a few dollars each). You need to watch out for the extended fee, as it can add up. For example, the Second Generation Colour Maximite 2 board was initially designed using M3216 (3.2 x 1.6mm, imperial 1206) sized resistors, but most of these are listed by JLCPCB as extended parts. Given the number of different resistor values, that would have added over $40 to the board assembly cost. siliconchip.com.au Redesigning the PCB to use the slightly smaller M2012 (2.0 x 1.2mm, imperial 0805) resistors, listed as basic parts eliminated that cost with no difference in functionality. The components supplied by JLCPCB are generally reasonably priced. For example, an M2012/0805 SMD resistor is less than half a cent. The other factor is that there is no wastage; your project might need (for example) one 10W resistor. If you were assembling that at home, you would likely end up purchasing 10 or even 100 to get that single resistor at a reasonable cost. Component Placement Files With the correct part codes entered into the component properties, you can then get your PCB design software to generate the Bill Of Materials (BOM) and Component Placement List (CPL) files. These are spreadsheets, normally in Excel format. Depending on the software, these files might need some reformatting to suit the fabricator’s specifications (eg, adding headers, swapping columns etc). The BOM file is a list of all components, including their description, the reference designator (R21, C1 etc), the component footprint and the fabricator’s part code. The fabricator is really only interested in their part code and the reference designator. The CPL file lists the reference designator, the X and Y coordinates of the component’s centre on the board, the PCB layer that the component is to be placed on and the rotation of the component in degrees. JLCPCB can only populate one side of a PCB, so in our example CPL file that side is the top layer. The PCB is defined by files in the standard Gerber format, and these are the same as you would use if you were only getting a PCB made without the component assembly. You do need to supply the “paste” file (which is used to create the PCB stencil), which has the outlines of the solder paste stencil that is used to deposit solder paste on the pads as required. Most PCB assemblers will add a separate charge to manufacture the PCB stencil. For a four-layer PCB, as used in the Second Generation Colour Maximite 2, there are a total of ten files required to make the PCB, plus the “paste” file. Placing the order JLCPCB requires that you create a siliconchip.com.au login so that you and they can manage your job. You can then upload your Gerber files defining the PCB. That is easy; just drag and drop the ZIP or RAR file containing all the files onto the web page. Following this are multiple options that you can select (solder mask colour, PCB thickness, copper finish etc), but you can leave these at their defaults for most projects (including the CMM2 Gen2). JLCPCB will auto-fill most of the entries based on the Gerber files which is very convenient – but not all manufacturers do this, so take note. At this point, the website will ask you to select which Gerber files represent the various copper layers on your board and the number of boards that you want to be made. If you just want a PCB (without assembly), you are finished. But at the bottom of the web page, there is a button that allows you to select “SMT assembly”. If you choose that, you will be asked how many you want to assemble and who should add the tooling holes. The tooling holes are small holes in the PCB used in the assembly process, and you usually let JLCPCB add them. Clicking “next” will take you to a web page that asks you to upload the BOM and CPL files. Again, this is a simple drag-and-drop operation. Final checks Clicking “next” again will take you to the summary page. This page lists all the components on the board and provides a ‘preview’ of the assembled board. It is vital that you check this thoroughly as it is easy for a mistake to propagate through, and this is the last checkpoint before sending the board off for assembly. For example, you might find some components listed as being out of stock, and this is where you need to go back to the JLCPCB parts list and select something different. You can either go back to your PCB design software to make the change, or you can just manually edit the BOM file and change the part number there. Either way, you will have to upload your files again and recheck the component listing to ensure that all is OK. The final step is to check the preview provided by JLCPCB of the assembled board. This image is very realistic and shows the PCB with its Australia’s electronics magazine solder mask, vias and silkscreen in great detail. The components are photorealistic, with their markings clearly visible, and they should be positioned in their correct location. This image is almost as good as having the final board in your hand, and provides confidence that you will get what you intended. A detailed check of this image is vital, as it can show all sorts of errors that you did not realise existed when you designed the board. The most common is incorrect component orientation. It is possible that the orientation of the component in your PCB footprint will be different from the footprint used by JLCPCB. That can cause polarised components to be reversed, ICs with pin 1 in the wrong place etc. So check every part thoroughly and, if necessary, edit the CPL file to change the orientation parameter for the offending component, then reload the file. The final result With the component list and image checks completed, JLCPCB will present you with a list of the costs that make up the total price for the assembled board. This includes the price for the board itself, fixed setup charges, extended parts charges, the cost of components etc. Of course, the service is more cost-effective if you are getting a reasonable number of boards made, but it is still worthwhile if you only want two boards assembled (their minimum). The cost of our assembled board for the Second Generation Colour Maximite 2 (as shown in the photo) was about $10 for the four-layer PCB, $59 for the components and $19 for assembly (plus postage). These costs are per board, for two boards and in Australian dollars. Since then, the exchange rates and component prices could have changed, so your experience might vary. Given the complexity of the board, we feel that this is a reasonable price, especially considering that everything is supplied and soldered for you. The actual assembly cost was small, and it makes you wonder why you would be bothered soldering a hundred tiny components when you could have it done professionally for the price of one dish at a restaurant. SC August 2021  37