If you have hidden your tools , you can open them from here:
Top toolbar View > Wiring Tools…

Note: All of the commands in Wiring Tools are electronics related. Don’t use a wire when you just need to draw a line, shape or an arrow: use Drawing Tools instead.


There are three ways to enter the wire mode in EasyEDA.

  1. Click the Wire button from the Wiring Tools palette.
  2. Press the W hotkey.
  3. Click on the end of a component pin (where the grey pin dot appears if you select the component):

EasyEDA automatically enters Wire mode.

Here is a screenshot of the Astable Multivibrator LED project schematic after wiring:

Moving Components And Wires:

If you place a component, such as a resistor, on top of a wire then the wire breaks and reconnects to the ends of the component.

When moving selected components using the mouse, they will drag attached wires with them (“rubber band”) to some extent but please be aware that the rubber banding feature has some limitations. When moving selected components most wire will move vertically and horizontally. Using the arrow keys will not rubber band. Selected wires do not rubber band.

A selected wire can be moved directly by clicking on it using the mouse or by the arrow keys. If a wire is selected by clicking on it using the mouse then green grab handles will appear at the ends and vertices.

Auto adjust connection

If you put a resistor or capacitor on a wire, the wire will auto connect the pins as below:

When you want to wiring a series of resistors which are in a row, you can just wire through them, and then you will find they all be connected.


When you design a professional schematic, perhaps it will use a lot of wires. If you wiring one by one, much time would be wasted, and then you need to use Bus.

Bus Entry

If you decide to wire with Bus , the Bus Entry must connect to Bus and other nets with wires. such as in the above image.
The “Bus” and “Bus Entry” just for the indication, because when you place Bus and Bus Entry, you have to place the netlabel on the Bus Entry dot point.

Net Label

NetLabel can be used to give your wires names to help you find them and identify any misconnections. You can find the NetLabel from the Wiring Tools palette or by using the N hotkey. When selecting the netlabel, you will find its attributes in the right hand Properties panel:

You can change its name and colour. If you only want to change its name, it may be easier to just double click the netlabel.

Multi-NetLabels in One Wire

EasyEDA support mutil-netlabel in one wire now.

When you convert the schematic to the PCB, the editor will choose the first netlabel you placed as the net name for this wire, as below NETLABEL1.

As above image, when you click anyone netlabel’s name in the design manager, the wire will be highlighted.


  • If wire 1 has 3 netlabels A B and C, and wire 2 has netlabel A, then wire 1 and wire 2 are the same net.
  • Netlabel/Netflag/Netport/volprobe only support English characters and letters, and Arabic numerals.
  • If a part prefix is P1, which has two pins, it will have two nets “P1_1” and “P1_2” by default, if you place a netlabel named P1_1 at other wire which is not connect with P1 pin1, the default “P1_1” will change to “P1_1(1)” for avoid the wrong connection with netlabel “P1_1”.

Net Flag

NetFlag is the same as NetLabel, you can find the NetFlag from the Wiring Tools palette or using the Ctrl+G hotkeys for GND or Ctrl+Q for VCC. You can also change its name, for example from VCC to VDD:

The screenshot below is after adding NetLabels

  • indicated by the little egg marks
    -and a GND NetFlag

This schematic is almost finished.

Wiring Tools palette provides NetFlag: Digital GND, Analog GND, VCC and +5V for your convenience.

Net Port

At EasyEDA, Net Port works like Net Label, it doesn’t differentiate the input and output net port. When you don’t want to route too many wires, how about trying Net Port :

It will make your schematic look more clean, and you just need to set each Net Port a net name.

No Connect Flag

You can find the NO Connect Flag via wiring tool,


In the below schematic, if you don’t add a NO Connect Flag, there is an error flag in the nets collection of the design manager.

After adding a NO Connect Flag, the error disappears.

Note: NO Connect Flag only works on the symbol’s pin directly.

Voltage Probe

EasyEDA provides a simulation feature for the schematic. After the simulation is running, you will see the waveform where you placed the voltage probes in the circuit.

For more detail about the simulation, please check the Simulation section.


When you create a new symbol in schematic and schematic lib, you must use Pin to create pins for the new symbol, otherwise your symbol can’t be wired with wires.

For more information please refer to the Schematic Lib: Pin section.


On the Wiring Tools palette there is the Group/Ungroup Symbol… button.

Just like the Symbol Wizard, this tool is also for you to quickly create schematic library symbols.

Using the Symbol Wizard you can only create generic symbols but how can you quickly and easily create symbols like these?

Here’s how.

EasyEDA allows you to do something that very few other EAD tools support.

Using the P Hotkey, you are allowed to add a PIN directly onto the Schematic canvas. So you can add 8 Pins, draw a rectangle from the Drawing Tools palette and add 555 as text to form a symbol for the NE555 like the one shown below:

Now comes the clever bit.

Up to this point you have a collection of separate pins, a drawn rectangle and some text that are all separate items with no particular association with each other.

So now select all of the items and click the Group/Ungroup Symbol… button. A dialog will be opened:

After you click OK, all those separate elements will be grouped together to form your new symbol directly in the schematic.

Using the group function, you can create any symbol in the schematic, easily and quickly.

How cool is that?

So what does Ungroup do? Try selecting a symbol and then click the Group/ungroup command to see what happens!


  • The pin numbers and names cannot be moved independently of the pin.
  • The symbol you created in the schematic will not be save in the personal libraries, if you want to use it repeatly, please create a schematicLib.

If it’s still difficult to understand, don’t worry, you can see the process in the dynamic image below: