kicad 下面教大家如何去修改已经存在的封装，比如修改封装的丝印，焊盘钻孔的尺寸，焊盘与焊盘之间的间距等，在修改封装之前要确保我们封装库中是存在的，

In this recipe, you will learn how to modify an existing footprint. You may want to do something simple, like relocate silkscreen graphics, or change the drill size of the pads. Whichever the case may be, the process is the same.

Start by finding a footprint to edit. Let's assume that you know which library this footprint is in, and you know its name. If you don’t, use the footprint browser in Pcbnew to find it first.

From the main KiCad window, start the Footprint Manager. In the Footprint Manager, use the 'Import footprint' button to find and import the footprint (Figure 39.1). If the Editor already contains a footprint, you will get a prompt asking for confirmation to discard it. Consider saving it if you haven’t done so already, and continue.

Figure 39.1: Import the footprint you want to edit.

In the browser, navigate to the .pretty folder where the footprint is, and select it. In my example, I navigated to the location of the Digikey footprints directory, and I have selected to modify the LED3mmRadial footprint (Figure 39.2).

Figure 39.2: Navigate to the footprint’s location and select it.

Click 'Open' to import the footprint. The footprint will appear in the Editor sheet. Let’s make a couple of simple modifications:

1. Add the block text 'LED' in the silkscreen.
2. Mark the cathode pad with the letter 'C' in the silkscreen. Note: According to IEEE 315, Clause 8.4, the letter “K” should be used to mark the Cathode, while the letter “C” is reserved for the Collector.21
3. Reduce the drill size to 0.8 mm for both pads.

Let’s start with the text. Select the 'F.SilkS' layer from the Layers Manager. Select the Text tool. Click on the right side of the LED footprint; the text properties will appear. Type 'C' in the text box and click on 'Ok'. Position the text block right next to the symbol cathode (the straight section of the circle), and then click below the footprint to create the second text block. Type 'LED' in the text box, and click 'Ok' to create the new block. Click on the sheet to commit the new block. Continue with the pad drill size. Hover the mouse pointer over pad 1 and type 'E' to bring up the pad properties. In the pad properties window,

21 For your convenience, I have included the text of IEEE 315, Clause 8.4.

8.4 Rules for Drawing Style 1 Symbols To draw a device symbol, start at an electrode whose polarity is known (usually an emitter) and proceed along the device, showing all of its regions individually. Finally, indicate ohmic connections where required.

NOTE — 8.4A: Numbers, letters, and words in parentheses are to correlate illustrations in the standard; they are not intended to represent device terminal numbering or identification and are not part of the symbol as shown in items 8.5, 8.6, 8.10, and 8.11. Name of Terminal Letter Anode A Base B Collector C Drain D Emitter E Gate G Cathode K Source Main terminal S Substrate (bulk) T U Used with bidirectional thyristors. The terminals are differentiated by numerical subscripts 1 and 2, T 1 being the terminal to which the gate trigger signal is referenced, if applicable.

change the hole size X value to 0.8 mm (Figure 39.3). Then click 'Ok' to make the change effective. Figure 39.3: Modify the drill size for pad 1. Do the same for pad 2. The modified footprint should look like the example in Figure 39.4. Figure 39.4: The modified footprint.

Before you can use the modified footprint you must save it. Use the Export Footprint button (the one with the red arrow) to do this. Navigate to the location of your custom footprints .pretty folder, and store the modified footprint there (Figure 39.5). Figure 39.5: Store the modified footprint in the custom footprints folder. You are now able to use your modified footprint in your layouts.