HW #2 - Eagle Tutorial The goal of this homework is to teach the - PDF document

ECE 477 Digital Systems Senior Design Project Rev 8/12 HW #2 - Eagle Tutorial The goal of this homework is to teach the user the basic steps of producing a switching power supply schematic and a printed circuit board using the Eagle Application. While tutorial in nature, it is by no means an exhaustive explanation of the application. Prior to beginning this it is recommended that you look at the Sparkfun Eagle tutorials located at http://www.sparkfun.com/tutorials/108. Eagle documentation and tutorials are also included in the application directory. The circuit you will duplicate is a switching power supply circuit using the National Semiconductor LM2675 Simple Switcher 1A step-down regulator which you may choose to use in your design. It comes in either fixed or adjustable modes and uses two popular outputs, 3.3 and 5 volts. Eagle Schematic Start the Eagle application. The Control Panel window will come up similar to the one shown below. Start a new project. Click File / New / Project. A file titled New Project will be set up as shown. Rename the file to Power Supply as shown. Right-click on the project you just created and select New / Schematic. Click File / Save As and name the schematic Power Supply. You should now see it listed in the project folder as Power Supply.sch. Creating a new library and parts Ideally all the parts you need would already be created so that assembling the parts into a logical schematic would be a matter of pulling them out of the existing libraries, placing, and connecting them together. However, you will most likely need to create a part at some point as is the case with the LM2675M. For this design we will use the schematic symbol shown on page 9 and the part layout as shown on page 24 of the pdf for our device. 1

ECE 477 Digital Systems Senior Design Project Rev 8/12 For this project we will create a new library and add a part to it. -At the Control Panel, click on the project folder, then right-click and select New / Library . -In the library window click File / Save As and name it Power Supply.lbr. Creating a new part consists of three steps: creating a schematic symbol, finding or creating the package for the printed circuit board, and linking the two together in a library. Creating the Schematic Symbol -In the Library window click Symbol , . In the New: textbox enter LM2675M and click the SYM button and click Yes to confirm. -Using the grid, you can use the Wire tool, , to draw a rectangle. Use the PIN tool, , to place the pins similar to the placement shown with the schematic symbol on page 9. Label the pins by selecting the NAME tool and using the nomenclature of the data sheet. Two more items to add to the schematic symbol are Name and Value tags which allow information to be added to the part by the user. Select the Text tool, , type ‘>NAME’ and ‘>VALUE’ and place them close to the part. The tags need to be placed on specific layers to be used appropriately, so click on the Change tool, , select Layer… , select the Names layer, click OK and click on the >NAME tag. The color of the tag should change to the color representing the layer. Do the same for the >VALUE tag. 2

ECE 477 Digital Systems Senior Design Project Rev 8/12 Save your schematic part. Creating the Package In the Library window click the Package tool, , name it SO-8/DIP and click Yes to confirm. From the recommended land pattern on page 26 of the data sheet: Note that the recommended pad size is .02 x .09 inches. If you click the SMD tool, , the SMD toolbar appears. This pad dimensions noted above will probably not appear in the Smd: dropdown, so click the Change tool, , select SMD / … and enter the new pad size, .02x.09 in the Change Smd box. You can now produce the recommended pattern based on the datasheet’s dimensions. Click the Name tool, , and number the pads as illustrated on the data sheet. 3

ECE 477 Digital Systems Senior Design Project Rev 8/12 It is a good idea to have some type of outline to indicate the outline of the device so that components are not placed too closely together, and this is not obvious from the pads. This is easily done with a silkscreen. Click on the Wire tool, , and set the layer to 21 tPlace, the silkscreen layer, Width and Style as shown. You may also need to modify the Grid, , setting to allow the silkscreen to be drawn in detail. Draw a silkscreen outline as similar to that shown below. Avoid drawing the silkscreen over the conductive pads where soldering may occur since this makes part placement and soldering more difficult. Add the >NAME and >VALUE tags to the package by clicking the Text tool, , typing ‘>NAME’ and ‘>VALUE’ and placing them close to the package. As with the schematic, the tags need to be placed on specific layers to be used appropriately, so click on the Change tool, , select Layer… , select the tNames layer, click OK and click on the >NAME tag. The color of the tag should change to the color representing the layer. Do the same for the >VALUE tag, using the tValues layer. 4

ECE 477 Digital Systems Senior Design Project Rev 8/12 Linking the Schematic Symbol to the Package Select the Device tool, , type LM2675M in the New textbox, click on the Dev button, click OK and then Yes to confirm . When the device window comes up click the Add button, , and select the schematic part. Place it in the work area. Click New in the Package area on the right of the window, select the SO-8 package created above and click OK . Click the Connect button to bring up the Connect window. Use the pdf datasheet page 2 to associate the package pins with the schematic symbol by clicking on the Pin Name, Pad name and clicking Connect until all the designated pins are connected. When complete, click OK . 5

ECE 477 Digital Systems Senior Design Project Rev 8/12 Click File / Save to save the part in the library. Close the Library editor. Creating a Schematic Duplicate the schematic for the switching power supply, shown below, from page 9 of the datasheet . Use the components provided to either find suitable devices in the standard libraries or create custom parts. Be sure to observe the notes related to the circuit layout . Libraries Eagle supports an extensive set of libraries of schematic and layout parts. These are subdivided by category and manufacturer. Finding the correct part is often by trial and error until you get familiar with how the parts are arranged. Schematics are usually bounded by a frame which is a standard form of documentation. To pick a frame, click Library / Use… and locate the Frames library. Click the Add tool, , and select the FRAME_A_L , which is the standard A-size paper in landscape. Now you should be able to place the newly created part in your schematic. On your schematic, click Library / Use… and go to the project directory where your Power Supply library is located. Select the library. Click the Add tool, , then select the library and part to add to the schematic. Place the part, then hit Esc button twice to get out of Add. Your schematic should now look similar to that below. 6

ECE 477 Digital Systems Senior Design Project Rev 8/12 At this point it would be a good idea to check and make sure your new component fits the package you have designed. This is easily done by clicking the Schematic/Board toggle button, , to bring up the printed circuit board window. Click on the crosshairs of the part and move it somewhere within the frame as shown. A LaserJet output is usually close enough to check by placing your part on the copy, so print off a 1:1 copy of the board and see if your part fits. The pads should extend beyond the pins of the device when it sits on the package as shown below. This simplifies heat transfer and solder flow during assembly. Return to the schematic page. 7