How to convert Altium Designer files to KiCad and vice versa

Altium and KiCad are two mainstream EDA (Electronics Design Automation) tools for schematic capture and PCB design. Both have their advantages and disadvantages, but users may need to convert a PCB design made in Altium into KiCad, or a KiCad design into Altium. 

Updated for KiCad 9

In this guide, we will break down how to convert and import Altium schematic and layout files to KiCad and vice versa. For help importing Altium libraries to KiCad, you can refer to our guide here for a quick and tool-less method.

Can Altium read KiCad files and vice versa?

The short answer is yes; however, care has to be taken to ensure accuracy and compatibility. 

Migrating tools and need to take your projects with you? Perhaps you need to work on a design made by someone who used a different tool. In either case, you’ll need an efficient and accurate way of converting between the two formats. As with any file conversion, make sure you verify the accuracy of the result and be aware of the limitations.

Importing Altium Files into KiCad

Since KiCad 7, KiCad has vastly improved support for importing files from other EDA tools, including Altium CircuitMaker and CircuitStudio. From the table below, we can see that apart from the project file, KiCad 8 and greater support the main Altium file formats: Schematic import (.SchDoc), PCB import (.PcbDoc) and library imports, including symbols and footprints. Schematic and PCB layout support was added in KiCad 7, but for best performance and fewer bugs, we strongly recommend upgrading to the latest KiCad release (which is KiCad 9 at the time of writing). Update: KiCad 9.0.3 now supports PCB Project file (.PrjPcb) import, including support for flat schematics. You can download the latest version of KiCad through our gateway here.

How to import schematics from Altium to KiCad

1. 1. Open KiCad and create a new project.
    
2. 2. In the Schematic Editor, go to File -> Import -> Non-KiCad Schematic...
   
   
    
3. 3. Select the Altium .SchDoc file you want to import and select Open. For hierarchical designs, choose the top-level schematic, and KiCad will automatically pull in the sub-sheets.
   
   
    
4. At the same time, KiCad will create a project library for the symbols used in the schematic, netlists and preserve the hierarchy in multi-sheet designs, as can be seen in the example below. Compared to the original in Altium, they are virtually the same.
    

Altium schematic in KiCad after import

Original schematic file in Altium

Note that KiCad 7 and 8 do not support flat structure or non-hierarchical schematics. For these, each page needs to be imported one by one, or you can use KiCad's Altium project import feature available from KiCad 9.0.3, which is explained here.

How to import PCB layout from Altium to KiCad

1. 1. Open the PCB editor (Pcbnew) in KiCad
    
2. 2. Click File -> Import -> Non-KiCad Board File...
   
   
    
3. 3. Select the .PcbDoc file you wish to convert and click Open.
   
   

KiCad will then import the Altium design. From the example below, we can see they look identical.

Even with this MiniPC design, the Altium to KiCad import has no problems, importing the 3D model as well.

How to import Altium project files to KiCad (v9.0.3+)

New to KiCad version 9.0.3 is the feature to import Altium project files (.PrjPcb) into KiCad directly. This includes a quicker way of importing a whole project, especially in the case of flat schematics which require importing one by one in previous workflows. 

1. 1. Go to File -> Import Non-KiCad Project... -> Altium Project...
   
   
    
2. 2. Select the Altium .PrjPcb file you wish to import, then click Open. In the next window, select where you want to export the converted files and click Select Folder. This should be an empty folder.
   
   
    
3. 3. In the next window, match the Altium layers to the KiCad layers as appropriate. Alternatively, you can use the Auto-Match Layers button. This is accurate in most cases, however, it will depend on your specific design. Be sure to verify the layers afterwards.
   
   
    
4. 4. KiCad will then import the schematic and PCB layout files in an Unsaved state. Verify the correctness and click Save to permanently add them to the project as KiCad .sch_kicad and .pcb_kicad files.
   
   
   
   
   
   

Importing KiCad files into Altium Designer (v24.6+)

Whether you need to import KiCad schematic files or PCB layout files into Altium, Altium has always supported KiCad imports, but older versions can only import KiCad 6 files. To seamlessly import KiCad 7, 8 and 9 files, use Altium Designer 24.6 or later. 

How to Install the KiCad Importer

The KiCad Importer is an Altium extension, so an official paid Altium license is required. Make sure you are running genuine Altium software with an active license. 

1. 1. Open Extensions & Updates... in the top right corner
   
   
    
2. 2. Switch to the Purchased tab
   
   
    
3. 3. Under Software Extensions you will find a selection of EDA importers, exporters and third-party tools. Find the KiCad Importer and click the download icon.
   
   
    
4. 4. Restart Altium once downloaded

How to use the KiCad Importer extension

1. 1. In Altium, go to File -> Import Wizard 
   
   
    
2. 2. Under the list of file types, click KiCad Design Files then click Next. The KiCad Importer supports the following file types:

• KiCad pro Files (*.pro)
• KiCad kicad_pro Files (*.kicad_pro)
• KiCad sch Files (*.sch)
• KiCad kicad_sch Files (*.kicad_sch)
• KiCad kicad_pcb Files (*.kicad_pcb)
• KiCad lib Files (*.lib)
• KiCad kicad_sym Files (*.kicad_sym)
• KiCad kicad_mod Files (*.kicad_mod)

1. 
   
   As we can see, both older and newer KiCad file formats are supported by the importer tool, as well as KiCad symbol and component libraries.
    
2. 3. Open and add all the KiCad files that require importing to the list then click Next. Project, schematic, layout and library files can be added at the same time. 
   
   
    
3. 4. In the next window, map the KiCad layers to the Altium layers for your project. Ensure these are correct to avoid translation errors. The other settings are not important.
   
   

FPGA Board Example Import

Let's try converting an FPGA KiCad design into Altium. Preview the design using the online KiCad viewer link below:

Preview FPGA board online

This is the schematic after import, which looks pretty good.

However, the PCB import fails - uh-oh. Looks like Altium still has some improvements to make.

RP2350 Example Import

Let’s try converting a simpler board, specifically the Pico 2 based on RP2350.

Preview RP2350 Pico 2 board online

This is what the schematic looks like after import:

From general appearances, it looks like the importer did a good job. However, always be sure to run the ERC check after importing and resolve them as necessary.

The imported PCB layout also looks fine, however, the DRC rules have not been imported. In this example, the trace width rule has not been imported. 

You may also encounter a bug where two .PcbDoc files are generated after import. It appears there is no difference between the two, so feel free to delete one of the copies.

Both tools have their unique set of advantages and are suited for different products and scenarios. From Altium’s advanced features and industry-standard capabilities to KiCad’s free, open-source flexibility, whether you are migrating tools, collaborating across platforms, or just need to use a specific feature, accurate conversion of file formats between tools is important. Knowing how to efficiently convert between formats and the limitations is essential for seamless transitions. 

Now that you know how to import projects, check out our article on how to bring your symbols and footprints from Altium to KiCad

About NextPCB

NextPCB provides PCB manufacturing and assembly services, focusing on reliability without breaking the bank. With 5 factories in China and over a decade of quick turnaround electronics manufacturing from prototype to mass production, NextPCB serves over 160 countries around the world, pairing dependable electronics hardware with exceptional service. 

As a Platinum sponsor of KiCad and host of KiCon Asia, the only KiCad conference in the East, NextPCB is committed to supporting the KiCad development team and it’s vibrant community with development resources, manufacturing support, organizing events and amplifying awareness to make innovation accessible to everyone. Download Kicad here.

About the Author

Carmen Zheng, content creator at NextPCB

With over eight years of experience in China's PCB manufacturing industry, Carmen has built a diverse expertise spanning operations, technical support, sales, content creation, and community engagement in electronics manufacturing, assembly, and EDA software. A UK native with a Master's degree in Electrical and Computer Engineering, her innate curiosity for how things are made and unique Western-Eastern perspective enable her to bridge cultural and technical gaps while amplifying Chinese manufacturing expertise globally.

LinkedIn