Skip to end of metadata
Go to start of metadata


What is KiCad?

KiCad is an open-source, multi-platform EDA (Electronic Design Automation) package. It captures your schematics, build your parts libraries and lay out your PCBs. It runs under Windows, Linux and, experimentally, on Apple OSX.

What is the official name for KiCad EDA?

The official name of KiCad is KiCad.

Where can I get KiCad?

Please look at the Installing Kicad page.

Which version should I download?

You have a choice between stable release or nightly builds. They are based on two different source code branches: stable and product, respectively.

Stable branch is outdated and lacks recent features, but as the name indicates - there are almost no significant bugs there, as it has been thoroughly tested.

Product branch is under very rapid development, so it literally changes every day. Because of that, sometimes minor difficulties are introduced, as the code is briefly tested. You must be ready to face some issues (and save your project frequently), but KiCad developers are known to react promptly to serious problems. If you find any anomalies, please report them on the "KiCad bug tracker".

It would be very appreciated (and I think also enriching your knowledge) to use the product version. This way you benefit from the freshest add-ons, and also help us to drive KiCad to a stable release, which is our current primary goal. The best way to do so, is to build it from "source". Please note that new features in the "product" branch required changes to the file format, so it is not backward compatible with the "stable" version.

Where can I find a KiCad tutorial?

A very good KiCad tutorial  is available from the KiCad Help menu of KiCad itself. Alternatively, the same tutorial can be found in the doc folder (or the tutorial folder for older versions) of the installed KiCad tree or in the kicad-doc package.

Renie S. Marquet created a mini tutorial with a simple RS232 adapter on his site. This is only in Portuguese but, it has many pictures, including the tools to use. Perhaps it will help you. Renie's tutorial is basic, but covers all steps from zero to creating the schema and pcb.

Where can I get the documentation in my native language?

Please take a look at Documentation page. All KiCad manuals have been translated in several languages but naturally the most updated ones are the English manuals.

Is this the official KiCad wiki? used to be the Official International KiCad wiki. Now is the official site KiCad.

Can I help with KiCad development?.

Of course you can. There is a developer's mailing list that focuses on the development of KiCad. All major communications happen here.

If you are interested in helping out with the programming behind KiCad, read over the mail list archive:

Joining the launchpad team named "kicad-developers" is the gateway onto the mailing list.

Why does KiCad try to connect to the Internet?

KiCad does not connect to the Internet. It uses sockets for client-server communications from eeschema to pcbnew. Some firewalls misinterpret socket access as Internet access. Because of this, when you click on a pin in eeschema, the corresponding net is highlighted on the board.


How do I output other netlist formats?

Such as the standard EDIF netlist format?

EESchema has a NetList plugin system. eeschema creates a generic (intermediate) NetList output (generic list of components, list of pins and list of nets). The plugin reads this generic file and creates the new NetList format, and eeschema can automatically run this plugin. This plugin is very easy to create because the generic NetList output is designed to make such a plugin straightforward. A sample is given, with comments to create new plugins. Currently this sample creates a PADS-PCB NetList format. (Note, this format is not very well tested.)

The new eeschema NetList tool has up to 8 user programmables entries to launch these plugins. The first time you use it, you must open the NetList dialog box, open the blank page (the last entry) and :

  • Give a title (ex: PADS-PCB)
  • Give the command line to launch the plugin (e.g. /usr/lib/kicad/plugins/netlist_form_pads-pcb or d:/kicad/bin/plugins/netlist_form_pads-pcb.exe)
  • Run the NetList generator (like the other formats).

This version is unstable because the user interface may be modified, and the documentation is not yet updated.

If you use this feature, please report any problems.

Another work-around is the Edif to KiCad translator.

How do I copy and paste from one schematic to another?

To copy a block from a schematic, open your previous schematic, select the block to copy and in pop-up menu (right click), and choose Save Block (or delete block but DO NOT SAVE YOUR OLD SCHEMATIC).

Within the same window, use the menu to open the new schematic and press the Paste button (tool bar). The block will be pasted into your new schematic.

To copy components from a schematic, select the components you want to copy/cut using the right mouse button to select copy/paste from the pop up menu, and then press the escape key. That will return the selected components to the starting point. Switch to the other schematic and paste the component.

If you want to copy icons, you must deactivate the "auto pan" option in preference menu.

As an alternate option, you can enter the block command with holding the shift key (copy) or shift+ctrl keys (delete) ( See doc eeschema 2.2.2)

Non-homogeneous multi-part modules?

Part-A is the default. Load the part, right click on it, select edit->unit, and change the part-A to part-X

For Non-homogeneous multi-part components, do not forget to check (in library editor) the "Parts are Locked" option for these components.With this option, Eeschema does not change the part selection when it annotates the schematic.

What are Markers in the Locate dialog?

Markers are from the ERC - and show where there is an error.

How to apply a completely re-annotated schematic to a board?

This is an operation that requires careful attention. The main reason is that two separate steps occur in the re-annotation path where a .cmp-file is created. The .cmp-file contains the one-to-one associations between component and module.


  1. Prior to re-annotation, start Cvpcb and do the save operation. This will ensure that the .cmp-file fits.
  2. Now, back in eeschem, perform the desired re-annotation operation.
  3. You may think that a new Vcpcb session is needed, because of false component-module association. But currently, there is no mechanism to get things right here, instead open pcbnew (or get to it) and then:
  4. Load the netlist. Tick "Module Selection": Time stamp and then start loading. No error report should be shown here. The magic is in the .cmp-file, which is however no longer OK for any Cvpcb operation.
  5. In order to allow correct Cvpcb operation, a new .cmp-file must be generated from WITHIN pcbnew: File->Fabrication Outputs->Component File.

Ready. In fact, you can repeat step 1, and you can see, that annotations are right now. As a reminder: for any subsequent re-annotation, a .cmp-file must have been saved here, in cvpcb.

How does one import the .stf file into a schematic and what does it do?

.stf files are generated by CVPCB (stuff file). It consists of a line for each component, giving the name of the footprint according to its reference.


If the U3 component was assigned the footprint 14DIP300, the generated line is

comp “U3” = module “14DIP300”

In EEschema svn version (r1064) a button was added to back-annotate Footprints from a "Stuff File" to the schematic. It is NOT a backannotation of reference designator changes in the board. Instead, you can use this with a new project. Insert some different, frequently used components in eeschema. After doing a first iteration with Cvpcb, you will no longer need to assign footprints to new compontents in eeschema as long as you copy components.

Use case: The process for keeping the schematic up to date would be:


  • enter starting schematic
  • output initial netlist annotated with ref designators


  • read initial netlist
  • add missing footprint info
  • output modified netlist & stuff list (with footprint info)


  • the modified netlist could be used to start initial placement
  • save working pcb


  • back-annotate footprint info from "stuff file"
  • modify schematic if desired, maybe change a few footprints
  • output updated netlist (containing footprints)


  • import updated netlist with new components, optionally removed unused parts no longer in netlist
  • place new components


Schematic symbol creation and editing.

There are two ways to save the part - one to RAM and the other to the library. What is the use of this?

If you save your modifications into RAM, you can go back to your schematics and see the result of it. If you don't like it, you can still "roll back" to the previous situation. If you save your part into the library, there's no way back any more.

If you change a part in the library - what do you have to do to update a part in a schematic?

In fact, it's done automatically for you, when you press the button to save the modified part into RAM. The only thing which apparently doesn't work yet (release 2006-08-28) is the update of the fields. But you will see your modified drawings at least.

How do I create a new parts library?

In EESchema select the icon "Go to library editor". It opens with a clear view and Libedit: No Lib header. Then select "New Part" icon ... go through simple questions and you are ready to draw your own part.

Once you've created it - use "Create a new library and save current part into". Than select location and give a filename. For example, I made my own directory at /home/xtc/kicad/libs_xtc - where I save all my personal lib files.

When You finish editing our part - save and close. Then in EESchema you have to add this new library to library list. You do this in "Preferences > Libs&Dir > ADD (button)" - browse to find your library and it will be added to list. From now on - your part will be visible in place_part dialog list.


This allows the user to see which parts are contained in each library of schematic symbols. This can speed up the creation of a schematic project by allowing the user to directly load a library and go directly to a specific part. If the part needed can not be found in a library it can be created in LibEdit (described above) or look for libraries on the internet.


CVPCB is for associating footprints (modules) with schematic parts.

If you create a new component in LibEditor and you immediately assign a footprint to it (Icon "Edit component properties -> Footprint filter -> Add), then CvPcb will automatically filter the footprints. For example, enter "14*" in Libedit will make CVPCB propose to you 14DIP-ELL30 and 14dip300 (assuming you have selected "Display the filtered footprint list for the current component").


How can I use relative coordinates?

Press the SPACE-key at the position where you want your relative coordinates origin. Now you can read the relative coordinates at the status bar, at the right of the absolute coordinates.

How do I manually route a PCB?

Manual routing is straight forward. You don't even need to have a schematic. Start a new project then select PcbNew. Right click in the drawing area and select Select Working Layer. Set working layer to edges PCB. Select Line tool from RHS and draw PCB outline.

Now right click and select working layer copper. Select Add Tracks and Vias tool from RHS toolbar. Draw your tracks. You can place a via by pressing the V-key.

To change track size you need to create a new track type. From the main menu select Dimensions then Tracks & Vias. Fill in the values for your new track size and press OK. Your new track type is now in the tracks drop down box.

If you have a schematic then start Pcbnew as normal. Choose the Add Tracks and Vias tool from the RHS toolbar and click on a ratnest. Be sure you are working on the components layer for single sided PCB with SMD components. If you are using default colors all tracks should be red. If you get green tracks, you are working on the copper layer.

How do I un-route a PCB?

In Pcbnew select Miscellaneous/Global Deletions and in the dialog that pops up check the 'delete tracks' option then click the Accept button.

How do I connect a copper fill to a net?

One method is while in the fill zone mode you move the pointer inside the track, right click and choose "select net". Then you can do "fill zone" from anywhere outside the track.

You could also use the 'net highlight' tool. This took me forever to figure out actually. I would expect some option in the Fill dialog to select a net to connect to. (This appears to have been fixed in newer versions of Kicad, where you can select the net you want from the fill options dialog.)

How I can move SMT components to the solder side

With "flip module" in the pop-up menu. You can also press the "F" key to do the same thing.

How do I change the grid size inside the library editor?

Right click and choose grid select.

What's the difference between printing and plotting PCB layouts?

New in pcbnew, in the print menu, is a new scale option: "Accurate scale 1", which prints the board at scale 1.00, but does not keep exactly the board position in page. The Approx. scale 1 (old option) keeps the board position in page and is intended to produce documents for users. The real scale depends on printer, margins, pcbnew page size and real paper size, and is intended primarily for documentation purposes.

There is also a change in page margin management, both in eeschema and pcbnew. Margins reduce the user drawing area for 0.4 inch (10mm) on left, right, top and bottom sides. In older versions, there was no margin, and the schematic drawings were drawn at reduced scale (smaller than scale 1), to fit in page + margins. In the new version the scale is near scale 1, and the page setup in the print dialog window is removed.

There are two reasons for this:

1 - The print dialog window page setup option is buggy under Windows (this is a wxWidget problem, not a KiCad problem). Therefore, the user could not really change the margins values, or the printer paper size.

2 - Boards now can be printed at exact scale 1, and the necessary margins reduce the user drawing area. (old versions drew the board at nearly 0.95 scale mainly to fit in the usable paper area, which is the paper size - margins).

The margin setup dialog is not currently available (currently, margin values are hard coded), but i hope i put this feature in a next release of KiCad.

How can I print a PCB mirrored?

There are two ways to do it:

First, Pcbnew has a mirror option in File/Plot menu (Postscript format). Secondly, modify the board by the "Flip block" command ( Block command: select the whole board, right click and select flip bock).

How do I make PCB mounting holes?

A hole can be seen as a footprint, with only one pad. You can add one (or many) footprint (right toolbar, button "add module") like the "1pin" footprint existing in library. Edit the pad in order to have the correct size (pad diameter and drill value).

How do I make a ground or power plane?

  • Select Add Zones icon
  • Trace the limit of the zone. You do not need this step if you have defined the edges of the board on the edges Pcb layer and if your zone is going to follow these edges.
  • Place the cursor on a pad belonging to the net you want for the plane, (GND or any other)
  • Click right on the zone an select fill zone

Note that the pads belonging to this network must already be connected by tracks, else the design rule test will see them not connected. The addition of the zone must therefore be done at the end.

How do I add vias to a zone?

  1. Select the option 'Add tracks and vias'
  2. Left click at the place in the zone where you want the via.
  3. Without moving the mouse, right click and select 'Place Via'
  4. Without moving the mouse, right click again and select 'End Track'

Now you have a via... Quick route: hit keys x, v, End.

How do I rotate a footprint by a specific angle (e.g. 45 degrees)?

  1. Right click on the module you want to rotate
  2. Select Footprint ... (Component) -> Edit to open the Module Properties dialog
  3. Here, in the Properties tab, select User in the Orient section
  4. Now you can enter an arbitrary angle in the Orient (0.1 deg) box. You have to multiply your angly by 10, e.g. enter 450 for 45°

How do I make coils for planar cores?

I make Switch Mode Power Supplies. I use a sandwich of two ferrite cores around one ore more PCBs to make a transformer. How do I make make arc tracks and spiral coils ?


Does Pcbnew have an autosave facility?

This function exists in PCB editor. Better consider buying UPS.

How can I make my own default footprints?

A convenient method is to create .equ files and use the automatic association command with cvpcb. This is because for many components, the "standard default footprint" depends on the value. Diodes, Polarized Capacitors are an example. For most of the components you can use an SMD version for a project and later the "standard" version for another project.

With a .equ file you can have a "standard default footprint" which solves this because the .equ files can be specific to a project.

here is an example ( see kicad/modules/devices.equ) '680K' 'R4' '1M' 'R4' '2,2PF' 'C1' '3,3PF' 'C1' '74HC00' '14DIP300' '74LS00' '14DIP300' '74HCT00' '14DIP300'


  • .equ file gives the standard default footprint from the component value and can be created by your favorite editor. The editor replace command can very quickly change the 14DIP300 to SO14E for a SMD based project...

In kicad/modules/ you can find some .equ files.

Do not forget to configure cvpcb to select the .equ files you want.

Why doesn't the 3D viewer work?

You must ensure the color depth of your graphics card is set to 24 or 32 bits.

In Linux you can edit /etc/X11/XF86Config-4

and change the line

DefaultDepth 24

Why are the 3D models not inside the .pretty repos?


How can I see the solder mask layers?

Solder mask and other technical layers are only displayed in high contrast mode. Enable high contrast mode by clicking the icon that looks like a small palette, bring up the layers management toolbar (the icon just below with a green and red square) and select the layer you are interested in.

How do I draw a keepout area for the solder mask?

Just draw a zone in the desired soldermask layer. This will remove the solder mask on the zone.

Module editor

PCBnew also contains the module (foot-print decal) editor where you can change and create modules.

There are two default text strings on a new decal; What are they called and what are they for?

The first string is the part “Designator”. In the module editor this is a module name under which it is stored in the library. As the module will be put on the board this name will be replaced by the name under which this part occurs in the schematic/netlist, for example R1.
The second string is a part “Value”. In the module editor this string has a default content: VAL **. After inserting the module on the PCB this will be replaced with the value that has been assigned to that part on the schematic/netlist, such as 100k.

Under Module properties there are attributes (normal, Normal+Insert, and Virtual) what are they for?

These attributes are used primarily to determine whether an element have to be put on the module positioning list. In the case of automatic assembly, especially in the case of SMD elements, this list can be used to program the inserting machine.
These attributes means exactly:

  • Normal - This module is a normal element, which is mounted on the board during its assembly. All of THT (through hole) and SMT (surface mount) elements are classified to this group. Elements with this attribute set are not included in the module positioning list.
  •  Normal + Insert - an element that has all the properties that have an element with the attribute Normal, but in this case it is possible the automated mounting, so it’s placed on the module positioning list. As a rule, only SMD components should be set to this attribute, because there is a possibility for automatic insertion. There are also machines for mounting through-hole components, but their popularity is now quite low.
  • Virtual - an element that occurs only on the board and is a part of it - cannot be separated from the PCB. To this group belong all the pads, which the wires are directly soldered to, all edge connectors allowing to place the boards in the slots; uncovered test points for testing and measurements, etc.
How do I place vias in the module editor?

Some packages, such as QFN, require thermal vias in a particular arrangement. How do I do that with KiCad?

Some documentation and tested/suggested footprints may be found here:

What do the different numbers mean in the gridding drop-down. i.e. the "10" in "Grid 10.0" and "100" in "Grid 100.0"

Auto router

How can I force the auto-router to work on only one layer?

I have discovered I can force the auto-router to work only on the copper side by selecting copper for both layers in the Select Layer Pairs dialog.-

NB: This possibility was inopportunely forgotten in certain versions, but should be restored soon (version of June 2008).

Note 2: I've found that it's possible to force the auto-router to work only on the copper side by setting "Numbers of layers" to "1" in Preferences -> General options. I think this works regardless of version.

MUCS-PCB Auto-router


Where to get MUCS-PCB


Steps to Produce Gerber output files

Library maintenance

Where can I get other component libraries?

There is a library folder in the files section of the group for just this purpose. Feel free to create your own sub folders and contribute your work.

How do I import libraries from other PCB programs?


I just uploaded "exp-kicad-lib.ulp" under the rm_sharkey_libs folder in the files section of the group. This is a ULP script to export EAGLE PCB parts to KiCad. To use, open EAGLE PCB, load the library you're interested in, into the library editor, and then run this ULP script.

It has one bug that I have not gotten around to fix yet (I did not write this script). The bug is in selecting the correct layer for the pads. However, even in it's current state, you can manually edit the KiCad output and touch up the pads using search and replace, just compare with a similar "good" KiCad lib and you'll see what has to be modified. Aside from that, it does a pretty good job of exporting.....maybe if someone has some time they could tweak this script a bit to make it work better.

(Mike Sharkey)

I've wrote a simple script for exporting pcbnew libs from Eagle CAD libraries but don't know what kind of restrictions eagle's librarians apply to their libraries. I've uploaded about 200 converted libs on our ftp server and using them now. Please look at it and say me what are you thinking about. I think it will be good if that libs be available to all KiCad users.

Link: <--- broken link

(Dmitri N. Sytov)

Large Converted Library

A large number of symbols and footprint converted from an Eagle Library can be found:

Link: (Download All)

User beware that compatibility with KiCad should to be verified: long pins names, valid file names, geometry, pin assignments, etc

In particular, KiCad chokes on the "m-pad-2.1.mod" file merely because of its file name. Work-around: rename to "m-pad-2-1.mod"; then that library works fine with KiCad.

How can I generate an array of pads fast?

I've uploaded one perl script I made to the yahoo files section. (jpdborgna folder). I append the readme file of that.

The function of this simple script is to generate pad arrays, the symbol and the module, for using with KiCad. These arrays can be used for pins connectors, for prototyping areas or for any other component which requires many pads uniformly distributed. Given the simplicity it can be easily modified to make other functions.

Import Methods

Se also "Other related tools" for aditional format converters.





What are the steps involved in making a change ( ECO) in a design?

There is more going on that just creating a new netlist and importing it -: the .stf file may be involved - how are changes to the footprint handled? This dosn't quite work as documented in (2006-08-28)

Is there a forward and backward eco process going on? Is there inter process communication going on between eeschema and pcbnew? I read that there was - but what is it doing?


Links to other KiCad related tools

NameDescriptionurlProgramming language
CmpToCsvConvert the Kicad CMP file into a CSV file. (run under windows). source code
DIP generation helperCreate library simbols from XML
drillfile.zipCreates Excellon drill files from a KiCad board, separated into PTH and NPTH drill files.
Eagle2kicadConverts Eagle to KiCad ULP
Edif to KiCad translatorAn Electronic Definition Interchange Format (EDIF) parser which allows exportsfrom one EDA schematic capture system (such as OrCad) for import into another (such as KiCad)
fpedFped is an editor that allows the interactive creation of footprints of electronic components. Footprint definitions are stored in a text format that resembles a programming language.
GerbAnalyseCrude Gerber File Viewer / Analysator. Can read and analyse Gerber247d and Gerber247x without macros and some drill files, and display them in a very rough manner (without apertures and so on)., kdupe2-1.plAn update to the KDupe perl script for panelizing a board.
KicadComponentsListToCsvUtility to create components list in CSV. platform "C" sources.
KICAD lib managerList, join, export an delete libraries (PCB an Schema) from commandline
KiCADLibModA small GUI tool which can load, save and merge KiCAD *.lib and *.mod files. Footprint generator that is capable of creating pin arrays.
Kicad PCB Diff/patchShow differences between two kicad boards.
KiCAD utilsGenerate eeschema libraries, parse KiCAD files (eeschema, eeschema library, netlist), generate Russian GOST specifications for schemes and do other actions.
KiLibManFreeware library manager for KiCAD (non-free? source code available)
LIB2LIBisualization, edition and comparison of eeschema libraries 5.0 (r)
LibmanA simple library manager GUI. (pcb and sch)
LibTool_Kicad.zipTool to convert orcad lib to kicad lib without dos commands 
Max2BRDConversion from MAX (PCBs OrCAD 9/10) to .BRD (KiCAD).
MOD2MODVisualization, edition and comparison of PCB library modules 5.0 (r)
OrKiOrcad 2 Kicad Pcb Converter
PCadToKiCadPCBPCad (Protel) PCB Board or PBC lib conv., C
pcbmultiplyerGraphic utility to multiply/panelize boards.
Pinarray paNxNCreate simbols and footprints from command line. Conectors, prototype zones, etc.
QuickLibQuickly build your library symbols for KICAD
RSMegl2kicadBoard conversion from Eagle to Kicad 5.0 (r)
Search KicadlibSearch for modules in various sites
SeteditText Editor for programmers, with basic syntax highlight for .sch, .brd, libs and mods
TokicadConversion from Tango to Kicad (schematic and PCB) 5.0 (r)
TTConvConvertion scripts: Orcad2Kicad (pcb), Dxf2Kicad, Kicad2Dxf
VerlibPCB library visualization 5.0 (r)
XML4PCBXML is one way to transfer a Printed Circuit Board (PCB) data basebetween Software Applications. This projects starts with an exportfrom PCB123 and creates a Kicad brd file.

Links to other KiCad modules and libs Tools, modules, 3D, tutorials (in Portuguese).

Posting Guidelines

The group is very young so there is as yet no group policy for posting guidelines., However, as a start I recommend we adopt the standard netiquette guidelines in Section 3 of RFC 1855 which can be found here:

PCB manufacturers that accept KiCad gerber files

Ernesto Mayer S.A, Buenos Aires, Argentinasent gerber files by email, everything was exactly as expected
American Circuit Technology, CA, USAAble to email through quotation system everything worked out OK.
Advanced Circuits, Inc., CO, USAsubmitted files by internet, everything was Ok
Circuitos Impresos de Morelos, SA de CV., Morelos, Méxicosubmitted files by e-mail, PCB Ok
DPSKé Mesto nad Váhom, Slovak Republicsent gerber files by e-mail
Electrocir, Spainsent gerber files by email
Inarci S.A Aires, ArgentineSent gerber files by email. A 4 layer PCB, 7x7cm, with a BGA FGG320. Everything was Ok.
Gatema, Czech Republicsent gerber files by email
PCB4Less Grove Village, IL, USAsubmitted files by internet, everything was quickly produced and as expected
PCBexpress, OR, USAsubmitted files by internet, everything was exactly as expected
PCB Train, UKsent gerber files by email, everything was exactly as expected
San Francisco Circuits, Inc. Mateo, CAsubmit files by internet or email (added on their own request)
Sierra Circuits Inc., CA USAsubmitted files by internet, quality job and free solder mask and silkscreen for both sides
Sunstone Circuits LLC, OR USAfiles by email, and upload
Southdown Circuits Ltd.(website offline)Arundel, West Sussex, UKsent the pretty much default configured Gerber files, been told they are OK
PCBcart them the gerber files with a quick description of each file, they review it and let you know if they spot any errors.
PCB-POOL.COMhttp://www.pcb-pool.comGermanyuploaded gerber files in their web interface, everything was OK (exact Gerber/drill settings here)
Propox files sent via e-mail, required wider VIAs, they sent spec on request; board was very precise. (Do not use without www - it does not work.)
Hackvana via mail,
NICEVT and drill files sent by e-mail or upload in their web interface, PCB OK.
TePro and drill files upload in their web interface, PCB OK.

Who wrote this FAQ?

This FAQ was written and is maintained by Ian Bell. Contributors include:

How can I contribute to the FAQ?

Feel free to add/edit/translate required information to the KiCad wiki. (KiCAD wiki on SourceForge no longer exists, please refer to:

Where do I submit new/updated libraries?

How can I contribute custom footprints to the project?

Is KICAD Libraries ( an official project site?

Where is the submission link? Go on, click on the language flag of your choice on top of the page. A window pop-ups which explains how to submit your libraries.

Is it best to submit the additions/changes individually, or to integrate them into the appropriate pre-existing library?

Is there a good reason to split up KiCad into 4 Sourceforge projects?

How do I install new/updated libraries?

How exactly do I install a KiCad schematic or footprint library I downloaded from or some other web site? Is there a menu option where I can type in the URL of the library and KiCad will download and install it in the right place"KiCAD Tutorial: Adding Libraries -- How to add new KiCAD libraries to your projects" [1] via [2]

Which version should I download?

You have a choice between stable release or nightly builds. They are based on two different source code branches: stable: and product, respectively.

Stable branch is outdated and lacks recent features, but as the name indicates - there are no significant bugs there, as it has been thoroughly tested.

Product branch is under very rapid development, so it literally changes every day. Because of that, sometimes minor difficulties are introduced, as the code is briefly tested. You must be ready to face some issues (and save your project frequently), but KiCad developers are known to react promptly to serious problems. If you find any anomalies, please report them on the "KiCad bug tracker".

It would be very appreciated (and I think also enriching your knowledge) to use the product version. This way you benefit from the freshest add-ons, and also help us to drive KiCad to a stable release, which is our current primary goal. The best way to do so, is to build it from "". Please note that new features in the "product" branch required changes to the file format, so it is not backward compatible with the "stable" version.


  • No labels