PCB Design Process and Fabrication Challenges

Transcription

1 PCB Design Process and Fabrication Challenges Nikola Zlatanov* Virtually every electronic product is constructed with one or more printed-circuit boards (PCBs). The PCBs hold the ICs and other components and implement the interconnections between them. PCBs are created in abundance for portable electronics, computers, and entertainment equipment. They are also made for test equipment, manufacturing, and spacecraft. Eventually, almost every EE must design a PCB, which is not something that is taught in school. Yet engineers, technicians, and even novice PCB designers can create high-quality PCBs for any and every purpose with confidence that the outcome will meet or exceed the objective. Also, these designs can be completed on schedule and within budget while meeting the design requirements. Designers just need to mind the essential documentation, design steps and strategies, and final checks. The Basic Design Process The ideal PCB design starts with the discovery that a PCB is needed and continues through the final production boards (Fig. 1). After determining why the PCB is needed, the product s final concept should be decided. The concept includes the design s features, the functions the PCB must have and perform, interconnection with other circuits, placement, and the approximate final dimensions. Fig. 1. The ideal PCB design flow begins when designers recognize a need that must be fulfilled, and it does not end until testing verifies that the design can meet those needs.

2 Ambient temperature range and concerns regarding the operating environment should be addressed and used to specify the materials selected for the PCB. Components and PCB materials must be selected to guarantee operation under all expected and potential forms of duress the board may be exposed to during its lifetime. The circuit schematic is drawn based on the concept. This detailed diagram shows the electrical implementation of each function of the PCB. With the schematic drawn, a realistic drawing of the final PCB dimensions should be completed with areas designated for each of the circuit s schematic blocks (groups of components closely connected for electrical reasons or constraints). Bill Of Materials Simultaneously with the schematic s creation, the bill of materials (BOM) should be generated. The components in the circuit should be selected by analyzing the maximum operating voltages and current levels of each node of the circuit while considering tolerance criteria. With electrically satisfactory components chosen, each component should be reconsidered based on availability, budget, and size. The BOM must be kept up-to-date with the schematic at all times. The BOM requires the quantity, reference designators, value (numeric value of ohms, farads, etc.), manufacturer part number, and PCB footprint for each component. These five requirements are critical because they define how many of each part are needed, explain identification and circuit locations while exactly describing each circuit element used for purchasing and substitution, and explain the size of each part for area estimations. Additional descriptions may be added, but it should be a condensed list describing each circuit element, and too much information can over-complicate library development and management. PCB Documentation The PCB s documents should include the hardware dimensional drawings, schematic, BOM, layout file, component placement file, assembly drawings and instructions, and Gerber file set. User guides also are useful but are not required. The Gerber file set is PCB jargon for the output files of the layout that are used by PCB manufacturers to create the PCB. A complete set of Gerber files includes output files generated from the board layout file: Silkscreen top and bottom Solder mask top and bottom All metal layers Paste mask top and bottom Component map (X-Y coordinates) Assembly drawing top and bottom Drill file Drill legend FAB outline (dimensions, special features) Netlist file The special features included in the FAB outline include but are not limited to notches, cutouts, bevels, back-filled vias-in-pad (used for BGA-type IC packages that have an array of pins under the device), blind/buried vias, surface finish and leveling, hole tolerances, layer count, and more. 1 Schematic Details Schematics control the project, so accuracy and completeness are critical for success. They include information that is necessary for the proper operation of the circuit. A schematic should include adequate design details, such as pin numbers, names, component values, and ratings (Fig. 2).

3 Fig. 2. Proper schematics, such as this one for the IDTP9021R wireless power receiver s buck regulator block, include pin numbers, names, component values, ratings, and other vital details. Embedded within each schematic symbol is the manufacturer part number used to determine price and specifications. The package specification determines the size of the footprint for each component. The first step should be to make sure the exposed copper for each pin is in the proper location and is slightly larger than the component pins (3 to 20 mils) depending on available area and soldering method. Consider assembly when designing footprints, and follow the manufacturer s recommended PCB footprint. Some components come in microscopic packages and do not allow room for extra copper. Even in these cases, a stripe of 2.5 to 3 mils of solder mask should be applied between every pin on the board. Follow the rule of 10. Small vias have a finished hole size of 10 mils with 10 additional mils of pad ring. Traces should be 10 mils or further from the edge of the board. Trace-to-trace pitch is 10 mils (5-mil airgap, 5-mil trace width, 1-oz copper). Vias with 40-mil diameter holes or larger should have a pad ring added for reliability. An additional 15 to 25 mils of clearance beyond the design rule should be instated for copper planes on outer layers from plane to pins. This reduces the risk of solder bridging at all solder points. Component Placement Component placement is next in the process and determined based on thermal management, function, and electrical noise considerations. A first-pass component placement step commences after the outline of component and interconnect position has been assigned. Immediately after the individual components are placed, a placement review should be held and adjustments made to facilitate routing and optimize performance. Placement and package sizes are often reconsidered and changes are made at this point based on size and cost. Components absorbing greater than 10 mw or conducting more than 10 ma should be considered powerful enough for additional thermal and electrical considerations. Sensitive signals should be shielded from noise sources with planes and be kept impedance-controlled. Power management components should utilize ground planes or power planes for heat flow. Make highcurrent connections according to the acceptable voltage drop for the connection. Layer transitions for high current paths should be made with two to four vias at each layer transition. Place multiple vias at layer transitions to increase reliability, reduce resistive and inductive losses, and improve thermal conductivity.

4 Thermal Issues The heat generated by the IC is transferred from the device to the copper layers of the PCB (Fig. 3). The ideal thermal design will result in the entire board being the same temperature. The copper thickness, number of layers, continuity of thermal paths, and board area will have a direct impact on the operating temperature of components. Fig. 3. IC thermal conduction can be achieved through the use of thermal vias and copper planes. To reduce operating temperatures easily, use more layers of solid ground or power planes connected directly to heat sources with multiple vias. Establishing effective heat and high-current routes will optimize heat transfer by means of convection. The use of thermally conductive planes to spread the heat evenly dramatically lowers the temperature by maximizing the area used for heat transfer to the atmosphere (Fig. 4). 2 Fig. 4. Effective heat spreading can distribute the heat uniformly from a heat source to all of the PCB s exposed surfaces.

5 With even heat distribution, the following formula can be used to estimate surface temperatures: P = (heat Convection) x area x (ΔT) where: P = power dissipated on the board Area = board (X axis x Y axis) ΔT = surface temperature ambient temperature Heat Convection = convection constant based on ambient conditions Fine-Tuning The Component Placement Components should be placed in the following order: connectors, power circuits, sensitive and precision circuits, critical circuit components, and then the rest. The schematic is built around each part on the PCB and completely interconnected. Routing priority for the circuit is chosen based on power levels, noise susceptibility, or generation and routing capability. In general, trace widths of 10 to 20 mils are used for traces carrying 10 to 20 ma and 5 to 8 mils for traces carrying less current than 10 ma. High frequency (greater than 3 MHz) and rapidly changing signals should be carefully considered when routed along with high-impedance nodes. The lead engineer/designer should review the layout, and physical locations and routing paths should be adjusted iteratively until the circuit is optimized for all design constraints. The number of layers depends on power levels and complexity. Add layers in pairs since the copper cladding is produced that way. The routing of power signals and planes, the grounding scheme, and the board s ability to be used as intended all influence operation. Final inspections should involve verification that sensitive nodes and circuits are properly shielded from noise sources, solder mask exists between pins and vias, and the silkscreen is clear and concise. When determining layer stack-up, use the first inner layer below the component sides as ground and assign power planes to other layers. Stack-ups are created in a manner that balances the board relative to the midpoint of the Z-axis. Consider any concerns the PCB designer has during the reviews, and correct the PCB based on feedback generated by the reviews. Create and verify lists of changes during each review iteration until the board is finalized. During all stages of the layout, keep the design error free by using the design rule checker (DRC). The DRC can only catch errors that it has been programmed to monitor, and DRC rule sets often change based on individual designs. At the minimum, the design rule checking should cover package-to-package spacing, unconnected nets (a unique name identifying each node of the circuit), shorted nets, air-gap violations, if vias are too close to solder pads, if vias are too close to each other, and vertical clearance violations. Many other important DRC rules can be set to ensure a robust design, and they should be researched and understood. For example, keep clearances at or above 5 mils. Vias should not be located within surface-mount pads (unless back-filled). And, solder mask should be between all solder points. Cost is often a driving influence behind PCB design, so it is good to understand the cost adders in PCB manufacturing. A typical board is two to four layers, with no drill holes less than 10 mils in diameter and 5-mil minimum air gaps and trace widths. It also should be in. thick with standard FR-4 and a copper foil weight of 1 oz. Additional layers, extra thick or thin boards, vias-in-pad, back-filled vias (nonconductive preferred due to conductivity limitations and thermal expansion differences), blind/buried vias, and lead time all substantially add to the overall cost. Manufacturer capabilities should be understood when the PCB design commences. PCB fabs are routinely contacted about capabilities and cost reduction techniques when designing PCBs for manufacturability.

6 Placing Components Generally, it is best to place parts only on the top side of the board. When placing components, make sure that the snap-to-grid is turned on. Usually, a value of for the snap grid is best for this job. First, place all the components that need to be in specific locations. This includes connectors, switches, LEDs, mounting holes, heat sinks or any other item that mounts to an external location. Give careful thought when placing component to minimize trace lengths. Put parts next to each other that connect to each other. Doing a good job here will make laying the traces much easier. Arrange ICs in only one or two orientations: up or down, and, right or left. Align each IC so that pin one is in the same place for each orientation, usually on the top or left sides. Position polarized parts (i.e. diodes, and electrolytic caps) with the positive leads all having the same orientation. Also, use a square pad to mark the positive leads of these components. You will save a lot of time by leaving generous space between ICs for traces. Frequently the beginner runs out of room when routing traces. Leave between ICs, for large ICs allow even more. Parts not found in the component library can be made by placing a series of individual pads and then grouping them together. Place one pad for each lead of the component. It is very important to measure the pin spacing and pin diameters as accurately as possible. Typically, dial or digital calipers are used for this job. After placing all the components, print out a copy of the layout. Place each component on top of the layout. Check to insure that you have allowed enough space for every part to rest without touching each other. Placing Power and Ground Traces After the components are placed, the next step is to lay the power and ground traces. It is essential when working with ICs to have solid power and ground lines, using wide traces that connect to common rails for each supply. It is very important to avoid snaking or daisy chaining the power lines from part-to-part. One common configuration is shown below. The bottom layer of the PC board includes a filled ground plane. Large traces feeding from a single rail are used for the positive supply.

7 Placing Signal Traces When placing traces, it is always a good practice to make them as short and direct as possible. Use vias (also called feed-through holes) to move signals from one layer to the other. A via is a pad with a plated-through hole. Generally, the best strategy is to lay out a board with vertical traces on one side and horizontal traces on the other. Add via where needed to connect a horizontal trace to a vertical trace on the opposite side. A good trace width for low current digital and analog signals is Traces that carry significant current should be wider than signal traces. The table below gives rough guidelines of how wide to make a trace for a given amount of current Amps Amps Amps Amps Amps Amps Amps When placing a trace, it is very important to think about the space between the trace and any adjacent traces or pads. You want to make sure that there is a minimum gap of between items, is better. Leaving less blank space runs the risk of a short developing in the board manufacturing process. It is also necessary to leave larger gaps when working with high voltage. When routing traces, it is best to have the snap-to-grid turned on. Setting the snap grid spacing to often works well. Changing to a value of can be helpful when trying to work as densely as possible. Turning off the snap feature may be necessary when connecting to parts that have unusual pin spacing. It is a common practice to restrict the direction that traces run to horizontal, vertical, or 45-degree angles. When placing narrow traces, or less, avoid sharp right angle turns. The problem here is that in the board manufacturing process, the outside corner can be etched a little narrower. The solution is to use two 45-degree bends with a short leg in between. It is a good idea to place text on the top layer of your board, such as a product or company name. Text on the top layer can be helpful to insure that there is no confusion as to which layer is which when the board is manufactured. Checking Your Work After all the traces are placed, it is best to double check the routing of every signal to verify that nothing is missing or incorrectly wired. Do this by running through your schematic, one wire at a time. Carefully follow the path of each trace on your PC layout to verify that it is the same as on your schematic. After each trace is confirmed, mark that signal on the schematic with a yellow highlighter. Inspect your layout, both top and bottom, to insure that the gap between every item (pad to pad, pad to trace, trace to trace) is or greater. Use the Pad Information tool to determine the diameters of pads that make up a component. Check for missing vias. ExpressPCB will automatically insert a via when changing layers as a series of traces are placed. Users often forget that via are not automatically inserted otherwise. For example, when beginning a new trace, a via is never inserted. An easy way to check for missing via is to first print the top layer, then print the bottom. Visually inspect each side for traces that do not connect to anything. When a missing via is found, insert one. Do this by clicking on the Pad in the side toolbar; select a via (0.056 round via is often a good choice) from the drop down listbox, and click on the layout where the via is missing. Check for traces that cross each other. This is easily done by inspecting a printout of each layer.

8 Metal components such as heat sinks, crystals, switches, batteries and connectors can cause shorts if they are placed over traces on the top layer. Inspect for these shorts by placing all the metal components on a printout of the top layer. Then look for traces that run below the metal components. Design Tools Criteria As time has progressed, technology has become more accessible. PCB design tools used to be priced so high that only companies could afford them. Today many PCB tools are available to the home user. Each tool has a different set of strengths and weaknesses, though there are some really standout tools that are either free, open-source, or relatively low-cost. Many of the freeware programs are a subset of a commercial code. Some may be skeptical about the usability and productivity of freeware, open-source, or low-cost programs. With regard to PCB tools, I have established a list of criteria that I find essential. Please note that freeware programs are often more polished than some open-source programs but will have limitations, such as number of components or pins allowed. Here is the minimum standard that I have set for PCB tools for my home use. Windows compatible: This is a must for me. Everyone has an opinion on this, but I find that I spend less time debugging programs in Windows than I do in any other operating system. Native schematic tool: Some programs require an external schematic editor. Even simple designs tend to change as you work through them. Some of the changes are as simple as changing an input pin on the microcontroller, but may also include adding circuitry to increase functionality. If the schematic editor is not tied to the rest of the software package, it is very easy for changes not to propagate into the final design. Footprint wizard: This is something that makes life much easier. PCB products without a footprint wizard have a tedious workflow. They direct you to find a product from the library that is somewhat similar and modify it. The problem with this workflow is that many new sensors are coming out with nonstandard footprints. Hacking something to fit your needs is tedious. It is much easier to start from scratch. With a good footprint wizard, you should be able to have a new part created in less than five minutes. Multilayer design capability: A two-layer board greatly simplifies routing, and most PCB prototyping houses offer this as their base option. 3D preview: Perhaps this is because of my mechanical background, but I find that this capability is underrated by many. With 3D preview, it is very easy to verify that all your parts will fit, and that you will have sufficient access to solder the parts. In my last project, I was able to use 3D preview to identify a problem very quickly with my connector spacing and correct it. This will serve as your final design check before manufacturing. Autorouter: Though many purists will argue that an autorouter is not desirable, I disagree. An autorouter helps find the best placement for components and can be used in an iterative method. I usually hand route any critical traces and then autoroute the remaining traces, followed by a final cleanup performed by hand. With care, an autorouter can be used to great advantage and can dramatically reduce the time spent in your design. Evaluating PCB layout tools As edge rates of logic devices become faster and PCB designs become more advanced and geared towards miniaturization, a number of issues and pitfalls can emerge at the layout stage if you do not have appropriate tools at your disposal to handle your requirements. In-depth experience using the various PCB layout tools available today is the best indicator of the direction to take regardless of densities, application, or speed requirements. Some design tool parameters that require some experience involve design speeds ranging from a few megahertz (MHz) to over 15 gigahertz (GHz) with board layer counts going from single layer to 50 layers, sometimes more. An experienced designer always works diligently with tighter constraints, and uses the more advanced manufacturing technologies paired the right layout tools.

9 From the perspective of the experienced PCB designer, compared to the ideal PCB layout tool, most current commercial tools lack key features and attributes: Gentle Learning Curve Intuitive GUI Routine Tasks Performed By Easy To remember Hotkeys Comprehensive Constraint Manager handling High-Speed Signal Integrity and Easy to Grapple Manageable File Structure Easy to Create and Manage Library Manager Intuitive 3D Visualization Engine Decent Auto-Routing capability Connect Seamlessly to Its Schematic Tool For Easier ECOs Allow Manageable Exports of Manufacturing Outputs Handle Large Number of Copper Shapes Allow Designer to Easily Manage Large Number of Layers Embedded CAM Engine That Follows CAD Tool s GUI Not Too Overpriced My ideal PCB layout tool Today s PCB layout tools have a combination of some of them, but no vendor has all of those capabilities embodied in one tool. Thus, no tool can be perfect. One can only choose the best tool that is most suitable for his/her needs. Since we are not at the ideal design scenario yet, we have to make do with today s available tool technologies. Among the most popular PCB layout tools today are Cadence Allegro, Mentor Graphics Pads, and Altium designer. Each has its own unique capabilities, advantages, caveats and limitations. Although you can use any of these three tools to design virtually every kind of board, it does not mean you should. Choosing the right tool for the layout should be at the forefront of PCB layout planning and must never be ignored. As an example, using Cadence Allegro to layout a single sided board with a few components will be counterproductive when you have tools like PADs and Altium Designer also at your disposal. Similarly, it is not advisable to design a high-speed board with edge rates in excess of 10 GHz on any tool other than Cadence Allegro. The three tools offer some sort of portability. Altium allows import of OrCAD schematic, Allegro board files, as well as Pads PCB database. Pads allows import of Altium board file. Allegro allows import of Pads Ascii file. Having said that, when one applies any sort of import, it is never a 100% clean transition from one CAD tool to another without tweaking the data to a certain extent and running design rule checkers (DRCs) and netlist checks on the schematic afterwards. Therefore the only time the designer would port the data is when the company is switching platforms. Cadence Allegro Allegro is one of the oldest and the most diversified tools in the industry. No one can question the power it gives to the designer to tweak every aspect of the layout. It also has one of the best constraints managers that give better control on signal and power integrity of the board. Fig. 5 below shows how detailed and comprehensive its constraint manager is.

10 Fig. 5. Allegro s Constraint manager at a glance. It is also the best tool to handle a large number of board layers. Ever since Cadence bought OrCAD, their developers have tried to integrate the two. Therefore, one will find that Cadence OrCAD for schematic capture is integrated to a certain extent with Allegro for layout. Fig. 6 below shows cross- Probing being done between Cadence OrCAD and Allegro. Fig 6. Cross-Probing done between Cadence OrCAD & Allegro. Allegro PCB SI and OrCAD Signal Explorer help to do a pre- and post-layout signal integrity analysis and are efficient at doing this for complex PCBs. Allegro also provides a much better integration to Allegro PCB router, formerly known as Cadence SPECCTRA, than any other layout tool. SPECCTRA is one of the most well-known products used for Auto-routing. However, Allegro is not without its drawbacks and limitations. Most importantly is its cost. A Cadence seat along with a suite that can handle almost all design needs can cost upwards of $90K. Spending this amount on a layout tool by a mid-sized company or start up OEMs does not seem plausible and would be the deciding factor for most. Secondly, Cadence tools are sometimes too complicated and cryptic to understand. The GUI is not intuitive or user friendly. Many functions are hidden deep within the tool and many easy tasks are difficult to carry out. Moreover, Allegro part libraries are difficult to create and maintain.

11 Thirdly, Cadence has a tortuous file structure that is awkward to manage. Generating outputs for manufacturing can become an arduous task in Allegro. As an example, PCB designer has to go through numerous steps in specific order to setup and generate drill files and Gerbers. Also, this tool is not effective at handling multiple copper fills for power and ground planes. Designers have to work diligently while dealing with static and dynamic shapes and suffice to say that handling numerous copper shapes in Allegro is not a walk in the park and can become too laborious for some. Finally, Cadence Allegro is notorious for the use of its scripts and macros to perform fairly basic tasks that could be performed fairly automatically in other layout tools. Mentor Graphics PADs The PADs platform, even though not as dated as Allegro, has been available for some time now. It is best suited for small to medium complexity boards. Hence, by 2005, PADs had become one of the most widely used platforms for PCB layout. It has its own schematic tools in DxDesigner and PADs logic, but can also work with OrCAD capture with some limitations. PADs Logic and DxDesigner are fairly integrated into the tool and easy to work with. PADs is known for its intuitive and easier to understand GUI. Fig. 7 below shows the PADs design rules window showing constraints setup of a particular net class. Notice how the options are comprehensible and straightforward. Even though it is still a hassle to learn PADs, once you get the hang of it, performing tasks is fairly quick and easy. Its hot keys enable the designer to perform tasks quite promptly. Fig. 7. Design Rules window with physical constraints setup based on a particular net class Library creation is much easier with PADs compared to Allegro. Part libraries are fairly easy to manage and maintain. One can find free part libraries online that are already built and time tested and vetted. The file structure is straightforward. Project outputs are uncomplicated to set up. HyperLynx from Mentor is also another resourceful tool that enables engineers to quickly and accurately analyze signal integrity at all stages of design life cycles and follows its intuitive GUI from PADs. HyperLynx thermal is another tool that that allows designers to analyze board level thermal problems by performing thermal simulations. Both of these tools provide excellent integration with PADs. PADs also comes with its own auto-router as an option. While it is not as powerful as its Cadence counterpart, it performs auto-routing of medium complexity with satisfactory results.

12 Like Cadence Allegro, PADs also has its disadvantages. First is its cost. Even though it is not as expensive as Cadence, one can end up paying tens of thousands of dollars for all its options. Secondly, it is not a very good tool in handling signal integrity issues. Its design rules system is too simple and inflexible to carry out tasks required on high-speed boards. As an example, it is not an option to import the Chip pin-delay information into the tool as can be done in Allegro. This information can be quite important when dealing with timing analysis of high-speed signals. Thirdly, PADs is not effective at handling large number of layers. Having numerous copper layers in PADs can make the database size hefty and can become a burden on system s resources. Altium Designer Altium Designer was created based on the idea of a unified electronics design system. It uses a single data model that holds all the design data to create a product. FPGA design, PCB design and layout, simulation, CAM tools, and embedded software development are all housed in one software system. Altium Designer is a decent PCB layout tool. The main advantage that it has over other tools is its cost. Due to its cost alone, it has taken over much of the PADs and Allegro market over the last few years. All the options are provided at one cost. Another plus that it has over other tools is its gentle learning curve. A designer who has used any of the other layout tools will not find it difficult to learn this relatively new tool. Thirdly, Altium's tool gives the PCB designer an almost perfect balance between its intuitive GUI and its powerful options facilitating the designer to have more control over the layout. Fig. 8 below shows how one can selectively modify characteristics of individual component pads. The schematic tool within the Altium designer is sync ed perfectly with the layout tool, which allows easier engineering change orders (ECOs) during the design process. Fig.8. Changing characteristics of individual component pads in Altium Designer.

13 Fourthly, creating a parts library for your project is easiest in Altium. The package includes thousands of already created and vetted parts from various manufacturers. Its library creating tools give the designer a comprehensive set of options that are fairly straightforward at the same time. One of its library creation utilities also allows creation of package symbols based on the IPC-7351 standard. It also allows the designer to incorporate 3D bodies into the layout by importing step models to an extent that was not possible with any of the other layout tools. The design community and mechanical engineers in particular favor this option. Detailed 3D drawings of the completed layout can be generated once the layout is finalized. Figure 5 below shows a 3D view of a completed board layout from within Altium designer. Fig. 9. 3D visualization engine of Altium Designer showing a completed board. Generating manufacturing outputs is very easy in Altium. Unlike other tools, output generation is not overly complicated and gives all the options that the designer would require. CAM tool is also provided with the Altium designer package, based on the CamCASTIC, which allows the designer to view the Gerber data. Finally, Altium recently bought Morfik Technology a provider of cloud-based software applications. Altium expects that cloud technology will pervade future electronics and embedded systems. Even though the technology has a lot of potential, it is yet to be seen how it will assist the board designer. Like other tools, Altium Designer also has its limitations. First and foremost are its limited capabilities for handling high-speed designs. The simulation tools that come with the package are not powerful enough to handle speeds above 2GHz. So designs that incorporate speeds in excess of 5GHz must be simulated in other tools like HyperLynx or AnSoft. A second drawback is its overly comprehensive query system, which is based on the query language. Even though it is a powerful system, the designer will have to write the queries to do simple tasks much of which is automatic in PADs. Finally, some tools that are incorporated into Altium Designer have been acquired from existing software, e.g. CAMCASTIC. The drawback of this approach is that its GUI is rather different with the layout tool, which can sometimes be frustrating to the designer. A better approach would have been to redesign the CAM tool such that the GUI and hotkeys were identical to the layout tool.

14 All type of boards can be designed by any of the layout tools. It is a question of preference, cost and the limitations of each tool. However, for every board, I am sure there will be a tool that best suits its complexity and requirements. Summary I spent significant time after college doing Schematic Capture and PCB Designs using different tools and even testing the new PCAD software on DOS and UNIX machines. Later, I moved onto better and more sophisticated tools like Altium Designed and Cadence Allegro. PCB design may be complex, but it is quite possible to design good boards with a little technique and practice. Using these guidelines and adding research when needed, seasoned veterans may continue honing their skills and novice designers may learn to create high-quality PCBs that exceed expectations. References [1] Cohen, Patricio, Concepts and terminology used in Printed Circuit Boards (PCB), Electrosoft Engineering, Web, May 25, [2] Mauney, Charles, Thermal Considerations for Surface Mount Layouts, Texas Instruments, Web, May 13, [3] David Lieby. The constraint Manager from a User Perspective. Web. 22 Oct [4] Wikipedia contributors. "Altium Designer." Wikipedia, the Free Encyclopedia. 14 Oct Web. 28 Oct [5] Gabe Moretti. Altium releases 3D PCB visualization. EE Times. 26 Nov Web. 25 Oct [6] A Guide to Low-Cost PCB Tools. Adam Carlson, Lead Engineer, GE Aviation 10/28/2013 [7] Advanced Design System ADS Software - Current Version [8] "PCB tools supporting ODB++". Artwork.com. Artwork Conversion Software Inc. Retrieved [9] "ODB++ Data Exchange". Mentor.com. Mentor Graphics. Archived from the original on Retrieved 25 September * Mr. Nikola Zlatanov spent over 20 years working in the Capital Semiconductor Equipment Industry. His work at Gasonics, Novellus, Lam and KLA-Tencor involved progressing electrical engineering and management roles in disruptive technologies. Nikola received his Undergraduate degree in Electrical Engineering and Computer Systems from Technical University, Sofia, Bulgaria and completed a Graduate Program in Engineering Management at Santa Clara University. He is currently consulting for Fortune 500 companies as well as Startup ventures in Silicon Valley, California.