EasyEDA 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
After the simple introduction of EasyEDA, we are going to look at how to create a simple schematic in EasyEDA , 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.
Head to easyeda.com, 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.
Fill out your information and click Register.
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.
Feel free to keep it private (or not if you want to share it) and add a short description. Click OK.
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 . 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.
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.
We will be looking at the barrel jack’s datasheet for the dimensions we need. Click on Pad in the PCBLib Tools box.
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
Place 3 more pads with the following attributes:
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
In the layers box, click on the yellow box next to TopSilkLayerstrong text to edit the top silk screen. In the PCBLib Tools box, select Track.
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.
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
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.
Place two holes, and change their properties:
Hole(D): 1.6mm Center-X: 5mm Center-Y: 0mm Hole 2:
Hole(D): 1.8mm Center-X: 9.5mm Center-Y: 0mm
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.
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.
From the Drawing toolbox, select Rectangle.
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.
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.
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
Do the same for the rest of the pins.
Name: TIP Number: 1B Pin 3:
Name: DET Number: 2 Pin 4:
Name: SLV Number: 3
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.
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.
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