3.6 Starting layout in orcad  (Page 3/9)

Now you can begin to place the rest of your components. You will probably want to print out your schematics so that you can see where the components are supposed to go in relation to each other. When you pick up a component, the ratsnest for that component will appear to show you the connections to other parts. If you want, you can also turn the ratsnest back on to see all of the connections. Personally, I like to turn on at least the power and ground nets and give them a distinct color, especially in designs with multiple voltages. Open the nets spreadsheet and find the net GND . Right-click and select Change Color . Choose any color you like. Right-click again and select Enable<->Disable . When you close the spreadsheet, the GND net should be visible. Do the same thing for the other power nets. When you close the spreadsheet it will look a little messy. You can use the Refresh All icon to force OrCAD to redraw connections.

When placing components, you may want to work on a finer grid. Right now, the grid is probably set at 100 mils. You can change this by selecting Options-->System Settings and then changing the Place Grid setting. I usually use a value of 25. I also like to adjust the Visible Grid setting to give me an on-screen reference. I usually use a value of 50 when placing components.

Start placing the remaining components on your board. Start with placing the power connector on the left side of the board, the PLD in the center, and TIL311 on the right. Try to keep components that belong together near each other. When you are done, your board should look something like this.

The silkscreen is a bit messy, but we will deal with that later. In fact, during routing, the silkscreen can get in the way, so go ahead and turn off the SST layer now using the same method you used before for the other layers.

Save your design. We have added a few components, so you may get the following warning.

We will address this later. Do not worry about it now.

Routing power, ground&Copper pours

In any design, it is usually wise to route all power and ground connections before anything else. On a thru-hole technology board, this is very easy because connections can be made to the solid plane as the pin passes through the board. The pin will be “flashed” to power or ground. We need to set up our design so that OrCAD knows that the two planes are associated with nets. Open the nets spreadsheet and find the net GND . Double-click to open the Edit Net dialog and click the button labeled Net Layers… Under the section Plane Layers , check the box labeled GND . This will inform OrCAD that the net GND is associated with the solid plane on layer 2. Do the same thing for the net VCC5 . When you close the spreadsheet, click the Refresh All button. The ratsnests for VCC5 and GND will disappear. This is because they are now connected to the plane layer. To see this, press Backspace to clear the screen, then press ‘ 3 ’ (the shortcut key for the ground layer) to view the ground layer.