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).
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. Use the hotkey
TAB to change the track width.
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. And you can right-click the point and delete it.
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.
9. If you want to create the solder mask for the track, you can use “Create Solder Mask” when you select the track on the right-hand panel. The solder mask will bigger 4mil than the track.
10. And if you want to create the slot hole, you can route a track, and then right-click the “Convert to NPTH” menu.
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. Or right-click delete the node.
When you routing a track on the signal layer, you will see an outline around the first track, it is the DRC outline, the clearance from outline to the track edge depends on your Design Rule(DRC) clearance setting.
When the PCB comes from the schematic converted, the “Routing Conflict - Block” will be opened automatically.
At the right-hand attributes panel - others, you can find a “Routing Conflict” option:
- Ignore: You can route the track overlap the different net name objects.
- Block: If the track net name different with other objects, your track will be blocked when routing.
- Walk Around: under developing
- Push: under developing
EasyEDA provide a easy experience for the differential pair routing.
Via: Topbar - Route - Differential Pair Routing
You must make sure the Differential Pair net names must be
XXX_N, XXX_P or
and you need to set Differential Pair net rule at the “Topbar - Tool - Design Rule” first.
How to route Differential Pair:
1.Set the Differential Pair net name as
XXX_N, XXX_P or
XXX+,XXX-, and set the rule for the Differential Pair net at the “Design Rule”
2.Click the menu
Topbar - Route - Differential Pair Routing
3.Click the one pad of the Differential Pair
You can tunning your track very easy on the editor.
Via: Topbar - Route - Track length Tuning
How to use:
1.Select the track which is you want to tune
2.Click the menu:
Topbar - Route - Track length Tunning
3.Set the parameter, start
4.Left-Click the track where is you want to start, and then move the mouse
5.When the track length close your setting, it will stop tunning.
For some simple or prototype PCBs, you may want to use the auto router function to save time. Layout is a time costly and dull job. EasyEDA spends lots of time to provide such a feature and it is loved by our users.
Before using the auto router, you need to set the board outline for the PCB.
1 Click the the auto router button from the topbar “Topbar > Route > Auto Router”
2 Config the auto router
After you click that button, you will get a config dialog like in the image below.
In the config dialog, you can set some rules to make the auto router result professional. These rule must equalize or more than DRC setting.
- Unit: The unit follows PCB canvas unit.
- Track width: The auto-route track width.
- Clearance: The clearance of the objects.
- Via Diameter/Via Drill Diameter: The via placing by auto-router.
- Realtime Display: when you select it , the real time routing status will show on.
- Router Server:
- Cloud: Using EasyEDA online server.
- Local: Using the local auto router server, when you click the Auto Router icon, the editor will check the local router server available or not automatically. How to use please see as below.
Router Layers: If you want to route inner layer, you have to enable the inner layer first.
Special Nets: For the power supply track, you may want it to be bigger, so you can add some special rules.
Skip Nets: If you like to keep the a net with no route, you can skip it. For example, if you want to use copper area to connect
GNDnet, you can skip the
GNDnet. If you want to reserve the routed track, you need to select the
Skip Routed Nets.
3 Run it
After click the “Run” button , The real time check box will let you see how it is going, but it will make the process a little bit slow.
Waiting for a few minutes, after adding bottom and top copper area, you will get a finished PCB board.
EasyEDA suggest that using local auto router rather than using the cloud server, because when many users using cloud server, the cloud auto router will fail. Only support 64bit system.
For the local auto router, please follow the steps as below:
1.Download the local auto router server.
- Windows7(x64) or later 64bit Windows
- Ubuntu17.04(x64) or other 64bit Linux
2.Unzip it to the User folder, such as driver D.
3.Configure the browser.
Notice: Please use the latest Chrome or Firefox !!!
The Chrome Browser don’t need to be configure, If the local auto router is unavailable, you have to upgrade Chrome to version 60.0.3112.78 or later.
- 1.Type “about:config” into the address bar then press enter.
- 2.Search and double click the options as below (change the values to “true”):
- 3.Re-open Firefox.
4.Open the decompress folder, Start local Auto Router:
- Double click
sh lin64.shon command terminal in Linux. Open the terminal, use the
cdcommand to change the directory to the
lin64.shlocation, and type
sh lin64.sh, then enter.
sh mac64.shon command prompt in MacOS. Open the terminal, use the
cdcommand to change the directory to the
mac64.shlocation, and type
sh mac64.sh, then enter.
- Double click
5.Open the editor, open the PCB, Click the Auto Router icon at editor to start auto-router.
If the local router server is available, the dialog will tell you. Click the Run button, the dialog will show the process.
Sometimes, if you can’t get it done, try the tips below.
- Make sure PCB rule doesn’t have 3 decimal places, EasyEDA only support 2 decimal places.
- Skip the GND nets, add copper area to GND net.
- Use small tracks and small clearance, but make sure the value is more than 6mil.
- Route some key tracks manually before auto routing and ignore them when auto routing.
- Add more layers, 4 layers or 6 layers. That will make the PCB more expensive.
- Change the components layout, make them have more space between each other.
- Don’t make any via/pad/solid region overlap the different net objects.
- Use local auto router rather than cloud server.
- Tell the error detail to us and download and send your PCB file as EasyEDA Source json file:
to [email protected].
Some professional people don’t like the auto router, because they think auto router is not professional, but you can use the auto router to check your placement to check the density of your PCB.
At present, the auto router is not good enough, suggest routing manually, we will improve it in the future.