PCB tools provide many function to fulfill your PCB design requirement.
Such as: Track, Pad, Via, Text, Arc, Circle, Move, Hole, Image, Canvas Origin, Connect Pad to Pad, Copper Area, Solid Region, Measure/Dimension, Rect, Group/Ungroup. etc.
In the schematic editor, we use Wire or the
W Hotkey to connect Pins, in a similar way in the PCB editor, we use Track to connect Pads. Track allows you to draw PCB tracks and can be found on the PCB Tools palette or using the
W Hotkey (not T: see above!).
Some Tips about Track.
1. Single click to start drawing a track. Single click again to pin the track to the canvas and continue on from that point. Right click to end a track. Double right-click to exit track mode.
2. Drawing a track at the same time as using a hotkey(for example hotkey
B) for changing the active layer will automatically insert a Via:
If you start drawing a track on the top layer - you will see it drawn in red - then press the B key to change to bottom layer and you will see EasyEDA insert a grey via and then the track will continue being drawn but now on the bottom layer in blue.
3. Pressing the
- Hotkeys when drawing the track will change the width of the track on the fly.
4. Double clicking on a drawn section of the track will add a new vertex at that point. You can drag the vertex to form a new corner.
5. Click to select the track and then Click and Drag on a segment of the track to adjust the segment between vertices.
6. Pressing the
L Hotkey when drawing the track will change the track’s Route Angle on the fly. And you can change Route Angle on the Canvas Attributes of the right panel before the next drawing.
7. You can change inflection direction when routing, just press
8. If you want to route a track and use “L”, and the then press “+”, you will get two different size track segment.
When a track is selected, you can find its Length attribute in the right panel.
Delete a Segment from a Track
In lots of other EDA tools, the track is segment line, but in EasyEDA, the track is polyline. Sometimes, if we want to delete a segment, we must delete the whole track and route again. Now we provide a better way to do this. Move your mouse to the segment which you want to delete, click it, then hold
SHIFT and double click it. the segment will be removed.
The more information of routing, please refer at PCB: Route Tracks
You can add pads using the Pads button from the PCBLib Tools palette or using the
After selecting one of the pads, you can view and adjust its attributes in the right hand Properties panel.
Number: Remembering the pin numbers you set in the schematic symbol in your Schematic Lib: to connect those schematic symbol pins to the pads in your PCB footprint, the pad numbers you set here in the PCB Lib footprint must be the same.
Shape: Round , Rectangular , Oval and Polygon.
EasyEDA supports four shapes:
OVALPAD will give your more space.
POLYGONPAD will let you to create some strange pad.
Like in the image below, you can edit the PADs points when you select a
Layer: If the pads are part of a SMD footprint, you can set it to Top layer or Bottom layer. For through hole components you should set it to Multi-Layer.
Net: You don’t need to enter anything here because at present this footprint is not connected to anything in a circuit.
Width and Height: When the shape is set to Round, Width will equal Height.
Rotation: Here you can set the Pad’s rotation as you want.
Hole(D): This is the drill hole diameter for a through hole pad. For a SMD Pad, set this to zero.
Center-X and Center-Y: using these two attributes, you can set the pad’s position with more precision, compared to using the mouse.
Plated： Yes or No.
When you want to lay a multilayer PCB, you need to add Vias for nets getting through layer and layer.
Place a Via On a Track
When placing a
via on a track, the track will be cut to two segments. Placing two vias on a tracks, you will get three segments, then you can change one segment to other layer id, or remove one of them.
- EasyEDA only support the through via for all layers, doesn’t support the Buried hole/via.
if you need Japanese or Korean you can use Google Noto fonts
Select the text, then you can find a Font-family attribute on the right panel like in the image below.
Click the add button, then choose the font, the font file must be
So you can add any fonts by yourself. EasyEDA doesn’t cache the font on our server, so if you close the editor, you need to add the font again by yourself.
Note: If you use the other font, the
LineWidth attribute is useless, because it will be automatically set by changing the
You can draw many Arcs with different sizes, it’s easy to create a pretty cool PCB as you like.
EasyEDA provides two Arc tools:
- Start point fixed, you can change the end point position and radius.
- Center point fixed, you can change the radius.
You can draw a circle in PCB , but it can only be drawn at SilkLayer and Document Layer. If you want to draw a circle at TopLayer or BottomLayer, please use Arc.
This option is same as schematic’s drag.
There were lots of users that didn’t know how to use PAD or VIA as a HOLE, they asked EasyEDA for help, so EasyEDA added a HOLE TOOL in the PCB toolbar.
On PCB and PCB Lib editor, there is a nice feature on the PCB Tools bar.
After clicking on the image icon, you will see the Insert Image window as below.
In this dialog, you can choose your favorite image, EasyEDA support
SVG. Unlike some other EDA tools which only support a Monochrome Bitmap image, EasyEDA supports full color, but Monochrome Bitmap is welcome.
You can adjust the color tolerance, simplify level and reset the image size there.
And you can select shape invert.
The image will be inserted to the active layer, if it is not right, you can change the attribute. Such as TopSilkLayer.
This option is the same as schematic’s Canvas Origin.
We provide a protractor for PCB tools.
When creating a PCB without a Schematic, none of the pads on the Footprints have nets connecting them so there will be no ratlines.
Rather than try to track the pads from scratch, it is a good idea to connect them up by hand first using
Connect Pad to Pad from the PCB Tools palette. This will help you to remember to track the pads correctly with fewer mistakes.
You could also do this by setting net names for all the pads: if the two pads are given the same net name then EasyEDA will understand that they are connected together and will automatically create a ratline between them.
Or you can set these two pads with the same net name at the right panel Pad Properties after you click the pad.
This tool only works for footprint’s pad, the single pad you placed in the PCB can’t be connected by this tool.
Sometimes you will want to fill in or flood an area with copper. Usually this copper area will be connected to a net such as GND or a supply rail. You can draw the outline of a flood using the Copper Area button from the PCB Tools palette.
When selecting a copper area, you can find its attributes from the right hand Properties panels.
Layer: Bottom, Top, Inner1, Inner2, Inner3, Inner4;
Net: the net that the copper area is connected to;
Clearance: clearance of the copper area from other nets and floods;
Pad Connection: direct or spoke (i.e. a cross shaped heat shunt);
Keep Island: Yes/No. This keeps or removes any isolated areas of copper created as part of the flooding process. It is usually good practice to removes these unless you really need them to maintain a more even spread of copper (copper balance) on your PCB.
Fill Style: No/Filled. Selecting No will removes the fill so that you can see the tracks more clearly;
After drawing the copper area, set the net it is to be connected to (floating copper areas are not recommended because they can cause EMC and Signal Integrity (SI) problems).
Lastly, don’t forget to click the button Rebuild Copper Area to rebuild the flood.
Shift+Bto build all of the copper areas.
Shift+Mto clear all of the copper areas.
- If you after copper pour but no copper show up, you need to set it a net same one of the PCB nets, or keep the island as YES, and the rebuild the copper area via “Rebuild Copper Area” button or “SHIFT+B”.
- If you want to hide the copper area and keep routing tracks, you can set the copper zone invisible at the right-hand panel.
EasyEDA does’t support inner copper pour or copper overlap now, but we will support that in the future, if you want to pour the inner area, please use Solid Region.
EasyEDA has added a new tool Solid Region for PCB design
This is a very useful, quick way to connect Pads. You can draw a Solid Region to include all of these pads with same net name, then set the region to the same net name as the pads. It is like Copper Area but easier to use for small areas. To use Solid Region like this, set the Type attribute (in the right hand Properties panel) to Solid.
The Solid Region can also be used to create a cutout in a copper area.
If you have a copper area but need an area inside it to not be filled then you can draw a Solid Region and set the Type attribute (in the right hand Properties panel) to Cutout , then this area will be free of copper, as shown in the image below:
Lastly, by setting the Type attribute (in the right hand Properties panel) to NPTH(Non Plated Through Hole), Solid Region can be used to create a Non Plated Through Hole of an arbitrary shape.
When the Gerber files are generated, an area defined by a Solid Region set to a Type NPTH in the PCB editor will create an area defined to be a NPTH hole and you can see it in the PCB photo view as below:
Making and adding measurements is useful in PCB design. EasyEDA provides two methods to do this.
Dimension tool in the PCB Tools palette:
This tool can show three units on the canvas, milliliter, inch and millimeter.
When you click one side of the dimension on the PCB, you can drag it for any directions or change its length.
Measure a distance using M Hotkey: press M, Or Via: Super menu > Miscellaneous > Measure Distance, then click the two points which you would like to measure.
Note: This method will display the distance units which is the canvas’ units.
It looks like a Solid Region, but it can’t be set Nets and you can’t set the Layer as NTPH.
Just like Group/Ungroup in the Schematic Editor can be used to create a schematic lib symbol, you can use Group/Ungroup from the PCB Tools palette to create a PCB Lib footprint in the PCB editor.
For example, place Tracks and Pads on the canvas, then select all of them and click Group/Ungroup to group them like in the image below: