Lesson 2: Placing and Wiring Parts
Searching for and placing parts on your schematic sheet.
If not already open, launch PADS Designer and go to: File ► Open ► Project
Navigate to C:\PADS_Professional_QuickStart\Lesson 2 - Placing and Wiring parts\LED_Flasher.prj, select the file named LED_Flasher.PRJ and click Open.
Within the Navigator panel, Double-click the Design sheet to view its contents.
Within the Search panel search box, and click the Library - Parts tab along the bottom. Type: "NE555" and press Enter to see the NE555DR component as shown below (you may need to click once on the search result to see the part’s symbol and footprint).
Drag and drop the NE555 part from the search area onto the Design sheet (try to
position your symbols as shown in images to facilitate the wiring process).
From the My Parts panel, scroll to locate the Special Component named Source_VCC.1.
Drag and drop Source_VCC.1 onto the Design sheet.
Repeat Step 7 to add a second Source_VCC.1 component to your schematic (Or hold down the CTRL key while dragging the same symbol).
Wiring your schematic
Follow the steps in the image below to wire your Power components (The two VCC symbols) to the NE555.
Click the Net icon on the top toolbar area (or Press lowercase n key) to activate the wiring tool.
After your mouse cursor turns into a crosshair, Left-click and hold on Pin 6 (THRES) of the NE555 symbol.
Then, move your mouse cursor 2 grid steps to the left and press the Spacebar.
While still holding down the left mouse button, move your mouse cursor down 4 grid spaces and press the Spacebar again.
Finally, move your mouse cursor onto the bottom pin of R8 and release you left mouse button.
Press the Escape key to cancel the command.
You should end up with a wire similar to the one shown below.
Catching and fixing potential wiring mistakes
Go to: Tools ► Verify.
In the Verify window, click the “OK” button.
The DRC panel will appear, displaying a list of potential electrical issue.
Click on the last error message in the DRC panel to see the unconnected pin in your schematic workspace.
Fix these errors by repeating Steps 2-6 of the Wiring Your Schematic section above, to finish wiring the rest of the design as shown.
Go to: Tools ► Verify, and Click “Ok”.
Notice the errors are gone.
Right click on the DRC panel and click “Close”.
Placing Net Labels
Right click the wire connecting Pin 3 of the NE555 and Pin 11 of the OpAmp, then click Properties.
Within the Properties panel, change the value of Name to CLK_OUT and press Enter.
Notice that there is now a label on this wire. Using this method allows you to easily name connections in your design.
Click any empty space in your schematic workspace to clear all filters.
Constraint Manager
Using the constraint manager, you can predefine design rules that will get forward annotated to the PCB layout workspace.
Click Tools ► Constraint Manager.
Within the Constraint Manager’s Navigator panel, select Net Classes ► PWR.
Expand Master, then PWR, and set the Trace Width (th) ► Expansion values to “20”. Note that everything under PWR in the Expansion column in Master will be changed.
Check the box to not show warning again in the same session, then click OK.
Close the Constraint Manager window.
Right-click and close the Output panel.
Go to: File ► Close Project.
Up Next: Lesson 3 - Forward Annotate, Create a PCB File and Draw Your Board Shape