| A number of things are required before starting a PCB design. They include: | ||||
| Board Dimensions | ||||
| A functional PCB is not a finished product. It will always require connections to the outside world to get power, exchange information, or display results. It will need to fit into a case or slide into a rack to perform it's function. There may be areas that will require height restrictions on the board (such as a battery holder molded into the case or rails in a rack the board is supposed to slide into). Tooling holes and keep-out areas may be required in the board for assembly or manufacturing processes. All these outside factors need to be defined before the board can be designed, including the maximum dimensions of the board and the locations of connectors, displays, mounting brackets, or any other external features. | ||||
| The function of a PCB includes the thickness of the copper laminated to the surfaces. The amount of current carried by the board dictates the thickness of this copper foil. Refer to the tables elsewhere in this site for information on calculating trace widths for specific current at specific copper thickness. Copper laminate thickness is usually defined (at least in the United States) in ounces per square foot. For general use boards like the ones we are talking about, most manufacturers will use 1oz copper, but since there are many others available it needs to be defined before starting the design. | ||||
| Parts List / Bill of Materials (BOM) | ||||
| The parts to be mounted on the PCB should be detailed on the parts list. Each part should be identified by a unique reference designator and a part description (i.e. a resistor might be shown as reference designator "R1" with a description of "1/2 Watt Carbon Film resistor"). Any additional information useful to the assembly process can be included on this list, such as mounting hardware, part spacers, connector shrouds, or any other material not shown in the schematic diagram. | ||||
| Data Sheets | ||||
| Part manufacturers provide data sheets to be used by the circuit designer to select parts for the circuit. If we are to be able to design the PCB, these sheets should also have the physical dimensions of the part included. If each part type to be used on the board does not have a data sheet, you should procure a sample part you can measure to define this data yourself. This measurment method is far less accurate than using the part manufacturer's information, especially if there is a large tolerance on the part, but it is better than just guessing. | ||||
| Schematic | ||||
| A schematic diagram must be made available that shows the connection of the parts on the board. Each part on the schematic should have a reference designator that matches the one shown on the BOM. Many schematic layout programs will allow automatic generation of the BOM. | ||||
Preparing the Design | ||||
| Generate the netlist | ||||
| A "netlist" file is usually required to design a board on an ECAD system. The file has the device names of the parts used on the board and a list of "nets" (interconnections between the pins of those parts). The file should be generated by the system used to generate the schematic, but may have to be typed in by hand if the schematic was manually drawn, or the schematic program can not generate a netlist the ECAD system will accept. This file is critical to PCB function. It should be double checked whenever time allows, since the smallest mistake can scrap the finished board. | ||||
| Build the symbols | ||||
| Parts are mounted to the board in a variety of ways. The method we will talk about here is called "through-hole," in which a wire lead or formed metal pin is inserted in a hole on the board and soldered into place. This process is still widely used, although many commercial designs now use what is called SMD. These designs are beyond the scope of this document (at least for now.) | ||||
| Most ECAD systems define the parts to be placed on a board as a special type of file called a "symbol." This allows better use of the computer's memory and disk resources by allowing multiple instances of a part to be represented by the same file. Symbols also allow the process of design to go faster, since you just have to build the part once and insert it a number of times instead of building it each time you need it on the board. Since procedures for building a symbol change for different ECAD systems, a general procedure is the only way to explain the process. | ||||
| PCB symbols are generally built in a hierarcy: Pads are defined, packages are built on the pads, and devices are built using the packages. | ||||
| Pads are the entities that interface the part pins to the copper traces of the board. The hole in the pad must be big enough to allow for variations in the pin size, variations in the hole size, variations in the hole location, and variations in the pin location. The pad must be big enough that the hole always has some copper around it on the surfaces of the board. Most ECAD systems also add solder mask information to their pad file, although there may need to be areas kept free from solder mask that are not associated with any pad. | ||||
| All these dimensions depend on the accuracy of the data sheet and the standards the board manufacturer uses. Most board shops can hold tolerances very well with the following calculations: | ||||
Pad Diameter = Finished Hole Size + (.020" or more) Soldermask Diameter = Pad Diameter + (0 to .010")
| ||||
| Some explanations: | ||||
| It is good practice (and makes for less expensive boards) to minimize the number of different hole sizes. You can vary the hole sizes within the range given to minimize the different sizes used, but remember that a hole that is larger than the ranges shown may be difficult to solder. You should use the bigger diameters of the range if the part is going to be auto-inserted so the machine tolerances are allowed for. | ||||
| The amount to be added to the hole size when calculating the pad size will vary depending on the current the pin will be conducting. The .020" figure should be considered a minimum for manufacturing the board, not as a general recomendation. Also remember that it is much harder to solder to a large area of copper than a smaller one. Don't make a pad huge just because you have the space. | ||||
| Check with your board manufacturer to get their recomendations before designing the PCB. Many board shops can easily increase soldermask openings to match their manufacturing tolerance, which is why the minimum size is specified as the pad diameter. | ||||
| Packages are the entities that represent the part. They consist of pads, lines, and text. | ||||
| ||||
| Devices are the entities that link the value or part number of a part with the ECAD package. It is much easier to design one "DIP14" package and a number of device files to link "74LS00" and other part numbers to it in the netlist. On the system I use, these are text files that also allow for selective swapping of pins and mapping of pin numbers to a different pin when inserted. | ||||
| Some ECAD systems come with pre-defined parts when you install them. I have found these parts are usually not sufficient for a commercial board, but may be a real time saver for educational projects or hobby projects. You need to look at a stock part carefully and decide if it is within your standards before you use it. | ||||
| Other information may be included within the pads, parts, or devices so they will interface with simulation and Electronic Computer-Aided Engineering (ECAE) systems. These are beyond the scope of this document, you will need to RTFM to find out more. | ||||
©1996 by George H. Patrick, III All Rights Reserved |
| Page design and content by George Patrick (gpatrick@aracnet.com). Last Modified: 08OCT96 |
![[*]](diamond.gif)