KiCad

From Mech
Jump to: navigation, search

--JasonMantzouranis 14:47, 22 July 2013 (CDT)

Contents

Overview

KiCad is a schematic and printed circuit board (PCB) layout editor, which lets the user design a PCB schematic, convert it to a PCB layout and then obtain the gerber files that are then sent to a PCB manufacturer. This page contains a basic step-by-step guide on how to use KiCad to design a PCB from start to finish.

  • Advanced Circuits will manufacture a 2-layer PCB for 33$ and a 4-layer PCB for 66$. (student deal)

Guide

  • To create a new project, click File -> New -> Blank, and give it a name.

Creating the Schematic

1. Click on EeSchema (the first of the main 5 buttons on the project window) to start your schematic. (A pop-up window will appear saying that the file was not found, click ok)

2. To save your project, click File -> Save Whole Schematic Project.

3. To add a component to your schematic, click on the third icon on the right hand column of icons, and browse through the pre-existing libraries.

4. To add your own (project-specific) library, click Preferences -> Library -> Add, and choose your library, which has been automatically created when you saved the project in step 3. It starts with the name of your project.

5. It is likely that the pre-existing libraries will not have all the components that you will need, so to create your own component, open the library editor by clicking on the icon at the top of the pen and book.

6. Click on the second icon at the top to select the library you want to work in. You can click File -> Save Current Library As to save it as a new library. It is a good idea to choose the library that KiCad created, which is named after the project, in order to have all the customized components for the project together.

7. Now, you can load a component from another library, and then click the 7th icon above to use it as a starting point to create your new component, making sure you give it a different name/reference.

8. The icons on the right are the editing tools. To add a pin, click on the second icon on the right and then click where you want to add it. Fill out the name and number fields, and select an orientation such that the empty circle, to which any traces must connect, points away from the component.

9. When you are done, click on the first icon above to save the current library.

10. Now you can close the library editor window, and add the component you just made to the schematic.

11. Create and/or add any other components you need to your schematic (Resistors, capacitors, diodes, etc are in the existing devices library). You can move components around, rotate them and edit them by right-clicking on them and selecting the appropriate option.

12. After placing your desired components on the schematic, click on the 5th icon on the right to add a trace. Click on where you want to start the trace, then click again once whenever you want to turn, and double-click on the ending point.

13. To add a ground or power port, click on the 4th icon on the right and select your desired element.

14. Make sure that everything is connected as necessary.

Suggestions and Additional Points

  • Instead of making all the necessary connections with wires on the schematic, which can get confusing if there are too many of them, you can click on the second to last icon on the right to create a net name, which you can place at whatever points you want to be connected. If you want 3 different pins to be connected together, you can place the same net name on all these pins, making sure that the small square to the bottom left of the name is on the pin.
  • You do not need to connect all the power and ground points with traces. Using the ground/power ports from step 13 tells KiCad that they are connected.
  • To create a plain text label, create a net name as described in the previous point, and then right click on it and change its type to text.

Converting your Schematic into a Layout of a PCB

1. In the schematic window, click the ".net" icon above, then click "Netlist" on the window that appears, and save it in your project folder. A window may appear asking you to annotate the schematic, click yes and then "Annotation" and then ok. Now close the annotation window.

2. Click on the third to last icon above that says "Run CvPcb" to associate footprints to the components on your schematic.

3. An error message will pop up the first time you do this in a project. This is normal. Click ok. All your components are listed on the left, and all the available footprints in pre-existing libraries are listed on the right. To add your own library, click Preferences -> Libraries -> Add.

4. Select each component on the left and double-click the corresponding footprint on the right. (Surface mounts start with SM). You can preview the footprint by selecting it and clicking the fourth icon above.

5. If the footprint for any of the components is not available, select a similar footprint for now. You will get the chance to edit it and make the exact footprint later. In this case, is a good idea to choose a footprint that has more than the number of pads that you need; it is easier to delete pads than to insert them.

6. When you are done, press File -> Save, and close the window.

7. Go back to the schematic file. Click on the second to last icon above to run Pcbnew. The window for the layout of the PCB will appear.

8. Click the ".net" icon above, browse to the netlist file you saved previously, and read it.

9. Now all the footprints of your components have appeared, with grey lines indicating where connections need to be made. (these are suggested connections based on where your components are located, so you do not need to follow them exactly; there are many more possible ways to make the connections as you will see when you move footprints around and the grey-line network changes)

10. Move the components into the working area so that they are not all on top of each other.

Creating the PCB Layout

1. It is now time to make the footprints for any components that did not have pre-existing footprints.

2. Click on the 5th icon above to start the Module Editor.

3. Click on the 6th icon above to create a new module/footprint.

4. You can choose an active library (first icon above) if you already have one, otherwise click on the third icon above to save the module into a new library.

5. Now start making the module. If there is a similar module available in a pre-existing library, load it into the module editor, and make any necessary adjustments. Using the graphic lines/shapes on the right for any outlines, and add all the necessary pads using the second icon on the right. Use the right-click to access any necessary settings, including pad sizes/shapes.

6. When you are done making the footprint, make sure you have named and labeled it correctly, and save it into the active library. You can now close the module editor.

7. Back in the layout editor window, click on Preferences -> Library -> Add to add the new library that you have created in the module editor.

8. Now, right-click on the footprint that needs updating and click on Footprint -> Edit Parameters -> Change Module(s) -> Browse, and select the footprint you made. Press ok in the exchange module window. You should get a message saying that the change was ok. Now click close. The footprint will have been updated. It is a good idea to read the netlist again to ensure that the pads are still connected the way you want them to be.

9. Once you have all the footprints you need, it is time to make the connections.

10. Place and orient the footprints in the approximate way that you want them.

11. Click on the "Add traces/vias" icon on the right, and connect all the pads that should be connected. You will only be able to draw traces between pads if and only if the pads are connected in your schematic. If you need to update your schematic, go back to the schematic window, make any necessary changes, create the netlist again, and read the netlist from the layout window.

12. When drawing traces, click on the pad that you want to start from, then click once for whenever you want to make a 45 degree angle to turn, and click once at the ending pad. KiCad will neither let you cross traces that are on the same level of the board nor let you cross vias. Try to keep traces as short as possible, and it is good practice to only have 45 degree angles.

13. To create a via in order to continue in another level of the board, start a trace and right-click wherever you want to create the via. This will cause the trace to continue on another layer of the board so that you can cross traces that are on other layers.

14. The number of connections remaining to be made is visible below, under "Unconnected". Also, you can use the second icon on the right to click on something and light up everything that should be connected to it.

15. When you have made all the connections and added all the labels that you want, choose the "Edge Cuts" layer and draw the outline for your PCB.

16. Now, click on the icon above with the ladybug to perform a check based on the design rules, and click on start DRC. Fix any errors that appear.

Suggestions and Additional Points

  • You can change the size of the tracks and the vias by clicking Design Rules -> Design Rules above. You should not make the trace width any smaller than 0.007 inches.
  • All the layers are visible on the right. The layer you are currently working on has a blue arrow to its left. To start a trace from another layer simply click on that layer before starting the trace.
  • Try to use as few layers as possible, ideally no more than two copper layers, and, whenever possible, keep all components on a single layer. To change the layer of a component, right-click it and click Edit Parameters.
  • You can prevent text from appearing in your final design by right-clicking on it, selecting edit and changing the display setting to invisible. You can also change the orientation in this way.

Acquiring the Gerber Files

1. Click on File -> Plot, choose your output directory, select all the layers that you have used that you want on your board, and click Plot. This will convert your design into the Gerber files needed by the manufacturer.

2. Now click Generate Drill File, choose your output directory, and click drill.

3. You now have all the files that you need to send to your manufacturer in a ZIP file to build your PCB.

Suggestions and Additional Points

  • Advanced Circuits will manufacture a 2-layer PCB for 33$ and a 4-layer PCB for 66$. (student deal)
  • Before submitting your order, it is a good idea to use the free PCB design file check that Advanced Circuits provides at this link. They will email you back with the results, listing any problems; some problems are permanent and need your attention, while others are automatically fixed.


Additional Resources & Tutorials

Personal tools