EasyEDA User feather
feather
Public Project: 531 Footprint Package: 0 Likes: 0 Favorites: 0 Views: 2835

Getting Started with EasyEDA Part 1: Create Schematic Public

2 years ago  
blogCreate SchematicCircuit Design

Introduction

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.

Signing Up

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.

enter image description here

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

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 . 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

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

We will be looking at the barrel jack’s datasheet for the dimensions we need. Click on Pad in the PCBLib Tools box.

enter image description here

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

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

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.

enter image description here

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

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

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

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

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

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

From the Drawing toolbox, select Rectangle.

enter image description here

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

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

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

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

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

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

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

Go to Part 2: Schematic Capture

Comments

Add Comment
你现在访问的是EasyEDA海外版,不推荐使用,我们已经建立访问速度更快的中国区数据中心 https://LCEDA.cn
如果你已经有EasyEDA账号,请使用谷歌浏览器访问 https://easyeda.com/applyForLceda 进行数据迁移到中国区数据中心。
有问题联系QQ 3001956291 不再提醒