3.5 Preparing for orcad layout  (Page 9/9)

Select the Radio button for Unused Routing . Click OK to continue. Do the same thing for the following layers: INNER2 , SPTOP , SPBOT , SSBOT , FABDWG , NOTES . Remember that you can use the CTRL key to select multiple layers at one time. Also remember that all designs are different and may need extra layers. For example, a design with surface mount components will need the SPTOP and SPBOT layers. If we were to place components on the bottom side of the board, then we would likely need a silkscreen on the bottom and, therefore, the SSBOT layer. Close the spreadsheet when you have made the changes.

The next thing we need to do is change the output settings for the Gerber files . Select Options-->Post Process Settings… to bring up the Post Process Spreadsheet . Select the *.ASB and *.FAB layers. Right-click and select Properties to bring up the Post Process Settings dialog. Uncheck the box that is labeled Enable for Post Processing .

Now select all the layers. You can do this by clicking in the cell in the top-left corner of the spreadsheet ( Plot Output File Name ). Right-click and select Properties to bring up the Post Process Settings dialog. Select the radio button for Extended Gerber . This is the format we want to use for fabrication. Close the spreadsheet when you are done.

Next, you will define a default via size. Click the View Spreadsheet icon and select Padstacks . This will open the padstacks spreadsheet and shows every padstack that is used in your design. Since there are no parts in the design right now, there are not that many padstacks, but this will change after weimport from Capture.

You will edit the VIA1 padstack that is first on the list. This will become the default via for your design. Editing padstacks here is identical to how you edited padstacks when creating a footprint. Let’s start with a clean padstack. Click the name VIA1 to highlight the entire padstack. Right-click and select Properties to show the Edit Padstack dialog. Select the radio button labeled Undefined and also check the box labeled Flood Planes/Pours . Click OK when done. This will reset the definitions for all layers of VIA1 . Now you will set the finished drill size. Highlight the DRILL and DRLDWG layers and open the Edit Padstack dialog. Select a pad shape of Round and give it a width and height of 13.5 (mils). We are using the same clearance requirements that we used before when defining footprints: +20 mils annular ring, +25 mils solder mask, and +35 mils plane clearance. Select the TOP , BOTTOM and INNER layers (we have no inner layers in this design, but it is good practice to define this since we may want to add layers later in a design). Make these layers round with a diameter of 35 mils. Select the GND and POWER layers and make these round with a diameter of 50. Finally, highlight the SMTOP and SMBOT layers and make these round with a diameter of 40.

We will only use one via type in our design, but OrCAD will allow you to define up to 16 different vias. You might want more than one if you wanted slightly larger vias for carrying high-currents. You can even assign specific vias to specific nets, but that is beyond the scope of this tutorial.

When a netlist from Capture is imported, we can set the default widths and other properties for all nets that get imported. After importing we can customize these parameters on a per-net basis. Let’s set the values for the default net. Click the View Spreadsheet icon and choose Nets . You will see a spreadsheet with just one net, DEFAULT . After you import your netlist from Capture, you will see all the nets in your design in this spreadsheet. Double-click the net to bring up the Edit Net dialog.

Our design will not be too aggressive, so we will use 10 mil traces. Set the Min Width and Conn Width to 10, and set the Max Width to 50. Click OK when you have made the changes.

The final thing we need to do to our template is set a few global spacing constraints. These spacing values will be used when you have Layout automatically check for design errors. Select Options-->Global Spacing… to bring up the Route Spacing spreadsheet. Click on Layer Name to highlight every cell, and then right-click and select Properties to bring up the Edit Spacing dialog. Put a value of 10 in every field and click OK. Close the Route Spacing spreadsheet.

Save your template. You are done with it and are ready to export your design from Capture to Layout.

Creating the netlist

To export your design to Layout, you must first create a netlist. A netlist is a file that has all the parts, footprints and nets for your design in a format that can be readby the layout program. To start netlist generation, highlight your dsn file and select Tools-->Create Netlist… to bring up the Create Netlist dialog box.

Click on the Layout tab in the dialog box. You don’t need to modify any settings, just click OK to generate the netlist. When finished you should have a file called Elec424Tutorial.mnl in your sch directory. Your design is finally ready for import into layout.