Under Windows run kicad.exe. Under Linux type 'kicad' in your Terminal. You are now in the main window of the KiCad project manager. From here you have access to eight stand-alone software tools: Eeschema, Schematic Library Editor, Pcbnew, PCB Footprint Editor, GerbView, Bitmap2Component, PCB Calculator and Pl Editor. Refer to the work-flow chart to give you an idea how the main tools are used.

Create a new project: File → New → Project. Name the project file 'tutorial1'. The project file will automatically take the extension ".pro". The exact appearance of the dialog depends on the used platform, but there should be a checkbox for creating a new directory. Let it stay checked unless you already have a dedicated directory. All your project files will be saved there.

Let’s begin by creating a schematic. Start the schematic editor Eeschema, . It is the first button from the left.

Click on the 'Page Settings' icon on the top toolbar. Set the appropriate 'paper size' ('A4','8.5x11' etc.) and enter the Title as 'Tutorial1'. You will see that more information can be entered here if necessary. Click OK. This information will populate the schematic sheet at the bottom right corner. Use the mouse wheel to zoom in. Save the whole schematic: File → Save

We will now place our first component. Click on the 'Place symbol' icon in the right toolbar. You may also press the 'Add Symbol' hotkey [a].

Click on the middle of your schematic sheet. A Choose Symbol window will appear on the screen. We’re going to place a resistor. Search / filter on the 'R' of Resistor. You may notice the 'Device' heading above the Resistor. This 'Device' heading is the name of the library where the component is located, which is quite a generic and useful library.

Double click on it. This will close the 'Choose Symbol' window. Place the component in the schematic sheet by clicking where you want it to be.

Click on the magnifier icon to zoom in on the component. Alternatively, use the mouse wheel to zoom in and zoom out. Press the wheel (central) mouse button to pan horizontally and vertically.

Try to hover the mouse over the component 'R' and press [r]. The component should rotate. You do not need to actually click on the component to rotate it.

Right click in the middle of the component and select Properties → Edit Value. You can achieve the same result by hovering over the component and pressing [v]. Alternatively, [e] will take you to the more general Properties window. Notice how the right-click menu below shows the hotkeys for all available actions.

The Edit Value Field window will appear. Replace the current value 'R' with '1 k'. Click OK.

To place another resistor, simply click where you want the resistor to appear. The symbol selection window will appear again.

The resistor you previously chose is now in your history list, appearing as 'R'. Click OK and place the component.

In case you make a mistake and want to delete a component, right click on the component and click 'Delete'. This will remove the component from the schematic. Alternatively, you can hover over the component you want to delete and press [Delete].

You can also duplicate a component already on your schematic sheet by hovering over it and pressing [c]. Click where you want to place the new duplicated component.

Right click on the second resistor. Select 'Drag'. Reposition the component and left click to drop. The same functionality can be achieved by hovering over the component and by pressing [g]. [r] will rotate the component while [x] and [y] will flip it about its x- or y-axis.

Edit the second resistor by hovering over it and pressing [v]. Replace 'R' with '100'. You can undo any of your editing actions with Ctrl+Z.

Change the grid size. You have probably noticed that on the schematic sheet all components are snapped onto a large pitch grid. You can easily change the size of the grid by Right-Click → Grid. In general, it is recommended to use a grid of 50.0 mils for the schematic sheet.

We are going to add a component from a library that may not be configured in the default project. In the menu, choose Preferences → Manage Symbol Libraries. In the Symbol Libraries window you can see two tabs: Global Libraries and Project Specific Libraries. Each one has one sym-lib-table file. For a library (.lib file) to be available it must be in one of those sym-lib-table files. If you have a library file in your file system and it’s not yet available, you can add it to either one of the sym-lib-table files. For practice we will now add a library which already is available.

Select the Project Specific table. Click the file browser button below the table. You need to find where the official KiCad libraries are installed on your computer. Look for a library directory containing a hundred of .dcm and .lib files. Try in C:\Program Files (x86)\KiCad\share\ (Windows) and /usr/share/kicad/library/ (Linux). When you have found the directory, choose and add the 'MCU_Microchip_PIC12.lib' library and close the window. It will be added to the end of of the list. Now click its nickname and change it to 'microchip_pic12mcu'. Close the Symbol Libraries window with OK.

Repeat the add-component steps, however this time select the 'microchip_pic12mcu' library instead of the 'Device' library and pick the 'PIC12C508A-ISN' component.

Hover the mouse over the microcontroller component. Notice that [x] and [y] again flip the component. Keep the symbol mirrored around the Y axis so that the pins G0 and G1 point to right.

Repeat the add-component steps, this time choosing the 'Device' library and picking the 'LED' component from it.

Organise all components on your schematic sheet as shown below.

We now need to create the schematic component 'MYCONN3' for our 3-pin connector. You can jump to the section titled Make Schematic Symbols in KiCad to learn how to make this component from scratch and then return to this section to continue with the board.

You can now place the freshly made component. Press [a] and pick the 'MYCONN3' component in the 'myLib' library.

The component identifier 'J?' will appear under the 'MYCONN3' label. If you want to change its position, right click on 'J?' and click on 'Move Field' (equivalent to [m]). It might be helpful to zoom in before/while doing this. Reposition 'J?' under the component as shown below. Labels can be moved around as many times as you please.

It is time to place the power and ground symbols. Click on the 'Place power port' button on the right toolbar. Alternatively, press [p]. In the component selection window, scroll down and select 'VCC' from the 'power' library. Click OK.

Click above the pin of the 1 k resistor to place the VCC part. Click on the area above the microcontroller 'VDD'. In the 'Component Selection history' section select 'VCC' and place it next to the VDD pin. Repeat the add process again and place a VCC part above the VCC pin of 'MYCONN3'. Move references and values out of the way if needed.

Repeat the add-pin steps but this time select the GND part. Place a GND part under the GND pin of 'MYCONN3'. Place another GND symbol on the left of the VSS pin of the microcontroller. Your schematic should now look something like this:

Next, we will wire all our components. Click on the 'Place wire' icon on the right toolbar.

Click on the little circle at the end of pin 7 of the microcontroller and then click on the little circle on pin 1 of the LED. Click once when you are drawing the wire to create a corner. You can zoom in while you are placing the connection.

Repeat this process and wire up all the other components as shown below. To terminate a wire just double-click. When wiring up the VCC and GND symbols, the wire should touch the bottom of the VCC symbol and the middle top of the GND symbol. See the screenshot below.

We will now consider an alternative way of making a connection using labels. Pick a net labelling tool by clicking on the 'Place net label' icon on the right toolbar. You can also use [l].

Click in the middle of the wire connected to pin 6 of the microcontroller. Name this label 'INPUT'. The label is still an independent item which you can for example move, rotate and delete. The small anchor rectangle of the label must be exactly on a wire or a pin for the label to take effect.

Follow the same procedure and place another label on line on the right of the 100 ohm resistor. Also name it 'INPUT'. The two labels, having the same name, create an invisible connection between pin 6 of the PIC and the 100 ohm resistor. This is a useful technique when connecting wires in a complex design where drawing the lines would make the whole schematic messier. To place a label you do not necessarily need a wire, you can simply attach the label to a pin.

Labels can also be used to simply label wires for informative purposes. Place a label on pin 7 of the PIC. Enter the name 'uCtoLED'. Name the wire between the resistor and the LED as 'LEDtoR'. Name the wire between 'MYCONN3' and the resistor as 'INPUTtoR'.

You do not have to label the VCC and GND lines because the labels are implied from the power objects they are connected to.

Below you can see what the final result should look like.

Let’s now deal with unconnected wires. Any pin or wire that is not connected will generate a warning when checked by KiCad. To avoid these warnings you can either instruct the program that the unconnected wires are deliberate or manually flag each unconnected wire or pin as unconnected.

Click on the 'Place no connection flag' icon on the right toolbar. Click on pins 2, 3, 4 and 5. An X will appear to signify that the lack of a wire connection is intentional.

Some components have power pins that are invisible. You can make them visible by clicking on the 'Show hidden pins' icon on the left toolbar. Hidden power pins get automatically connected if VCC and GND naming is respected. Generally speaking, you should try not to make hidden power pins.

It is now necessary to add a 'Power Flag' to indicate to KiCad that power comes in from somewhere. Press [a] and search for 'PWR_FLAG' which is in 'power' library. Place two of them. Connect them to a GND pin and to VCC as shown below.

Sometimes it is good to write comments here and there. To add comments on the schematic use the 'Place text' icon on the right toolbar.

All components now need to have unique identifiers. In fact, many of our components are still named 'R?' or 'J?'. Identifier assignation can be done automatically by clicking on the 'Annotate schematic symbols' icon on the top toolbar.

In the Annotate Schematic window, select 'Use the entire schematic' and click on the 'Annotate' button. Click 'Close'. Notice how all the '?' have been replaced with numbers. Each identifier is now unique. In our example, they have been named 'R1', 'R2', 'U1', 'D1' and 'J1'.

We will now check our schematic for errors. Click on the 'Perform electrical rules check' icon on the top toolbar. Click on the 'Run' button. A report informing you of any errors or warnings such as disconnected wires is generated. You should have 0 Errors and 0 Warnings. In case of errors or warnings, a small green arrow will appear on the schematic in the position where the error or the warning is located. Check 'Create ERC file report' and press the 'Run' button again to receive more information about the errors.

The schematic is now finished. We can now create a Netlist file to which we will add the footprint of each component. Click on the 'Generate netlist' icon on the top toolbar. Click on the 'Generate Netlist' button and save under the default file name.

After generating the Netlist file, click on the 'Run Cvpcb' icon on the top toolbar. If a missing file error window pops up, just ignore it and click OK.

Cvpcb allows you to link all the components in your schematic with footprints in the KiCad library. The pane on the center shows all the components used in your schematic. Here select 'D1'. In the pane on the right you have all the available footprints, here scroll down to 'LED_THT:LED-D5.0mm' and double click on it.

It is possible that the pane on the right shows only a selected subgroup of available footprints. This is because KiCad is trying to suggest to you a subset of suitable footprints. Click on the icons , and to enable or disable these filters.

For 'U1' select the 'Package_DIP:DIP-8_W7.62mm' footprint. For 'J1' select the 'Connector:Banana_Jack_3Pin' footprint. For 'R1' and 'R2' select the 'Resistor_THT:R_Axial_DIN0207_L6.3mm_D2.5mm_P2.54mm_Vertical' footprint.

If you are interested in knowing what the footprint you are choosing looks like, you can click on the 'View selected footprint' icon for a preview of the current footprint.

You are done. You can save the schematic now by clicking File → Save Schematic or with the button 'Apply, Save Schematic & Continue'.

You can close Cvpcb and go back to the Eeschema schematic editor. If you didn’t save it in Cvpcb save it now by clicking on File → Save. Create the netlist again. Your netlist file has now been updated with all the footprints. Note that if you are missing the footprint of any device, you will need to make your own footprints. This will be explained in a later section of this document.

Switch to the KiCad project manager. You can see the net list file in the file list.

The netlist file describes all components and their respective pin connections. The netlist file is actually a text file that you can easily inspect, edit or script.

To create a Bill Of Materials (BOM), go to the Eeschema schematic editor and click on the 'Generate bill of materials' icon on the top toolbar. By default there is no plugin active. You add one, by clicking on Add Plugin button. Select the *.xsl file you want to use, in this case, we select bom2csv.xsl.

sudo apt-get install xsltproc

sudo yum install xsltproc

brew install libxslt

xsltproc -o "%O" "/home/<user>/kicad/eeschema/plugins/bom2csv.xsl" "%I"

xsltproc -o "%O.csv" "/home/<user>/kicad/eeschema/plugins/bom2csv.xsl" "%I"

Now press 'Generate'. The file (same name as your project) is located in your project folder. Open the *.csv file with LibreOffice Calc or Excel. An import window will appear, press OK.

Let us suppose that you have three 4-pin connectors that you want to connect together pin to pin. Use the label option (press [l]) to label pin 4 of the P4 part. Name this label 'a1'. Now press [Insert] to have the same item automatically added on the pin below pin 4 (PIN 3). Notice how the label is automatically renamed 'a2'.

Press [Insert] two more times. This key corresponds to the action 'Repeat last item' and it is an infinitely useful command that can make your life a lot easier.

Repeat the same labelling action on the two other connectors CONN_2 and CONN_3 and you are done. If you proceed and make a PCB you will see that the three connectors are connected to each other. Figure 2 shows the result of what we described. For aesthetic purposes it is also possible to add a series of 'Place wire to bus entry' using the icon and bus line using the icon , as shown in Figure 3. Mind, however, that there will be no effect on the PCB.

It should be pointed out that the short wire attached to the pins in Figure 2 is not strictly necessary. In fact, the labels could have been applied directly to the pins.

Let’s take it one step further and suppose that you have a fourth connector named CONN_4 and, for whatever reason, its labelling happens to be a little different (b1, b2, b3, b4). Now we want to connect Bus a with Bus b in a pin to pin manner. We want to do that without using pin labelling (which is also possible) but by instead using labelling on the bus line, with one label per bus.

Connect and label CONN_4 using the labelling method explained before. Name the pins b1, b2, b3 and b4. Connect the pin to a series of 'Wire to bus entry' using the icon and to a bus line using the icon . See Figure 4.

Put a label (press [l]) on the bus of CONN_4 and name it 'b[1..4]'.

Put a label (press [l]) on the previous bus and name it 'a[1..4]'.

What we can now do is connect bus a[1..4] with bus b[1..4] using a bus line with the button .

By connecting the two buses together, pin a1 will be automatically connected to pin b1, a2 will be connected to b2 and so on. Figure 4 shows what the final result looks like.

The 'Repeat last item' option accessible via [Insert] has also been extensively used to place the many series of 'Wire to bus entry' using the icon .

From the KiCad project manager, click on the 'Pcb layout editor' icon . You can also use the corresponding toolbar button from Eeschema. The 'Pcbnew' window will open. If you get a message saying that a *.kicad_pcb file does not exist and asks if you want to create it, just click Yes.

Begin by entering some schematic information. Click on the 'Page settings' icon on the top toolbar. Set the appropriate 'paper size' ('A4','8.5x11' etc.) and 'title' as 'Tutorial1'.

It is a good idea to start by setting the clearance and the minimum track width to those required by your PCB manufacturer. In general you can set the clearance to '0.25' and the minimum track width to '0.25'. Click on the Setup → Design Rules menu. If it does not show already, click on the 'Net Classes Editor' tab. Change the 'Clearance' field at the top of the window to '0.25' and the 'Track Width' field to '0.25' as shown below. Measurements here are in mm.

Click on the 'Global Design Rules' tab and set 'Minimum track width' to '0.25'. Click the OK button to commit your changes and close the Design Rules Editor window.

Now we will import the netlist file if you created one. Click on the 'Read netlist' icon on the top toolbar. The netlist file 'tutorial1.net' should be selected in the 'Netlist file' field if it was created from Eeschema. Click on 'Read Current Netlist'. Then click the 'Close' button.

All components should now be visible. They are selected and follow the mouse cursor.

Move the components to the middle of the board. If necessary you can zoom in and out while you move the components. Click the left mouse button.

All components are connected via a thin group of wires called ratsnest. Make sure that the 'Show/hide board ratsnest' button is pressed. In this way you can see the ratsnest linking all components.

You can move each component by hovering over it and pressing [m]. Click where you want to place them. Alternatively you can select a component by clicking on it and then drag it. Press [r] to rotate a component. Move all components around until you minimise the number of wire crossovers.

Note how one pin of the 100 ohm resistor is connected to pin 6 of the PIC component. This is the result of the labelling method used to connect pins. Labels are often preferred to actual wires because they make the schematic much less messy.

Now we will define the edge of the PCB. Select the 'Edge.Cuts' layer from the drop-down menu in the top toolbar. Click on the 'Add graphic lines' icon on the right toolbar. Trace around the edge of the board, clicking at each corner, and remember to leave a small gap between the edge of the green and the edge of the PCB.

Next, connect up all the wires except GND. In fact, we will connect all GND connections in one go using a ground plane placed on the bottom copper (called B.Cu) of the board.

Now we must choose which copper layer we want to work on. Select 'F.Cu (PgUp)' in the drop-down menu on the top toolbar. This is the front top copper layer.

If you decide, for instance, to do a 4 layer PCB instead, go to Setup → Layers Setup and change 'Copper Layers' to 4. In the 'Layers' table you can name layers and decide what they can be used for. Notice that there are very useful presets that can be selected via the 'Preset Layer Groupings' menu.

Click on the 'Route tracks' icon on the right toolbar. Click on pin 1 of 'J1' and run a track to pad 'R2'. Double-click to set the point where the track will end. The width of this track will be the default 0.250 mm. You can change the track width from the drop-down menu in the top toolbar. Mind that by default you have only one track width available.

If you would like to add more track widths go to: Setup → Design Rules → Global Design Rules tab and at the bottom right of this window add any other width you would like to have available. You can then choose the widths of the track from the drop-down menu while you lay out your board. See the example below (inches).

Alternatively, you can add a Net Class in which you specify a set of options. Go to Setup → Design Rules → Net Classes Editor and add a new class called 'power'. Change the track width from 8 mil (indicated as 0.0080) to 24 mil (indicated as 0.0240). Next, add everything but ground to the 'power' class (select 'default' at left and 'power' at right and use the arrows).

If you want to change the grid size, Right click → Grid. Be sure to select the appropriate grid size before or after laying down the components and connecting them together with tracks.

Repeat this process until all wires, except pin 3 of J1, are connected. Your board should look like the example below.

Let’s now run a track on the other copper side of the PCB. Select 'B.Cu' in the drop-down menu on the top toolbar. Click on the 'Route tracks' icon . Draw a track between pin 3 of J1 and pin 8 of U1. This is actually not necessary since we could do this with the ground plane. Notice how the colour of the track has changed.

Go from pin A to pin B by changing layer. It is possible to change the copper plane while you are running a track by placing a via. While you are running a track on the upper copper plane, right click and select 'Place Via' or simply press [v]. This will take you to the bottom layer where you can complete your track.

When you want to inspect a particular connection you can click on the 'Highlight net' icon on the right toolbar. Click on pin 3 of J1. The track itself and all pads connected to it should become highlighted.

Now we will make a ground plane that will be connected to all GND pins. Click on the 'Add filled zones' icon on the right toolbar. We are going to trace a rectangle around the board, so click where you want one of the corners to be. In the dialogue that appears, set 'Default pad connection' to 'Thermal relief' and 'Outline slope' to 'H,V and 45 deg only' and click OK.

Trace around the outline of the board by clicking each corner in rotation. Finish your rectangle by clicking the first corner second time. Right click inside the area you have just traced. Click on 'Zones'→'Fill or Refill All Zones'. The board should fill in with green and look something like this:

Run the design rules checker by clicking on the 'Perform design rules check' icon on the top toolbar. Click on 'Start DRC'. There should be no errors. Click on 'List Unconnected'. There should be no unconnected items. Click OK to close the DRC Control dialogue.

Save your file by clicking on File → Save. To admire your board in 3D, click on View → 3D Viewer.

You can drag your mouse around to rotate the PCB.

Your board is complete. To send it off to a manufacturer you will need to generate all Gerber files.

From KiCad, open the Pcbnew board editor.

Click on File → Plot. Select 'Gerber' as the 'Plot format' and select the folder in which to put all Gerber files. Proceed by clicking on the 'Plot' button.

To generate the drill file, from Pcbnew go again to the File → Plot option. Default settings should be fine.

These are the layers you need to select for making a typical 2-layer PCB:

To view all your Gerber files go to the KiCad project manager and click on the 'GerbView' icon. On the drop-down menu or in the Layers manager select 'Graphic layer 1'. Click on File → Open Gerber file(s) or click on the icon . Select and open all generated Gerber files. Note how they all get displayed one on top of the other.

Open the drill files with File → Open Excellon Drill File(s).

Use the Layers manager on the right to select/deselect which layer to show. Carefully inspect each layer before sending them for production.

The view works similarly to Pcbnew. Right click inside the view and click 'Grid' to change the grid.

From Pcbnew click on File → Export → Specctra DSN and save the file locally. Launch FreeRouter and click on the 'Open Your Own Design' button, browse for the dsn file and load it.

FreeRouter has some features that KiCad does not currently have, both for manual routing and for automatic routing. FreeRouter operates in two main steps: first, routing the board and then optimising it. Full optimisation can take a long time, however you can stop it at any time need be.

You can start the automatic routing by clicking on the 'Autorouter' button on the top bar. The bottom bar gives you information about the on-going routing process. If the 'Pass' count gets above 30, your board probably can not be autorouted with this router. Spread your components out more or rotate them better and try again. The goal in rotation and position of parts is to lower the number of crossed airlines in the ratsnest.

Making a left-click on the mouse can stop the automatic routing and automatically start the optimisation process. Another left-click will stop the optimisation process. Unless you really need to stop, it is better to let FreeRouter finish its job.

Click on the File → Export Specctra Session File menu and save the board file with the .ses extension. You do not really need to save the FreeRouter rules file.

Back to Pcbnew. You can import your freshly routed board by clicking on File → Import → Spectra Session and selecting your .ses file.

We can use the Component Library Editor (part of Eeschema) to make new components. In our project folder 'tutorial1' let’s create a folder named 'library'. Inside we will put our new library file myLib.lib as soon as we have created our new component.

Now we can start creating our new component. From KiCad, start Eeschema, click on the 'Library Editor' icon and then click on the 'New component' icon . The Component Properties window will appear. Name the new component 'MYCONN3', set the 'Default reference designator' as 'J', and the 'Number of units per package' as '1'. Click OK. If the warning appears just click yes. At this point the component is only made of its labels. Let’s add some pins. Click on the 'Add Pins' icon on the right toolbar. To place the pin, left click in the centre of the part editor sheet just below the 'MYCONN3' label.

In the Pin Properties window that appears, set the pin name to 'VCC', set the pin number to '1', and the 'Electrical type' to 'Power input' then click OK.

Place the pin by clicking on the location you would like it to go, right below the 'MYCONN3' label.

Repeat the place-pin steps, this time 'Pin name' should be 'INPUT', 'Pin number' should be '2', and 'Electrical Type' should be 'Passive'.

Repeat the place-pin steps, this time 'Pin name' should be 'GND', 'Pin number' should be '3', and 'Electrical Type' should be 'Passive'. Arrange the pins one on top of the other. The component label 'MYCONN3' should be in the centre of the page (where the blue lines cross).

Next, draw the contour of the component. Click on the 'Add rectangle' icon . We want to draw a rectangle next to the pins, as shown below. To do this, click where you want the top left corner of the rectangle to be (do not hold the mouse button down). Click again where you want the bottom right corner of the rectangle to be.

If you want to fill the rectangle with yellow, set the fill colour to 'yellow 4' in Preferences → Select color scheme, then select the rectangle in the editing screen with [e], selecting 'Fill background'.

Save the component in your library myLib.lib. Click on the 'New Library' icon , navigate into tutorial1/library/ folder and save the new library file with the name myLib.lib.

Go to Preferences → Component Libraries and add both tutorial1/library/ in 'User defined search path' and myLib.lib in 'Component library files'.

Click on the 'Select working library' icon . In the Select Library window click on myLib and click OK. Notice how the heading of the window indicates the library currently in use, which now should be myLib.

Click on the 'Update current component in current library' icon in the top toolbar. Save all changes by clicking on the 'Save current loaded library on disk' icon in the top toolbar. Click 'Yes' in any confirmation messages that appear. The new schematic component is now done and available in the library indicated in the window title bar.

You can now close the Component library editor window. You will return to the schematic editor window. Your new component will now be available to you from the library myLib.

You can make any library file.lib file available to you by adding it to the library path. From Eeschema, go to Preferences → Library and add both the path to it in 'User defined search path' and file.lib in 'Component library files'.

From KiCad, start Eeschema, click on the 'Library Editor' icon , click on the 'Select working library' icon and choose the library 'device'. Click on 'Load component to edit from the current lib' icon and import the 'RELAY_2RT'.

Click on the 'Export component' icon , navigate into the library/ folder and save the new library file with the name myOwnLib.lib.

You can make this component and the whole library myOwnLib.lib available to you by adding it to the library path. From Eeschema, go to Preferences → Component Libraries and add both library/ in 'User defined search path' and myOwnLib.lib in the 'Component library files'. Close the window.

Click on the 'Select working library' icon . In the Select Library window click on myOwnLib and click OK. Notice how the heading of the window indicates the library currently in use, it should be myOwnLib.

Click on the 'Load component to edit from the current lib' icon and import the 'RELAY_2RT'.

You can now modify the component as you like. Hover over the label 'RELAY_2RT', press [e] and rename it 'MY_RELAY_2RT'.

Click on 'Update current component in current library' icon in the top toolbar. Save all changes by clicking on the 'Save current loaded library on disk' icon in the top toolbar.

Head to the quicklib web page: http://kicad.rohrbacher.net/quicklib.php

Fill out the page with the following information: Component name: MYCONN3 Reference Prefix: J Pin Layout Style: SIL Pin Count, N: 3

Click on the 'Assign Pins' icon. Fill out the page with the following information: Pin 1: VCC Pin 2: input Pin 3: GND. Type : Passive for all 3 pins.

Click on the icon 'Preview it' and, if you are satisfied, click on the 'Build Library Component'. Download the file and rename it tutorial1/library/myQuickLib.lib.. You are done!

Have a look at it using KiCad. From the KiCad project manager, start Eeschema, click on the 'Library Editor' icon , click on the 'Import Component' icon , navigate to tutorial1/library/ and select myQuickLib.lib.

You can make this component and the whole library myQuickLib.lib available to you by adding it to the KiCad library path. From Eeschema, go to Preferences → Component Libraries and add library in 'User defined search path' and myQuickLib.lib in 'Component library files'.

Suppose that you want to create a schematic component for a device with 50 pins. It is common practise to draw it using multiple low pin-count drawings, for example two drawings with 25 pins each. This component representation allows for easy pin connection.

The best way to create our component is to use quicklib to generate two 25-pin components separately, re-number their pins using a Python script and finally merge the two by using copy and paste to make them into one single DEF and ENDDEF component.

You will find an example of a simple Python script below that can be used in conjunction with an in.txt file and an out.txt file to re-number the line: X PIN1 1 -750 600 300 R 50 50 1 1 I into X PIN26 26 -750 600 300 R 50 50 1 1 I this is done for all lines in the file in.txt.

While merging the two components into one, it is necessary to use the Library Editor from Eeschema to move the first component so that the second does not end up on top of it. Below you will find the final .lib file and its representation in Eeschema.

The Python script presented here is a very powerful tool for manipulating both pin numbers and pin labels. Mind, however, that all its power comes for the arcane and yet amazingly useful Regular Expression syntax: http://gskinner.com/RegExr/.

From the KiCad project manager start the Pcbnew tool. Click on the 'Open Footprint Editor' icon on the top toolbar. This will open the 'Footprint Editor'.

We are going to save the new footprint 'MYCONN3' in the new footprint library 'myfootprint'. Create a new folder myfootprint.pretty in the tutorial1/ project folder. Click on the Preferences → Footprint Libraries Manager and press 'Append Library' button. In the table, enter "myfootprint" as Nickname, enter "${KIPRJMOD}/myfootprint.pretty" as Library Path and enter "KiCad" as Plugin Type. Press OK to close the PCB Library Tables window. Click on the 'Select active library' icon on the top toolbar. Select the 'myfootprint' library.

Click on the 'New Footprint' icon on the top toolbar. Type 'MYCONN3' as the 'footprint name'. In the middle of the screen the 'MYCONN3' label will appear. Under the label you can see the 'REF*' label. Right click on 'MYCONN3' and move it above 'REF*'. Right click on 'REF__*', select 'Edit Text' and rename it to 'SMD'. Set the 'Display' value to 'Invisible'.

Select the 'Add Pads' icon on the right toolbar. Click on the working sheet to place the pad. Right click on the new pad and click 'Edit Pad'. You can also use [e].

Set the 'Pad Num' to '1', 'Pad Shape' to 'Rect', 'Pad Type' to 'SMD', 'Shape Size X' to '0.4', and 'Shape Size Y' to '0.8'. Click OK. Click on 'Add Pads' again and place two more pads.

If you want to change the grid size, Right click → Grid Select. Be sure to select the appropriate grid size before laying down the components.

Move the 'MYCONN3' label and the 'SMD' label out of the way so that it looks like the image shown above.

When placing pads it is often necessary to measure relative distances. Place the cursor where you want the relative coordinate point (0,0) to be and press the space bar. While moving the cursor around, you will see a relative indication of the position of the cursor at the bottom of the page. Press the space bar at any time to set the new origin.

Now add a footprint contour. Click on the 'Add graphic line or polygon' button in the right toolbar. Draw an outline of the connector around the component.

Click on the 'Save Footprint in Active Library' icon on the top toolbar, using the default name MYCONN3.