utorial In Practical Circuit Board Design Ben LeVesque ECE480 eam 3 November 9 th, 2007 Keywords Circuit board, Cadence, Layout, Capture, post processing, trace capacity, trace ampacity, Via Abstract his document explores the creation of a circuit board from the initial creation of a schematic to the final post processing of CAD files while covering a breadth of information that a first time circuit board designer needs to know. hese practical issues range from the selection of a board house to on board heatsink design with recommendations for the first time designer that are usually obtained through experience. 1 Introduction/Objective Engineering schooling tends to focus on the concepts and theories needed to create circuits, but how do we get those bread boarded circuits from the lab and onto a circuit board? he obvious place to start is with the tutorials for whatever CAD package you plan to use in order to learn the software, but these software tutorials do not cover the design issues that arise during the design of a circuit board. he goal of this application note is not to be a tutorial for any particular software package, but as a guide to what is needed to obtain a successful design the first time. In order to achieve these goals we will be exploring the creation of a simple circuit board that contains transistor drivers and a connector. he purpose of this circuit is to drive low power valves and a heater coil in an oven. he design of this circuit will be done in Cadence s Orcad Capture CIS 10.1 and Orcad Layout Plus 10.1 with the assumption that the reader has done the tutorials for this software.
2 Creation of Design 2.1 Capture Figure 1: Schematic of example circuitry he first step in the creation of a circuit board is to create the schematic of the circuit that you plan to make a circuit board for. his is done in Cadence s Capture program. If parts cannot be found in the local library or online database during the schematic capture process, symbols must be created for them. Creation of new device symbols is covered in Cadence s tutorials. he above example circuit is made up of parts obtained through the local and online databases, while the connector is a uncommon part that a symbol had to be created for. 2.2 Selecting a board house he next step to the creation of a circuit board is to select a manufacture to create the circuit board once your design is done. he following criteria should be used when selecting a board house
1) Capabilities a. olerances b. Copper thickness c. Solder mask d. Silk screening e. Number of layers 2) urn around time 3) Documentation (ease of use of service) 4) Cost It is important to select a board house at this time because the capabilities of the board house may define the tolerances of the boards design. olerances are important to ensure that the board house can make features small enough for the design. he thickness of the copper on the board defines how much current the traces of the board can carry and is covered later in this document. So if a design contains high current traces a board vendor who can create boards with thicker traces maybe desirable. If a solder mask and silk screen are desired then a board house that has these capabilities must be selected. Likewise, if a board with many layers is needed, then the board house must be capable of this as well. he example design is very simple in nature. It does not contain any very high current signals or tight tolerances, but does require a silk screen and solder mask. Because of the short time frame of the example project a very fast turn around time is required, and since this is our first design good documentation on how to use the board houses services is required. With these criteria, PCBepress.com is selected for this project. heir service is very well documented and automated so they are able to achieve quick two day turn around times at a low cost. 2.2.1 Drill Sizes Board houses typically do not have all sizes of drill bits, so all holes on the circuit board must be of the sizes that the board house you send your design to has. his information is typically available on the company s website. Some specify hole size before the circuit boards are platted, while others specify the size of the hole after it is plated. he platting process provides a conductive path through all holes on the circuit board and as such it adds a small amount of material to the inner diameter of the holes. It is important to be aware of this difference as it is desirable to have components fit snuggly in their holes because this makes it much easier to assemble the boards and reduces the amount of solder needed to place the component. o meet this requirement it is often necessary to go through the foot prints of all through-hole devices in a design and change the drill sizes to sizes that a board house has.
Our sample design requires several holes in two different sizes to be drilled for the connector. We had to create this part, so at the time it s creation we used holes of the proper size according to PCBexpress s website. 2.3 Layout Once all drill sizes have been corrected in all the devices foot prints, the layout process can begin. When the netlist from Capture is imported into Layout you will be forced to link each symbol from your schematic to a physical package for Layout. Once all the packages are linked you will be presented with a window like the one below in which the yellow lines between devices represent connections from the schematic created in Capture. Figure 2: Initial layout of parts he first step as the Cadence tutorial suggests is to create a board outline. Create an outline that fits your final required dimensions or if you are just trying to make the device as small as possible create an outline with some extra room. We will follow the creation of a device of the smallest size possible. he next step is to place your components with special consideration of the yellow lines that indicate connections. Keep in mind that you may be able to be swap pins on certain devices such as micro controllers and connectors to achieve a better layout. A better layout is one that keeps short signal paths directly back to a common ground point, short signal lengths and keeps the
number of vias required to a minimum. It is also desirable to keep devices that create large amounts of heat away from one another, and high current switching signals away from sensitive low level signals and parts. Figure 3: Initial board outline and placement of devices 2.4 race sizes While laying out the circuit board it is important to know how much current is flowing in each trace. he traces on a circuit board have capacitance, inductance, and resistance. he effects of capacitance and inductance are a large area of discussion beyond the scope of this application note, but should be considered by the designer if high speed circuitry is involved in the design. he effects of resistance are more important for the low speed application covered here. When current passes through a trace a voltage drop occurs which results in thermal dissipation. With this in mind the trace must be sized so that it does not get too hot or so it does not introduce too much voltage drop for proper circuit operation. he following table gives a conservative guide on how to size traces according to temperature increase. here are several online calculators for achieving these values and voltage drops in the reference section of this application note. It is suggested to use either this table or the online calculators as the equations that define these properties are too complex for the level of discussion in this document.
emp Rise 10 C 20 C 30 C Copper 1/2 oz. 1 oz. 2 oz. 1/2 oz. 1 oz. 2 oz. 1/2 oz. 1 oz. 2 oz. race Width Maximum Current (Amps).010.5 1.0 1.4 0.6 1.2 1.6.7 1.5 2.2.015.7 1.2 1.6 0.8 1.3 2.4 1.0 1.6 3.0.020.7 1.3 2.1 1.0 1.7 3.0 1.2 2.4 3.6.025.9 1.7 2.5 1.2 2.2 3.3 1.5 2.8 4.0.030 1.1 1.9 3.0 1.4 2.5 4.0 1.7 3.2 5.0.050 1.5 2.6 4.0 2.0 3.6 6.0 2.6 4.4 7.3.075 2.0 3.5 5.7 2.8 4.5 7.8 3.5 6.0 10.0.100 2.6 4.2 6.9 3.5 6.0 9.9 4.3 7.5 12.5.200 4.2 7.0 11.5 6.0 10.0 16.0 7.5 13.0 20.5.250 5.0 8.3 12.3 7.2 12.3 20.0 9.0 15.0 24.5 Figure 4: race Ampacity Military Standard 275 [1] For the example board a current carrying capacity of 7.5 Amps at an ambient temperature of 85 Celsius is desired, voltage drop is not a concern. he board house selected only carries one once copper plated boards so a trace width of 0.1 is required to keep the trace temperature under its maximum of 130 Celsius for the traces that carry a power signal. he signals in the design are of low current and are not critical, so a smaller trace size of 0.020 is selected for them. 2.5 Heatsinking A circuit board can be used as a heatsink to dissipate power from surface mount devices. he thermal resistance of the circuit board is largely dependent on the amount of copper on the surface of the board that is directly connected to the device. It is also dependent on the ambient temperature, overall size of the circuit board, and the presence of other thermally dissipative devices in close proximity
on the board. A very large amount of modeling can go into determining heat flow and temperature rise of a given circuit board layout, but typically it is done through the concepts of thermal resistance. hermal resistance is a value that is typically listed in a datasheet or derived experimentally in the units of degrees of temperature increase per watt of power dissipation. Figure 5: hermal resistance & Max Power Dissipation vs. P.C.B. Copper Area DPAK package [4] j B P * R a a d P * R d j a j c P P d _ max d _ max a a R R J _ max j c B _ max j c Junction emperature j Ambient emperature a P Power Dissipated R d j a R j c hermal Resistance, junction to ambient hermal Resistance, junction to case here are two considerations that must be made while selecting how much area a heat sink should have during the layout process. Both the maximum junction and board temperature must be within allowable ranges. he maximum junction temperature allowable by a device is typically listed in its datasheet while
the maximum board temperature must be obtained from your board house. As a general rule standard FR-4 circuit board material has a maximum repeatable temperature of 130 Celsius before it breaks down. With the equations above and a graph like to one above it is possible to select the proper amount of copper area on the circuit board for worse case thermal dissipation. Our example requires that a 150watt oven can be driven with 24volts continuously. An On Semiconductor N-channel mosfet was selected for this task. Specifications R 0.008 Ω DSon _ max 150w ( )^2 * RDSon _ max 312. 5mW 24V R 50 Minimum pad size (only enough copper area to mount component) j j a _ max B _ max 150 Celsius 130 Celsius a _ max 85 Celsius j 85 0.3125*50 100.6 Celsius he junction temperature of the device is much less than the board constraint of 130 Celsius and the device constrain of 150 Celsius so no additional copper area is required to heat sink the device. It should be noted that the traces used to connect the device to the rest of the circuit will serve to provide some additional heat sinking so the actual operating temperature of the device will be much less. With heat sinking requirements and trace sizes determined the actual routing of traces can begin. Start with the critical traces such as grounds, and power signals that must be kept as short as possible.
Figure 6: Critical length power signals routed 2.6 Vias Often it is necessary for a signal to go from one side of the board to the other. his can be done at the through hole lead of a device or through a via. A via is a hole that is drilled in the circuit that is plated all the way through with metal. his creates a connection from one layer to the layer on the other side of the board. A via s current capacity depends on the diameter of the via, the thickness of the plating, and whether the via is filled with solder. If the circuit requires that a significant amount of current be put through a via, analysis should be done to ensure that there is not potential for failure at the via. Such analysis is beyond the scope of this applications note, so it is assumed that only low current signals are passed through via s. In the case of the example, there are no possible direct paths from all of the resistors to the connector. So the signal must be passed to the other side of the board by passing it through a via. Also because the via is a drilled feature we had to select a via of a diameter that our board house could drill.
Figure 7: hree via s were required to route all signals to the connector With the remainder of the layout complete, the board s dimensions are pulled in to minimize the size of the board. Also if screw hole mounts or silk screen labels are needed, this is the time to add them. 2.7 Post Processing Once the circuit board layout is complete it must be converted to file formats that a board house can work with. Some board houses accept saved files from certain programs, while most require files in Extended Gerber RS-274X file format. hese files must be exported from Layout using the post processor. his process is straight forward and covered in Cadence s tutorials, but care is required in reviewing the board house s required file names and formats. It is highly recommended to use a Gerber file viewer such as the free version of ViewMate from pentalogix.com to view generated Gerber files to ensure that they are correct. Any flaw in these files will show up in the final circuit board. 3 Recommendations 3.1 Drawing Schematic If your schematic is very large or complicated, use multiple pages for your schematics in Capture with each page broken down into the segments of your circuit. his makes it much easier to read your schematics and go back to them
later. o link wires from page to page you want to use an off-page connector from the place drop down menu. 3.2 Auto-routing vs. Manual routing Most layout packages include some sort of auto trace router. Some are very complex and are very powerful. However, it is not recommended to use these auto-routers when you make your first design. he auto-routers tend to be very complicated to use and often do not do as good of a job as manually placing parts and traces with some thought. hose who do PCB layout for a living largely do it manually because a person can typically do a much better job of laying out parts than a machine because a person is much more in tune with compromises that can be made in the design to achieve a good layout. It is worth noting that auto-routers can be useful for quick and dirty layout or for quickly doing small sections of a board at time. 4 Conclusion Circuit board design like all areas of design requires experience to become good at it. his document should provide all the information the first time designer needs to create a working product when the board comes back from the board house. Circuit board design can be very tricky and complicated so it is suggested to start with a simple design for your first layout. References - for further information 1 race Ampacity Military Standard 275 http://www.dscc.dla.mil/downloads/milspec/docs/mil-sd-275/std275.pdf 2 Online trace ampacity calculator http://circuitcalculator.com/wordpress/2006/01/31/pcb-trace-width-calculator/ 4 hermal resistance of a DPAK package http://www.st.com/stonline/products/families/power_management/support/therma l/pdf/dppak.pdf 5 Via current capcaities http://www.ultracad.com/articles/viacurrents.pdf