The hard way of adding your components, which will be necessary on occasion, is to draw it yourself. Start by having the component's data sheet ready with the dimensions of the component available.
We will choose a simple component so you get the idea without a bunch of redundant tasks in this lesson. We will be creating the footprint for the .01uf capacitor. The capacitor is already in the library, but it will show you how to create footprints. The Digikey part number for the capacitor is 399-1158-1-ND and they cost about a nickel each.
The data sheet for the capacitor is located at the manufacturer's website at
http://www.kemet.com/kemet/web/homepage/kechome.nsf/vapubfiles/F3102X7R/$file/F3102X7R.pdf
. The information we need is located on page 1 of the data sheet. Each of the two pads is .02 inch by .049 inch and they are spaced approximately .030 inch apart. The capacitor is a ceramic capacitor so there is no need to specify a direction for the capacitor or label the pins to be able to differentiate between them.
Start by selecting the Pad Tool icon.
Figure 9.10
Select the square pad .024 X .059. The reason for selecting a larger pad is to allow easier attachment of the device to the board. Whenever possible, allow a little extra room for the component. Insure the layer is selected as the top layer (located next to the Pad Type).
Figure 9.11
Drop two of the pads on your board. Move the pads close to the point of origin (0,0) with one of the pads located at 0,0. That will center the pad directly over the point of origin. Next you have to do a little calculating to figure the correct distance apart to place the pads. The distance we have been shown in the data sheet is .030. We have to add to that the width of one pad as the pad's location is measured from the centers of the pads. Therefore, the total distance from center of pad to center of pad is going to be .054 inch.
With the first pad located at 0,0 you will need to highlight the second pad. With the pad highlighted, type the correct location for the second pad in the X coordinate as shown in figure 9.12.
Figure 9.12
Now that we have the landing pads spaced properly, you can change the names of the pads. Currently they should be labeled 1 and 2. If you want to change the pad labels, highlight the pad and change the label in the text box located next to the Y coordinate.
Next we need to add a silk screen outline for the component. Click the trace tool button, insure the line width is set to .10, and change the layer to top silk.
Figure 9.13
Now draw a square around the pads allowing enough room within the square for the component to fit comfortably. You will probably notice as you draw the square that you are unable to make it fit evenly on both sides of the pads. That is because the snap function is set to .025 inch. To change that setting, click Edit, go down to Preferences and click Preferences. In the window that appears, select Grids on the left of the pane. Change the snap feature to .001. Notice you can change the appearance of the grid on that page, whether it is shown or not, and under the General tab you can change the entire background appearance.
Figure 9.14
After you click OK, you can move the lines evenly around the pads. When they are in place, add a label to the component with the text button.
Figure 9.15
A text window will open for you to enter your text. In the same window you can change the font, size, etc of the text you are dropping on the board.
Figure 9.16
Type in C1 for the component label and click OK. Arrange the text in a meaningful location around the component. We are almost finished.
Highlight all parts of the component and right click the mouse. Go down to Group and click. All of the portions of the component that were part of the component are now grouped as a single object and can be moved around, copied and pasted at will in your project.
Figure 9.17
