CADSOFT EAGLE TUTORIAL

Transcription

1 CADSOFT EAGLE TUTORIAL IEEE OPS By Shubham Gandhi, Kamal Kajouke 1

2 Table of Contents 1. Introduction 1.1 Getting Started 1.2 Eagle Schematic Editor 1.3 The Toolbar and Command Bar 1.4 Importing Libraries 2. Schematic Capture 2.1 Adding Parts 2.2 Connecting the Parts 2.3 Nets 2.4 Naming and Values 2.5 Electrical Rule Check (ERC Tool) 3. PCB Layout 3.1 Creating a Layout From Schematic 3.2 The Ground and Power Planes 3.3 Airwires and Routing 3.4 Applying the Finishing Touches 3.5 Design Rule Check (DRC Tool) 4. Project Submission 4.1 Cam Processor 4.2 Submitting the Files 2

3 1. Introduction CadSoft EAGLE is a moderately powerful tool used for capturing schematics and laying out PCBs. Although it is capable of producing professional designs, EAGLE has a large hobbyist following because of its freeware version. This guide is meant to help you familiarize yourselves with creating schematics and PCBs in EAGLE. It will cover basic tools and navigation in the schematic editor, creating traces in PCB layout, and generating the gerber files used in fabrication. 1.1 Getting Started When you start Eagle, you will see a screen split into two columns with a directory structure on the left and information about Eagle on the right. We first need to create a new project and this can be done by going to File -> New -> Project as shown in Figure 1. Figure 1. Eagle start up Name the project something along the lines of IR_Sensor. There should be a green dot next to the name indicating that it is active. To create a new schematic within the project, go to File -> New -> Schematic. 3

4 1.2 Eagle Schematic Editor A schematic editor window similar to the one below should have appeared. Figure 2. Eagle Schematic Editor On the left is the toolbar, and the large white space is where you design the schematic. Right above the design space is the command bar where you can type in commands to access different tools (as opposed to clicking on them in the toolbar). Above the command bar are various action buttons (open, save, zoom, etc.). 4

5 1.3 The Toolbar and Command Bar Figure 4. Command bar The command bar can be used to type in commands that are used to access tools. For example, if you type move and press <Enter>, the Move tool will be selected. Even mo will select the Move tool. You may find it more convenient Figure 3. Toolbar The toolbar contains many useful tools, some of which this tutorial will cover. 5

6 1.4 Importing Libraries The parts libraries that are bundled with Eagle are often not added by default. Simply go Library -> Use. Figure 3. Adding libraries That should open up the lbr folder in your installation folder. Select all the libraries (Ctrl+A) and hit open. It may take a few seconds to add all of them. Figure 4. Selecting all libraries 6

7 2. Schematic Capture Here we will create a schematic for an IR sensor using a pair of IR emitters and detectors. 2.1 Adding Parts The first thing you want to do is to start adding parts into your design window. Click the add parts button ( ) to get to the parts that you just imported.. (Or type in add or ad into the command bar). Figure 5. Library list of parts A list of libraries will open up that literally contains tens of thousands of parts. We re going to be using 5. Many of these libraries contain subfolders with parts as well. The search bar will help us narrow down and find what we re looking for. 7

8 Lets go ahead and add in an LED into our schematic (it will be our IR emitter since they are IR LEDs technically). Search for *led*. We include * in our query to search for anything that has the string led as part of the name, not just the string by itself. Figure 6. Searching for led 8

9 Scroll down to the led library, and within this library there is subfolder called led. In this folder, we are going to select the LED5MM part. Figure 7. Select part LED5MM Note, in the upper right of Figure 7, we are shown what the part will appear as on the schematic and on the board layout. Double click the part, or click OK with it selected. Do not click Drop as that will remove the library from the list. Figure 8. Adding a part to the design space 9

10 Add it somewhere in the middle for now. You can press escape to go back to the parts list. Next, we ll add the IR detector (IR phototransistor). Search for photo transistor, this time without *. Select the part BPX81, since it most closely represents what we want. Figure 9. Selecting the IR detector (phototransistor) Add it next to the LED. Figure 10. Adding the phototransistor You can use the Move Tool ( ) to move misplaced parts, and the Delete Tool ( ) to delete any incorrect parts. 10

11 Next, we will add two resistors. Search resistor, and under the rcl library, open the subfolder R-US_ and select the part R-US_0204/7. Place two of them in the schematic as shown in Figure 11. Note that you can right click to rotate parts when placing. Figure 11. Place the resistors Then, we will add a capacitor. Search for capacitor, and under the rcl library, open the subfolder C-US and select the part C X050. Figure 12. Place the capacitor Finally, we will add a 3-pin header. Search for pin header, and under the pinhead library, open the PINHD-1X3 subfolder and select the part PINHD-1X3. Figure 13. Place the header 11

12 There are two additional things we need to add. These aren t quite parts, but nets for 5 volts and ground. Nets are covered in Section 2.3. Search for supply and under the supply1 subfolder, and add +5V and GND as shown in Figure 14.. Figure 14. Adding 5V and GND This is a good point to save. Hit Ctrl+S and make sure to save it in the project folder. Figure 15. Saving the schematic. 12

13 2.2 Connecting the Parts After laying out parts, we want to connect them.. Use the Net Tool ( ), not the Wire Tool ( ), to make connections between components. To keep the schematic neat, use only right angled nets ( ). Note, you will notice there two floating nets. They are intentional, we will address them in the next section. Figure 16. Connecting components 2.3 Nets Nets are essentially a node in a schematic. The highlighted portion below, and all the components connected to it form the +5V net, for example. Figure 17. The +5V net 13

14 We can make a connection between floating nets by naming them, or connecting them to the same net. Use the Name Tool ( ), to name both floating nets out. Figure 18. Naming a net Do the same with the other floating net. You will get a warning similar to Connect N$7 and OUT? Click yes, as this is what we want. Then, use the Label Tool ( ), to label the the connections so we know both of the seemingly floating nets are the same net.. Figure 19. Labeling the net 14

15 2.4 Naming and Values The schematic is almost complete. All that is left to do is give a name and value to the components using the Name Tool ( ) and Value Tool ( ). Figure 20. Naming components, and giving them values The value for R1 was omitted since it will vary depending on design constraints. The phototransistor already had a value of BPX81 which was removed, to make it more generic. 15

16 2.5 Electrical Rule Check (ERC Tool) The schematic is complete, but as a final measure, it needs to be check for errors. Eagle provides an ERC tool ( ) that will check any electrical errors such as floating nets or pins, and consistency errors between schematic and layout (when we get to it). Figure 21. Using the ERC Tool This final schematic section should be taken with a grain of salt because the results vary with application, and even errors can be ignored at times. 16

17 3. PCB Layout Now that our schematic is complete and error free, the next step is to design the circuit board. 3.1 Creating a Layout From Schematic Click the Generate/Switch to Board Tool ( layout. ) in the top left corner to generate a new Figure 22. Generate/switch to board You will be asked to create a new one from schematic. Click yes, as this is what want. A new window similar to that in Figure 23 should open up. Figure 23. Board layout window 17

18 There are a few things to point out here. Many of the tools in the toolbox are different, all the parts that we added in the schematic are in a jumbled pile on the bottom left, and the board outline is huge. You can zoom in and out of the board by scrolling. If you have a wheel-click mouse, clicking and holding the wheel will allow you to pan. We will be shrinking the board size to 1 square inch and turning on the grid to allow us to systematically place the components. Click the Grid icon ( ) in the top left, turn the Display to On, and hit OK. This will display a grid that the board outline and components will snap to. Figure 24. Grid turned on Note, below the Grid Icon, the coordinates of the cursor location are displayed as the mouse is moved. Figure 25. Coordinates of cursor displayed 18

19 Another note, if you zoom into the corner of the board outline, you will notice that it is not snapped to the grid. Using the Move Tool ( ), Ctrl+Click the corner to snap it to the grid. Figure 26. Board corner not snapped to grid Next, we want to resize the board outline so that it encapsulates 1 square inch. 1 by 1 will do. Use the Move Tool ( ) again to click the corners to resize the board to 1 by 1 Figure 27. Board resized to 1 by 1 Note that crosshair at the bottom left corner of the board represents coordinates (0,0). Now we are ready to place the components inside the outline. For our layout to function as a distance sensor, we will want to place the IR LED and phototransistor next to each other. The pin header connectors will need to be at the bottom of the board as they will be plugged into a breadboard. The resistors and capacitors can be placed anywhere on the board. You can right click to rotate components. 19

20 Figure 28. Placing the components 3.2 The Ground and Power Planes Printed circuit boards can contain many layers of copper: 4, or 8, or even 128. We are designing a simple board with 2 layers. The top layer will be designated as the power (+5V) plane, and the bottom layer will be the ground (GND). These layers will allow any component connected to power or ground to connect directly to the the planes. Grab the Polygon Tool ( ) and select the top layer as shown in FIgure 29. Figure 29. Select the Top layer 20

21 Use the tool to outline the board. When completed, it will appear as a red dotted line. Figure 30. Draw the power plane Next, using the Name Tool ( ), name the polygon you just created to +5V. This tells Eagle to connect this plane to the +5V net. Figure 31. Name the polygon to +5V to create a power plane 21

22 Repeat this process for bottom layer, but name it GND. Figure 32. Create the GND plane Now when you click the Ratsnest tool ( ), Eagle will flood the planes with their designated nets, and some of the component pads will be connected to the planes. Figure 33. Flooded planes 22

23 3.3 Airwires and Routing As you may have guessed already, the yellow airwires wires indicate unrouted connections. Use the Route Tool ( ) to finish up the rest of the traces by making electrical connections indicated by the airwires. You can route on both the top and/or bottom layers, and if any overlaps on the same layer occur, use a Via ( ) to weave between layers. A via will allow you to switch between layers in a trace. For neatness, use only 135 degree angles ( Do not use the autorouter ( ). ) in your traces. Figure 34. Routing Use the Ratsnest tool ( ) after each routed trace to see its effect. If a trace needs to be removed, the delete tool will not work. Instead, use the Ripup Tool ( ). You have a functional distance sensor once you have routed the rest of the traces. 23

24 3.4 Applying the Finishing Touches The board is nearly ready for production. It just needs to be polished a little more. Use the Smash Tool ( ) to click on each of the components. A new crosshair will appear for each name and value associated with the components. This will allow us to move the text around so that it looks cleaner. Remember, things can be rotated by right clicking when they are selected. They can also be snapped to the grid by Ctrl+clicking them. Figure 35. Smashing components and rearranging the text The part that we will be using for the IR phototransistor is actually much bigger than what is indicated on the board. We can simply draw a 5mm diameter circle around the part to indicate its actual size. Use the Circle Tool ( circle that is 0.2 inches (~5mm) in diameter. ) with the tplace layer selected, and draw a Figure 36. Drawing a circle around the phototransistor 24

25 Finally, we need to sign the design (like an artist signs his or her work), and maybe something that describes what the board is. Use the Text Tool ( board of varying sizes, and you are finished with the board. ) to add text to the Figure 37. Adding Text to the board 25

26 3.5 Design Rule Check (DRC Tool) The final step in the design process is checking for errors. When you are done routing, run the DRC Tool ( ) with the default settings. It will check for things such as overlapping traces in the same layer, traces that are too close to the edge or other traces, and double check size constraints on all vias and pads among other things. Figure 38. DRC Tool, run with default settings If any errors are returned, you must go back and fix them and run the check again. Figure 39. DRC giving errors 26

27 4. Project Submission This final section will guide you through the submission process, and how we will get them manufactured. We will generate Gerber files, a set of files associated with the layers on the board. 4.1 CAM Processor First we need to download the.cam file that will generate the correct gerber files for us from the following link: Browse to your Eagle installation folder and place this file in the cam folder with the other cam files. Click on the Cam Processor ( ) in the upper left in the layout window, and go File -> Open -> Job and select LaenPCBOrder.cam. 27

28 Once it loads, click Process Job. This will generate a separate file within your project folder for each layer in the board. Open up to the folder (usually Documents/eagle/ ), and zip up the following files: boardname.toplayer.ger boardname.bottomlayer.ger boardname.topsoldermask.ger boardname.bottomsoldermask.ger boardname.topsilkscreen.ger boardname.bottomsilkscreen.ger boardname.boardoutline.ger boardname.xln Drills boardname.sch Schematic boardname.brd Board 4.2 Submitting the Files us your Gerber files and we will review them and get back to you if anything needs to be fixed. Name the zip file firstname_lastname_irsensor.zip. This is due by 4/17, and this deadline is absolutely enforced because there will be a batch order for manufacturing. Late submissions will not receive PCBs! 28