Getting Started with EasyEDA Part 1: Create Schematic

**Introduction** [EasyEDA][1] is a free web-based electronic circuit design tool. It’s one stop design shop for your electronics projects, which offers schematic capture, spice simulation, PCB design and PCB order service. EasyEDA is designed to give electrical engineers, educators, engineering students and electronics hobbyists an Easier EDA Experience. More introduction about EasyEDA, you could check [https://easyeda.com/Doc/Tutorial/introduction.htm#Whats-EasyEDA][2] After the simple introduction of EasyEDA, we are going to look at how to create a simple schematic in [EasyEDA][3] , turn it into a PCB, and send out the design files to a PCB house for fabrication. We will do this in several parts–starting with part creation, then schematic capture, and PCB layout before sending out files for board fabrication. **Signing Up** Head to [easyeda.com][4], and click **Login** at the top of the page. While you can start without an account, being able to save projects to your account is quite useful. ![enter image description here][5] Fill out your information and click **Register**. **New Project** When you have logged in, click **New Project** at the top of the screen, and you will be presented with the main project screen. Click on **Create a new project** under the **Start** tab and give your project an appropriate name. In this tutorial, we will be creating a DC/DC converter using a simple linear regulator, so I’ll name mine “5V Power Supply. ![enter image description here][6] Feel free to keep it private (or not if you want to share it) and add a short description. Click **OK**. **Package Creation** Luckily, EasyEDA has a wide range of parts for us to use. We will base our design around the LM317 for DC/DC conversion, and we’ll put a barrel jack on the board so we can plug it into a wall outlet. Unfortunately, there is no barrel jack part or package in EasyEDA, so we’ll need to make one. We’ll base our design on the [PJ-002AH-SMT-TR from Digi-Key][7] . The first order of business is to create the package (footprint) for the part. Click on the **File** icon on the top of the window, and select **New**. Click on **PCB Lib**. ![enter image description here][8] You’ll notice that the units are in imperial, so we’ll change our canvas units. In the right-side pane, under **Canvas Attributes**, select **mm** from **Units**. ![enter image description here][9] We will be looking at the barrel [jack’s datasheet][10] for the dimensions we need. Click on **Pad** in the **PCBLib Tools** box. ![enter image description here][11] Click somewhere in the layout to drop the pad. Hit esc to stop placing pads. Click on the pad to edit its attributes. Change the following: Name: 1A Shape: Rectangle Layer: TopLayer (so it becomes a surface mount pad) Width: 2.8 (mm) Height: 2.4 Hole: 0 Center-X: 5 Center-Y: -5.7 ![enter image description here][12] Place 3 more pads with the following attributes: Pad 1B: Name: 1B Shape: Rectangle Layer: TopLayer (so it becomes a surface mount pad) Width: 2.8 (mm) Height: 2.4 Hole: 0 Center-X: 11.1 Center-Y: -5.7 Pad 2: Name: 2 Shape: Rectangle Layer: TopLayer (so it becomes a surface mount pad) Width: 2.8 (mm) Height: 2.4 Hole: 0 Center-X: 11.1 Center-Y: 5.7 Pad 3: Name: 3 Shape: Rectangle Layer: TopLayer (so it becomes a surface mount pad) Width: 2.8 (mm) Height: 2.4 Hole: 0 Center-X: 5 Center-Y: 5.7 ![enter image description here][13] In the layers box, click on the yellow box next to TopSilkLayer**strong text** to edit the top silk screen. In the **PCBLib Tools** box, select **Track**. ![enter image description here][14] Draw three separate, unconnected lines. We want to leave the front open so we can have some of the component hanging off the PCB. Right-click to end placement of the lines. ![enter image description here][15] Adjust the lines’ properties so that they make an open rectangle. Click on each one and change their attributes: Line 1: Start-X: 5mm Start-Y: -4mm End-X: 14.8mm End-Y: -4mm Line 2: Start-X: 14.8mm Start-Y: -4mm End-X: 14.8mm End-Y: 4mm Line 3: Start-X: 5mm Start-Y: 4mm End-X: 14.8mm End-Y: 4mm ![enter image description here][16] Finally, we need to add a couple of holes strong text for the part’s posts. Click on the **Hole** icon in the **PCBLib Tools** box. ![enter image description here][17] Place two holes, and change their properties: Hole 1: Hole(D): 1.6mm Center-X: 5mm Center-Y: 0mm Hole 2: Hole(D): 1.8mm Center-X: 9.5mm Center-Y: 0mm ![enter image description here][18] Click on the **File** icon, and select **Save As**. Give it a unique name, like PJ-002AH-SMT (manufacturer’s part name) and a short description, if you desire. ![enter image description here][19] Click **Save**. That’s it for package creation! **Schematic Part Creation** With the footprint complete, we need to create a schematic part. Click on the **File** icon, and select **New**. click on **Schematic Lib**. ![enter image description here][20] From the **Drawing** toolbox, select **Rectangle**. ![enter image description here][21] Click once at the origin (intersection of the two dark lines), move the mouse down and to the right, and click again to create a rectangle. This will be the body of the schematic symbol for our part. ![enter image description here][22] Click on the **Pin** icon, and click just outside the rectangle to create a pin. Move down a grid square and click. Repeat 2 more times for a total of 4 pins. Note that the pin’s connector (the circle at the end of the pin) should be facing away from the part body. ![enter image description here][23] Press **esc** to stop placing pins. Click on the first pin to highlight it. In the attributes panel on the right, change: Name: TIP Number: 1A ![enter image description here][24] Do the same for the rest of the pins. Pin 2: Name: TIP Number: 1B Pin 3: Name: DET Number: 2 Pin 4: Name: SLV Number: 3 ![enter image description here][25] Click outside the part so that you see **Canvas Attributes** and **Custom Attributes** in the right-side pane. In Custom Attributes, change **pre** to **J**?. Click on the **package** entry box (below the **pre** box) to bring up the package selector box. ![enter image description here][26] Under **User Package**, find the part we just made (**PJ-002AH-SMT**), select it, and click **Update**. Close the package selector box. Click the File icon, select **Save As**, and fill out the part information. I named my part “CON_BARREL_JACK” and gave it a short description. ![enter image description here][27] Click **Save**. We’re done with part creation, and tomorrow we’ll move on to schematic capture. A video will helpful to you by [https://easyeda.com/Doc/Tutorial/schematic.htm#Creating-The-Schematic][28] [Go to Part 2: Schematic Capture][29] [1]: https://easyeda.com/ [2]: https://easyeda.com/Doc/Tutorial/introduction.htm#Whats-EasyEDA [3]: https://easyeda.com/ [4]: https://easyeda.com/ [5]: /editor/20160406/5704dec8c33f1.png [6]: /editor/20160406/5704deffb687e.png [7]: http://www.digikey.com/product-detail/en/cui-inc/PJ-002AH-SMT-TR/CP-002AHPJCT-ND/669692 [8]: /editor/20160406/5704df299c60f.png [9]: /editor/20160406/5704df3d6c6ef.png [10]: http://www.cui.com/product/resource/pj-002ah-smt.pdf [11]: /editor/20160406/5704df9bdc24f.png [12]: /editor/20160406/5704dfb87d39b.png [13]: /editor/20160406/5704dfee81458.png [14]: /editor/20160406/5704e00119504.png [15]: /editor/20160406/5704e034c170c.png [16]: /editor/20160406/5704e0544419e.png [17]: /editor/20160406/5704e07627ef6.png [18]: /editor/20160406/5704e0997e6c8.png [19]: /editor/20160406/5704e0adbf724.png [20]: /editor/20160406/5704e0f78725d.png [21]: /editor/20160406/5704e11bbb3ed.png [22]: /editor/20160406/5704e1322b631.png [23]: /editor/20160406/5704e14d0ed64.png [24]: /editor/20160406/5704e16a31108.png [25]: /editor/20160406/5704e184ec037.png [26]: /editor/20160406/5704e1ad5b5f0.png [27]: /editor/20160406/5704e1cdf0fe4.png [28]: https://easyeda.com/Doc/Tutorial/schematic.htm#Creating-The-Schematic [29]: https://beta.easyeda.com/feather/Getting_Started_with_EasyEDA_Part_2_Schematic_Capture-GuoFzRL3l