Lesson 5: Routing the PCB
Adding Fanouts
Within PADS Professional Layout, go to: File ► Open.
Navigate to C:\PADS_Professional_QuickStart\Lesson 5 - Routing the PCB\PCB\LED_Flasher.pcb, select the file named LED_Flasher.PCB, and click Open.
In the bottom left corner of your screen, click on the “Net Explorer” tab to activate the “Net Explorer” panel. If the Net Explorer tab is not available Go to: Route ► Net Explorer. Then drag and drop the Net Explorer panel onto the Component Explorer to tabulate them.
Within the Net Explorer panel, select the PWR Net Class and notice that all objects assigned the DGND and VCC nets are highlighted on your board.
Go to: Route ► Fanout Patterns, ensure the settings are as shown, then click “Fanout Selected”.
Click “OK” to dismiss the Fanout report, then click close to exit the Fanout Patterns window.
You can group your components by creating the appropriate class type. Then select the class and run the Fanout command.
Single route
Next, let’s route the connection between Pad 8 of component U1 and Pad 1 of R1.
Left click once in the empty black space to clear any selection filter.
Zoom into U1.
Go to: Route ► Add Routes ► Plow (or Press CTRL+Q) to launch single trace routing.
Left click once on Pad 8 of U1, move your cursor down, then click on Pad 1 of R1 to complete the trace.
Press the Escape key twice to terminate the route command.
Left click once in the empty black space to clear the filter.
When the route command is active, right-click to access a drop down menu to
change trace width, routing layer, routing modes, and more. Interactive route tuning tools are available from the route menu.
Sketch Route
Sketch Route allows you to select a set of nets, draw a sketch path, then let the routing engine route the selected nets based on the user defined path.
In the bottom left panel area, click the Net Explorer tab.
Within Net Explorer, under LED_Flasher > Planning Groups > User Groups click the LEDS group to select all LED nets (Alternatively, draw a selection rectangle across the LED1-6 ratsnests directly in the PCB workspace).
Click Draw Sketch on the bottom toolbar area (Or press F8 key). Then left click once to start drawing the sketch path and once again to stop drawing.
Click Sketch Route (Or press F9 key).
Allow the route engine to route the traces.
Save your work.
Defining Internal Plane layers and nets
Go to: Planes ► Plane Assignments.
Within the Plane Assignments window, under the Layer Usage column for Layer 2, click on the keyword Signal and select Plane.
Click the dotted box next to “Layer 2” table entry, then assign it the DGND net as shown below.
Check the radio button to automatically add Pullbacks, then set the Plane Data State to Dynamic.
Repeat steps 2-4 to define Layer 3 as a Plane layer assigned to the VCC net.
Click “OK” to apply your changes and dismiss the Plane Assignment window.
Go to: View ►Fit Board (Or Press CTRL + B).
You should have results similar to the image show below.
Add Layer Stackup Table
Go to: Place ► Layer Stackup.
Click OK.
Left click to place the Layer Stackup table as shown below.
View Board in 3D
Click the 2:3D View document tab to see a 3D rendering of your board.
Go to: File ► Close, Click “Yes” to save your changes.
While in 3D mode, you can also place parts including multi-body mechanical
assemblies (such as product enclosures and mounting brackets). Live DRC rules can
be customized to enforce desired placement behavior.
Up Next: Lesson 6 - Creating Fabrication and Assembly Files