How to Export Gerber and Other Production Files in KiCad

In this tutorial, we will study how to export Gerber files and other production files in KiCad. To manufacture a PCB, we send these Gerber files and production files of the design to the manufacturers. Manufacturers send this data to plotters and Computer Numerical Controlled (CNC) machines to fabricate a PCB.

We have covered how to route in KiCad in our previous article, now our design is ready for manufacturing.

Once the routing is completed, we can export our gerber files. But before generating the gerber files, it is important to make sure our design is perfect with the schematics and the PCB layout. So for that, we have created a checklist here.

We will cover the following topics in this KiCad tutorial:

• Checklist for generating gerber files
• Files required for PCB manufacturing
• How to export gerber files in KiCad
• How to export drill file in KiCad
• How to generate pick and place files in KiCad
• How to generate netlist file in KiCad
• How to generate BOM file in KiCad
• How to generate PDF in KiCad
• How to use GerbView in KiCad

Checklist for generating gerber files

There are three types of checklists you need to go through before generating your production files – BOM, schematic, and layout.

You need to confirm whether the bill of materials (BOM) which you have created is as per your schematic. i.e. the footprint, the component values, etc., should match the manufacturer’s part number.

Later, check the schematic values, whether the components are placed correctly and the quality markings are correct in the circuit. Once these are done the layout checks are complete. Now check whether you have placed all components required for manufacturing as per your design requirements. Also, there should be several other pieces of information in the fabrication drawing, which are marked in the image below:

Now let’s check how to write the details in these sections before generating the gerber.

Page settings

We have to add the details such as the name of the board, part number and required comments, etc. in the title block at the right bottom corner. To do that follow these steps:

• Go to Files > Select page settings  
• A window will popup

Whatever you type in this window will appear on the right bottom corner. In the same way, you can do the page setting in your schematic as well.

Add logo and text

You may need to add text on your board, such as the company name. To do that, follow these steps

• Select the silkscreen layer and select text icon > click wherever you need to add the text
• A window will popup

• Add the text in the popup window and set the dimensions of the text as per your requirements.

Now to place the logo of your company you will require a DXF file of the logo. If you don’t have a DXF file then you can use an image of your logo, and you can find online software that converts your image into a DXF file. You can use that as the logo for your board. To import the file:

• Go to files > Import > Import Graphics
• A window will popup

Browse and select your DXF file from the popup window, and set the dimensions of the logo in the import scale option.

Add dimensions

We need to mark the dimensions of the board and then we need to mark the dimensions from one mounting hole to another.  Also, the dimensions from the mounting hole to the board edge. Mark the dimensions in the fab layer. To mark, select the add dimension icon and select the fab layer.  

Move your cursor to the center of the mounting hole, a circle appears when it is at the centre of the hole. Now click on that and then click on the mounting hole on the other side and pull the dimension down.

Once all dimensions have been marked, the layout of your board in the fab drawing is complete. Check if the orientation of your connectors and all components are as per the datasheet.

Stack-up

You need to draw the stack-up in your fab layer using the add graphics tool and mark all the details in the stack-up using the Text tool.

The stack-up drawing should contain all the details related to the stack-up such as the thickness of each layer and the thickness of the top and bottom solder mask. The board details such as the total dimensions of the board, the thickness of the board, the tolerance of the board, etc., can also be mentioned. We get all this information from the stack-up report as we saw in the last tutorial. We need to fill all this information over here in the fab drawing again.

Fab details

Fab details are written on the fab layer. In the fab details, you can point out all the required specifications and information about the board. Details include the IPC class for the board material, the number of layers in the board, solder mask color, etc. Next, there are pads on the board – plated through-hole pads and non-plated through-hole pads. The pad tolerances should be mentioned as well.

Drill chart

There is also one more thing we need to mention in the fab drawing which is the drill chart. A drill chart describes the number of holes in the board, the different sizes of the holes, and whether they are plated or non-plated. It also mentions the number of vias being used and whether they are through-hole vias, blind vias, or buried vias along with the tolerances for all of the holes.

Check the generated files for common errors associated with Gerber files, such as incomplete files, empty Gerber files, unregistered layers, and so on.  It is easy to avoid such errors with the help of DFM and CAD tools.

Files required for PCB manufacturing

Once we are done with the design part, the gerber files should be generated for the manufacturer. Gerber is an open and universally accepted file format used to export PCB designs. In this demo, we are exporting the design in the gerber format.

The set of files that are required for the production of PCBs are as mentioned below:

1. Gerbers:
   1. Top etch
   2. Bottom etch
   3. Middle layer etch
   4. Top and bottom silkscreen
   5. Top and bottom paste mask
   6. Top and bottom solder mask
   7. Top and bottom assembly
   8. Fab details
   9. Board outline
2. NC drill
3. Pick and place(XY)
4. IPC 356 netlist
5. PDF:
   1. Top and bottom assembly
   2. Fab details
   3. All layers
   4. Top and bottom silkscreen
   5. Board outline
   6. Schematic
   7. Stack-up report
   8. Top and bottom solder mask (optional)
   9. Top and bottom paste mask (optional)
6. BOM

Gerber files are a set of files that contains production information of each layer of a PCB. Here we are using a four-layer board, so we need to create gerber for all the four layers. The top and bottom silkscreen, top and bottom paste mask, top and bottom solder mask, top and bottom assembly layer should be mentioned in the fab details. You have to create gerber files for each layer used in your design.

Next, we need an NC-drill file. An NC drill file gives information about all the holes required in the board. It will serve as an input to the drill machine to drill the required holes on the board.

Pick and place files are used by the machine to identify the location of the various components on the board using coordinates.

IPC-356 netlist files have information about the connections between various components. Once you create your netlist make sure that it matches with your schematic netlist.

Next, we will need PDFs. Generate PDFs for top and bottom assembly, fab details, all the layers of your board, the schematic, and a stack-up report.

Finally, we need a BOM. The BOM consists of all of the components which will be used in our board and the manufacturer part numbers that will help the PCB manufacturer in identifying the components.

Now you know the files that you need to generate to manufacture your design. Let’s check how these files are generated in KiCad.

Read more: PCB Design Output Data that a Manufacturer Requires

How to export gerber files in KiCad

Now let’s generate the gerber for our design. To do that,

• Select the Plot icon  from the toolbar on the top
• A window will popup

Select the required settings in the popup window.

Required settings in the popup window:

• Select the Gerber from Plot format
• Select the Output directory where you want to save the file. – First, make a separate folder for gerber in your files.
• Select all the layers for which you need gerber files, from Included layers. If you are creating a 4 layer PCB select all four layers. Apart from that, select “forward paste”, “stop paste”, “bottom paste”, “forward silk”, “bottom silk”, “forward solder mask”, and “bottom solder mask”. Here we want an “Edge cut layer” which is the actual boundary of the PCB and fab layers, which are“front fab” and “bottom fab”. These are the minimum number of layers we require for generating gerbers
• Select the General options that are required.
• Deselect Plot footprint values because normally we don’t plot values of the components of the board. But we plot the references so select Plot footprint references.
• Select  Exclude PCB edge layer from other layers and Exclude pads from your silkscreen
• Choose  Select Use Protel filename extensions in Gerber options

Once these settings are done, we are ready to plot our gerber. Now Click Plot.

Your files will be saved in your selected folder. It will be displayed in the “Output message” section in the above popup. Don’t close the popup!

Also read: How to Export Gerber and Production Files in Altium Designer

How to export drill file in KiCad

Now we need to create the drill file. Once you complete generating the gerber click on Generate Drill File 

A new window will popup.

Choose all required settings from the window.

Required settings in the popup window:

• Select the Output folder where you want to save the file.. Save the drill file in a separate drill folder.
• Make sure you have selected “PTH and NPTH in single file” (recommended)
• Select the Drill units as “Inches”

Once the settings are done, click Generate Drill File. 

We need to create a map file as well, which gives you the dimensions of holes in the drill chart. Click on Generate Map File for that.  Save the map file in the gerber location. After the files are saved, you will receive a notification in the Messages box about the saved file.

How to export pick and place files in KiCad

• Go to File > Fabrication Outputs > Footprint Position (.pos) file
• A window will popup:

The popup window:

Required settings in the popup window:

• Select the Output directory where you want to save the file
• Under Format select ASCII. which will give you the drill locations and selecting CSV will give you drill locations in Excel format.  If you want, you can generate both the files.
• Select the Units in inches
• Select Files. If you select Single file for board, all the top and bottom components will be in a  single file. To generate two different files for top and bottom layers, select Separate file for front and back.

Once the settings are done, to generate the position file click the Generate Position File. 

After the files are saved, you will receive a notification in the Messages box about the saved file.

How to export netlist file in KiCad

Go to file > Fabrication Output > IPC – B – 356 netlist file

Once you finish this step, a window pops up in which you can choose the location to save the file. Select the location and the file will be exported to the location.

How to export BOM file in KiCad

Go to file > Fabrication Output > BOM

Here we need to follow the steps similar to the ones we used for netlist generation.

How to generate PDF in KiCad

Steps to generate PDFs are similar to the ones we used while generating gerber files with some changes needed in plot settings.

• Select Plot icon from the toolbar on the top menu
• A window will popup:

Required settings in the popup window:

• In Plot format, select PDF
• Select the Output directory where you want to save the file
• In  Drill marks, select the actual size
• You can select all the layers you selected while generating gerber files.

Click Plot

Generate PDF for schematic

Now go to your schematic window.

• Select Plot   
• A window will popup

Required settings in the popup window:

• Select the Output directory where you want to save the file
• Select the PDF option from the output format
• Choose Schematic size in Page Size.
• Select the Output mode either color or black & white.

Now click Plot All Pages. 

Your PDF will be created in the selected folder. We’ll require a stack-up as well. Save the PDF of the required stack-up along with the schematic PDFs.

How to use GerbView in KiCad

Now as per this document, all of the files are created. We now need to check whether the BOM which was generated by us, was properly generated before it goes to manufacturing. To view all your gerber files:

Go to the Project manager of the KiCad > Tools > View Gerber Files

Now, the Gerbview screen will appear. You would need to see whether the gerbers and the drill file generated was properly created. For that:

Go to file > Open Excellon Drill File 

Then browse and select your drill file from the location where the drill file was saved and click Open.

You will be able to see many green dots on the screen. This tells you the locations of all the holes and their dimensions. Let us see whether all the holes fit within our board. For that, we need to open the edge cut layer from the gerber.

• Go to file > Open Gerber file 

• Select the gerber of the layer which  you need to view

Here we need the edge cut layer.

Also, open the map file from the gerber files, so that you can view the dimensions of the holes in your Gerbview.

You can see the green dots which are the map of drill holes. There is a blue rectangle that covers the entire board set up which is the Edge cut layer. The drill map is displayed below the board.

Similarly, you can select each layer from the gerber and can check whether all the files in the board are following the layout design. For an overlapping view, you can also select several layers at a time. For example, we selected the top layer of our board as depicted in the image below:

Once your files are verified, you can send the files for manufacturing. Send the files in a single zipped compressed file format. This will ensure that there are no errors during the transmission of the files.

Also read, how to export Gerber files in Altium Designer.

To summarize, we have detailed the deliverables required for board manufacturing. You will require the gerber files, the drill chart of the map, the drill file, the placement file, along with the IPC Netlist. You need to check and verify each of your layers and the edge cuts carefully. If you find errors in Gerbview, you’ll need to go back to PCB new, fix the errors in your layout and then re-generate gerbers using the plot tool. It is easier to fix them at this point as it won’t be easy later on. Hope you found this tutorial to be helpful.

If you want to validate the KiCad design files and get a real-time cost estimate based on that, check out our KiCad PCB plugin. This will enable designers to get an instant quote without quitting the KiCad user interface.

KiCad Design Guide

8 Chapters - 98 Pages - 110 Minute Read

What's Inside:

• Creating a component symbol library
• Setting up board parameters and rules
• How to route differential pairs
• How to place of components

Download Now