EasyEDA PCB Software Review

I evaluated EasyEDA Designer (v6.4.20.6 July 6, 2021 on Mac OS 10.11) to design a simple but complete (SPICE simulation, parts, mounting holes, annotations) through-hole, one-sided PCB to illuminate an LED.

EasyEDA Designer is a proprietary program, but free to use (they make money by selling parts and PCB fab services online.) It is an Electron (Javascript) application. (If you have battery usage problems, close EasyEDA Designer, then restart it.)

Summary

The initial learning curve was moderately difficult, as any EDA software has the first time, but is very easy for the second PCB. I was able to accomplish exactly what I wanted. Both the Online and Desktop Clients require an Internet connection, so if that is an issue, try KiCad.

I used EasyEDA Designer on Mac OS 10.11, so it should work on any version of Mac OS, and the UI has a Mac-friendly UI with menus and shortcut keys.

EasyEDA works conceptually the same as KiCad, so it’s a good stepping stone.

Read the “Usage Tips” and “EasyEDA/LTspice Notes” below to save at least an hour when designing your first PCB!


EasyEDA 3D View
3D View of PCB created with EasyEDA Designer illustrating annotations, fiducials (pick and place registration dots), copper pour, plated grounding hole and mounting holes

Review and Notes

There are 3 EasyEDA product types:

  1. Online Editor (browser)
  2. Desktop Client (download), but is still a browser app that’s tied to the cloud
  3. local install (call for pricing.)

I used #2, expecting to use it locally, but a login and cloud connection is needed for Spice and likely other features.

The purpose of EasyEDA is:

– simple UI for creating PCBs
– upload your PCB artwork to their site to purchase services (parts or board fab.)

The workflow to create a PCB is conceptually identical to KiCad:

– New … Project
– (origin is automatically set to 0, 0)
– schematic capture (insert your electronic symbols from libraries. The symbols need Spice models if you plan to simulate.)
– simulate with LTspice (shows voltage (V) and current (I) over time per component)
– convert to PCB components (pick actual parts from the parts libraries)
– click on canvas, then set units to mm or inches, and snap size to 0.050″ or 1 mm and enable it
– inspect 2D or 3D views (provides assurance that the actual PCB resembles what you expected)
– move PCB to (0, 0)
– create any copper areas (pours/ground planes)
– export to Gerber (for sending to CAM machines.)

So learning one product allows you to understand the other, although the menus and keys will be different.

EasyEDA Features

EasyEDA has every feature that a hobbyist would need. This is not surprising, since they offer PCB fab services, so their EDA software literally has to function.

– very intuitive commands via mouse menus or shortcut keys. Click on Setting … Shortcut Keys to view or change shortcuts. Also has Help and Tutorial systems.
– has Panelize menu (in KiCad you must use the external KiKit program), but the panel looks odd in 2D and 3D views.
– has a very convenient dedicated Place … Hole menu for (drilled) board mounting holes
– has a built-in fiducials (alignment markers) feature with Shift+F for pick and place machines
– commercially-maintained components libraries
– set of video tutorials on Youtube.

EasyEDA Limitations and Problems

– requires Internet connection for LTspice and possibly other operations
– 3D view often renders a blank page, requiring closing and re-opening the worksheets
– no blind vias
– it’s unlikely that EasyEDA Designer has similar non-hobbyist high-frequency features as Altium. This includes “creepage” features, etc.

EasyEDA/LTspice Notes

– your schematic must use Spice library components (models), including a voltage source and GND. The EELib parts library does not include Spice models, so will not work for simulation
– not sure why the LTspice V/I graphs disappeared at some point, now I just see a text report that says “succeeded”
– Regardless of EDA software, it’s always recommended to do your Spice modelling on small subsystems, one at a time, to limit the complexity of each circuit.
– requires Internet connection for LTspice and possibly other operations

3D View Notes

– make solder masks invisible to see the traces
– image not as high-resolution as KiCad, but looks ok (see sample above.)

Usage Tips

These tips will save you at least an hour when making your first design, and are easy to remember:

– the default origin is (0, 0), which you don’t need to change for EasyEDA’s fab service. To change the origin, you need to use the EasyEDA API.
– the Start tab has a UI with various options. An important one is a button with
“Change to Simulation Mode” or “Change to Standard Mode”. (You need to be in Standard Mode for PCB layout.)
– click anywhere on the grid for the snap size setting. (I use 1 mm or 0.050 inches.)
– use Edit … Name Position to position annotations below board components (default is above for some reason)
– use right-click on Projects window to delete old project files
– use Shift+F to insert fiducials for pick and place machines. They should be 1 – 3 mm in diameter, and usually round. You can delete the annotation “U1” above, an usse with copy and snap to grid to make 3 fiducials at various corners of the board.
– View … Zoom … Fit in Window or K is the fastest way to scroll the screen to the origin, otherwise you have to use the left and right keys.
– has a very convenient dedicated Place … Hole menu for (drilled) board mounting holes.
– Place … Circle or C is rarely what you want, since it’s just an annotation graphic. Use the pads P, vias V, holes or fiducials Shift+F features instead.
– 3D view often renders a blank page, requiring closing and re-opening the worksheets
– isolation slots (relatively long cutout regions into the board) can be made with various pads or holes, just insert the component, select oval shape and define the oval dimensions. (Isolation slots are often used in various power supply circuits to provide air-gapping for high-frequency or high-current applications.)
– copper areas (pours) can be edited after pouring by clicking precisely on the edge of the pour. This will display the CopperArea Attributes dialog. Also, try the Tools … Copper Area Manager. You can click on the canvas and enable/disable display of copper areas.
– traces can be very wide in EasyEDA, so often copper area pours aren’t needed. For example, I have made traces 50 mm wide.

EasyEDA API

– Javascript scripts are run from the scripts window under Advanced … Extensions
API Documentation
Forum: API script editor and debugger
Github Shapes Example
User Extensions for EasyEDA Summary
easyeda-ibom-extension (Interactive HTML BOM Tool)

(Note that some experienced engineers avoid EDA scripts in general because the API can change over time without warning, causing problems with existing documents.)

Differences with KiCad

– EasyEDA has a dialog for round PCB corners, while KiCad users usually import a DXF file
– EasyEDA has copper area/pour integration, while KiCad users usually configure zones.
– EasyEDA has a very large, commercially-supported components library, while KiCad is more user-supported.
– KiCad has global labels as shorthand for schematic wires
– KiCad uses tilde ~ for “not”, try # in EasyEDA. See forum post.

Resources

Getting To Blinky 4.0 – LTspice simulation
What are the differences between solder mask and paste mask?

Re: What is paste mask?

A stainless steel template in a tightened frame, with holes corresponding to landpatterns on the bare board that are either cut, punched, or drilled with a laser. The solder stencil is used at the beginning of the circuit assembly process where it is placed on top of a bare board, solder paste is pushed through the holes, then the stencil is lifted away. This leaves small solder paste deposits on the bare board, onto which components are placed.

This entry was posted in API Programming, Cloud, CNC, kicad, Tech. Bookmark the permalink.

Leave a Reply

Your email address will not be published.

This site uses Akismet to reduce spam. Learn how your comment data is processed.