3.5 Preparing for orcad layout  (Page 4/9)

Next, we need to define the clearance on the plane layers. The middle layers of our circuit board are solid pieces of copper that are used for power and ground. To prevent short circuits, we need to define a clearance around our drill. Most board houses will also have requirements for this, but 35 milsbeyond the drill size is usually a good start. In our case, we will do a little rounding and just use 2 mm. Select the PLANE layer and define a round pad with a height and width of 2 mm.

The last thing we need to define is the solder mask. This is usually defined as slightly larger (about 5 mils) than the annular rings on the top and bottom layers. Select SMTOP and SMBOT and make them round pads with height and width of 1.625 mm.

You have finished defining your padstack for this part. You can close the spreadsheet and you will see that pin 1 should now look a little different based on the changes you just made.

You probably noticed that you don’t need to define all of the layers. As a guide, here are the layers that you need to define for thru-hole and surface mount parts.

• Thru-Hole - TOP, BOTTOM, INNER, PLANCE, SMTOP, SMBOT, DRLDWG, DRILL
• Surface Mount - TOP, SMTOP, SPTOP

As far as padstacks are concerned, surface mount parts are a lot easier to work with.

Library Manager can be a bit flaky sometimes, so it is best to save your changes to footprints often. Go ahead and click Save As . You have not yet created a footprint library, so you will need to click the Create New Library button. Browse to your lib directory and name the library Elec424Tutorial .

Let’s now clean up a few things before adding the rest of the pins. You will see a lot of text on your screen. Most of it is on the layer ASSYTOP , which we will not use. This text is safe to delete. Open the text spreadsheet and you will see five text items. Select all the text on the ASSYTOP layer and delete them. This will clean up your footprint a bit. You can leave the reference designator text on the SSTOP layer. We will need it.

We can add pins to the footprint in a number of ways, but the easiest way to do this is to use the footprints spreadsheet. Open the spreadsheet and you will see just pin 1 with an x,y location of 0,0.

For this part we have to take note of a few things. Our schematic symbol has pins 1 to 4, while the datasheet for the part labels the pins A, A', B and B'. We will make pin 1 = A', pin 2 = A, pin 3 = B and pin 4 = B'. To create a new pin, just highlight pin 1 in the spreadsheet and type CTRL-C . This will create open the following Add Pad dialog.

This dialog allows you to give the pad a name (OrCAD autoincrements, so 2 is already given as the name), adjust the x and y coordinates of the pin, and choose which padstack you want to use for the pin. In most cases, you will leave the other settings as they are by default. Set the x and y coordinates as they are shownabove and click OK . Add the remaining two pads as shown on the mechanical drawing for the pushbutton. When you close the footprint spreadsheet, your footprint should look like this.