KiCad 6: Peter’s BIG review 

KiCad is arguably the world’s best open-source printed circuit board CAD program. 

It’s been around for almost 30 years. Its community has been growing steadily both in terms of end-users and contributors.

KiCad’s importance as a fully-featured alternative to closed-sources PCB design tools has grown since version 4 came out in 2015. That’s about the time that I committed to using KiCad, after playing around with other commercial and open-source alternatives. I was so impressed with KiCad that I decided to teach others how to use it.

I’m pleased with my choice. As an educator and electronics hobbyist, KiCad has everything I need, without the limits.

When KiCad 5 came out in July 2018, KiCad presented an image of maturity. In my opinion, KiCad 5 was a significant milestone in its history because it signified a new approach to the development of the tool. 

The core development team, composed of members that give most of their time to the project, is supported by community donations and CERN.

KiCad 5 raised KiCad as a serious contender in the PCB CAD space. KiCad 5 was powerful enough to be used in corporate engineering departments as well as by hobbyists. 

After more than two years since the publication of version 5, version 6 is visible in the horizon. I expect that KiCad 6.0 will become a reality sometime in the second or (more likely) third quarter of 2021.

I wanted to take a deep dive in KiCad 6 and report on my findings in this article. As I am writing this post, it is middle of January 2021, a few months after a feature freeze was declared in late 2020.

After months of playing with the nightly builds containing the work in progress towards KiCad 6.0, I decided that it was time to take a closer look.

I felt confident that my findings would be useful to anyone wondering about KiCad 6.

In this article, I document the most important new and updated features coming in KiCad 6.0. In many cases, I make a Kicad 6 vs KiCad 5 comparison so that you can see these changes in context.

For my testing, I use the nightly build of KiCad, which is currently labelled “5.99”. The nightly development builds are snapshots of the development branch of the KiCad repository. 

I’m running KiCad 5.99 on an Ubuntu 20.04 virtual machine. 

If you want to learn how to install the nightly build, look for instructions at the end of this article.

I am comparing KiCad 5.99 (which will morph into KiCad 6 later this year) with KiCad 5.1.9 running on an Ubuntu 18.04 virtual machine.

Please note that I will be using the designation “KiCad 6” in this article, even though I did my testing on the KiCad nightly release designated “KiCad 5.99”. During this article’s writing, I updated my copy of KiCad 5.99 almost daily to make sure I worked with the latest available code.

KiCad 6 impressions in a nutshell

KiCad 6 includes several big changes and many smaller ones. 

Many of those changes are under the hood, designed to improve reliability and performance and set the stage for the future. 

Of course, there are numerous changes in the front end, the user interface, that will impact how you interact with KiCad.

New file format

KiCad 5, Eeschema file segment.

$Comp

L power:GND #PWR07

U 1 1 5EF25186

P 7150 2850

F 0 "#PWR07" H 7150 2600 50  0001 C CNN

F 1 "GND" H 7155 2677 50  0000 C CNN

F 2 "" H 7150 2850 50  0001 C CNN

F 3 "" H 7150 2850 50  0001 C CNN

1    7150 2850

1    0    0    -1  

$EndComp

KiCad 6, Eeschema file segment.

(symbol (lib_id "power:GND") (at 181.61 72.39 0) (unit 1)

    (in_bom yes) (on_board yes)

    (uuid "00000000-0000-0000-0000-00005ef25186")

    (property "Reference" "#PWR07" (id 0) (at 181.61 78.74 0)

      (effects (font (size 1.27 1.27)) hide)

    )

    (property "Value" "GND" (id 1) (at 181.737 76.7842 0))

    (property "Footprint" "" (id 2) (at 181.61 72.39 0)

      (effects (font (size 1.27 1.27)) hide)

    )

    (property "Datasheet" "" (id 3) (at 181.61 72.39 0)

      (effects (font (size 1.27 1.27)) hide)

    )

  )

The new S-Expressions notation file format is more verbose and takes more disk space, but it is much easier to read, edit by hand, or edit programmatically.

Symbol libraries are also moving to S-Expressions.

The new file format means that the main KiCad apps can soon be complemented by an abundance of plugins and extensions that can introduce new features. Think of plugins that can import PCB projects from other CAD programs or wizards that can create a new KiCad project within milliseconds to save you time.

The new file format is not backward compatible. You will not be able to open a KiCad 6 file with KiCad 5, but you will be able to import KiCad 5 projects and convert them to KiCad 6.

Another important attribute of the new file format for Eeschema is that schematic symbols will be embedded to the file (not linked, as they currently are). This means that in KiCad 6, Eeschema files will be self-contained and will not depend on libraries. You will be able to publish and share these files and be sure that they will open properly on other people's KiCad 6 instances. No more "[??]" indicating broken links to symbol libraries.

Tools and Workflow

If you already know how to use KiCad 5, or even KiCad 4, you will find that the KiCad 6 individual apps also known as “tools”.

You still have the main KiCad app, which allows you to launch the individual apps: 

• Eeschema, 
• Pcbnew,
• the editors for custom symbols and footprints, 
• and auxiliary apps like the Gerber file viewer, the image converter, the calculators and the schematic worksheet editor.

Some of these tools, like the Convert Image tool, are virtually unchanged. 

Most tools, however, contain small or significant improvements without changing their traditional look and feel.

The KiCad workflow is also streamlined without changing its fundamentals. You will still create PCBs by iterating through Eeschema and Pcbnew, but the two tools are now better integrated.

That’s good—no need to re-learn KiCad. 

User interface

Eeschema in KiCad 6

When you start Eeschema in KiCad 6, you will immediately see the familiar KiCad 5 organisation of the menus and toolbars, even with the new icon set for the buttons.

Let’s look at some of the most significant changes.

Schematic editing paradigm upgraded

A frequent complain voiced by KiCad users, old and new, is the way the the schematic editor reacts to user events. Prior to KiCad 6, Eeschema implemented an idiosyncratic editing paradigm that is unlike not just how things work in other CAD applications, but in other applications in general (word processing, email, etc).

Here's an example of how weird KiCad 5 (and older) can be. Open or create a new KiCad 5 project, open Eeschema, and click on any symbol. When you click on the symbol, information about it appears in the info bar at the bottom of the Eeschema window. It looks like this:

Now, after you click on the symbol and its information appears in the status bar, move the cursor away from the symbol, and press the "E" key (which should bring up the symbol properties window). Normally, you would expect that because this symbol is the last thing that you clicked on, it would still be selected, waiting for your next action. You should be able to click on the "E" key and see the properties window.

Right?

Well, no. Eeschema in KiCad 5 and older doesn't work like that. When you click on a symbol or other item the only thing that happens is to show its information in the status bar.

The click does not select the item.

The position of the cursor selects the item.

This is totally weird, and I have seen first hand how this confused me, and my students. Even Pcbnew in KiCad 5 does not work like this. Pcbnew in KiCad 5 works as expected, where you click on an item and the item becomes selected so you can then perform actions like to move it or bring up its properties (try it!).

I am ecstatic to report that KiCad 6 Eeschema has finally changed its editing paradigm so that it works as expected.

In KiCad 6, when you click on an item in the schematic, the item is visible selected (you can see a blue outline around the resistor in my example below), and remains selected even as your mouse pointer moves elsewhere, and until you click on something else.

With the item selected, you can use any of the available commands to do things such as move, drag, rotate, edit, copy, etc. 

There are even some functions that will work with multiple selected items, such as move, drag, and copy.

Considering how much time people spent working on schematics, this new editing paradigm for Eeschema in KiCad will go a long way to reduce friction for new and current users alike.

My hope for a future enhancement: the ability to multiple select symbols of the same time and bulk assign a value. For example, select all LED current limiting resistors and set the same value in one or two clicks.

Back-import and footprint association file

Looking at the top toolbar I noticed that one missing button is the back-import.

This button facilitated the importation of changes from Pcbnew into Eeschema via the Symbol Footprint Link file (or "Footprint association (.cmp) file"). To make this work, you would have to first export this file from Pcbnew, and then import it into Eeschema. 

This function is now handled by Update Schematic from PCB under the Tool menu.

In KiCad 6 Pcbnew, you can still export the Symbol Footprint Link file, except that it is now called "Footprint Association (.cmp) file" and is found under the File menu. Similarly, in KiCad 6 Eeschema, you can import a cmp file via the File menu.

One thing to note here is that terminology can still cause some confusion. The same file (cmp) is known as "Footprints Assignments file" (KiCad 6 and KiCad 5), "Footprints Associations File" (KiCad 6 and KiCad 5) or "Symbol Footprint Link File" (KiCad 5). In KiCad 6, the CMP file has one less name.

Schematic Setup

Under the File menu, you will now find a brand-new dialogue box: the Schematic Setup. You can also access the Schematic Setup dialogue via the top toolbar, where a new button appears right next to the save button.

The Schematic Setup dialogue box contains several new configuration options. It also hosts configuration options that existed in KiCad 5 but organised differently.

In KiCad 5, most settings were accessible via the Preferences dialogue box under the Preferences menu item. The same Preferences dialogue box is still available in Kicad 6. 

Here are the items that stand out in the Schematic Setup dialogue box:

General - Formatting

Under the General group, you will find the Formatting and Field Name Templates dialogues. 

The Formatting dialogue allows you to set your preferred default text sizes, symbol line thickness, junction dot size etc. Most of these options are available in KiCad 5.

General - Field Name Templates

The Field Name Templates is a feature inherited from KiCad 5 verbatim, except that in KiCad 5 it appeared in the Preferences dialogue box. 

Interestingly, in the nightly build version of KiCad 6 that I am testing at the moment (KiCad 5.99 of January 12, 2021), the Field Name Templates dialogue appears under both Schematic Setup and Preferences. 

But, they are not the same! The difference between these two identically named field is the scope. 

The Field name Templates in Schematic Setup have a project scope, whereas the one in the Preferences field has a global scope. 

To test this feature, I have created a Field Name Template via the Schematic Setup dialogue box (which has project-level scope), and the Preferences (which has global scope). 

These templates appear in the Symbol Properties field list, and in the Symbol Fields list, I can type custom text.

You can open the Symbol Properties dialogue by doing a right-click on a symbol and selecting “Edit”. 

You can open the Symbol Fields dialogue box by clicking on the button that looks like a spreadsheet in the top toolbar.

Text substitution

Text Substitution is a brand-new feature to KiCad 6.

With text substitution, you can create a variable that contains arbitrary text and display this text anywhere in the schematic where text can appear. 

The new text substitution feature is also available in Pcbnew.

Here’s a quick demonstration of how this works.

First, you can define your text variables in the Text Variables pane under the Project grouping of the Schematic Setup dialogue box.

You can see an example in my screenshot titled “6. KiCad 6 - Text Variables” (above).

Next, create something that contains text, such as a net label or a text item. 

To display the value of the text variable, use the notation “${name_of_variable}”.

The result is that KiCad will replace all variable placeholders’ occurrences with the variable’s value, as defined in the Schematic Setup dialogue.

You can also use syntax conventions to control how the text looks. There is a handy Syntax Help window with more information.

Text substitution even works in the title block, in symbol properties and hierarchical sheet properties:

Here is an example of how text substitution works with sheets and sub-sheets. In the screenshots below, first I have created a sub-sheet with the name "Sample-subsheet". In the sheet properties, I have created a new field, with name "SubsheetResistorValue" (apologies for the boring names). 

In the sub-sheet, I have created a resistor, and in its value property I have referenced the field "SubsheetResistorValue". KiCad will resolve the property reference with its set value.

Bye-bye netlist button

Before KiCad 5, the link between Eeschema and Pcbnew is the Netlist.

In KiCad 4, every single time that you made a change to the schematic, you had to create a new netlist file manually and (again, manually) import it into Pcbnew.

KiCad 5 provided a more seamless way of linking the two apps, but you could continue using the Netlist method as if you were using KiCad 4.

In KiCad 5, the Netlist button was still present in the top toolbar. My people used to it from the KiCad 4 years (myself included), continued to use it even though it was not necessary.

In KiCad 5, the correct way to import a schematic from Eeschema into Pcbnew was via the "Update PCB from Schematic" button. This method is also available in KiCad 6, and it remains the proper way of importing a schematic into Pcbnew.

In KiCad 6, the Netlist button has been removed from the top toolbar.

You will find the Netlist export and import functions under the File menu in Eeschema and Pcbnew respectively.

In KiCad 6, the netlist button is missing in an effort to simplyfy the workflow. You can import schematic data (and updates from already imported data) to Pcbnew by clicking on the new “Update PCB with changes made to schematic” (found in the top toolbar in Pcbnew). 

Let's recap. 

In KiCad 6, you can update Eeschema with changes in Pcbnew and vice-versa with these two commands:

Both are available under the Tool menu in either app. 

Interactive delete tool

A new tool that is designed to make it easier to edit complicated schematics is Interactive Delete. 

You will find it under the Edit menu (but I think it is useful enough to eventually have its own keyboard shortcut and button in the top toolbar).

Once you select the Interactive Delete Tool, the mouse pointer changes to an eraser. As you hover the pointer over a schematic item (such as a symbol, wire, text label etc.), that item is highlighted. 

This way you can be sure that the item you are about to delete is the correct one. Just click to delete the highlighted item. This is a new productivity feature that will reduce the dreaded “Doh!” moments to a minimum.

Edit text and graphics

KiCad 6 gives you the ability to customise almost every aspect of the way that schematic items look like. Colours, line widths, orientation, and decorations are all configurable.

Under the Edit menu, you will find the new “Edit text and graphics” tool which allows you to edit such attributes in bulk. 

The tool allows you to do this in two steps:

As with the Interactive Delete Tool, the Edit Text and Graphics tool is another example of how KiCad’s development focuses on providing ways to make us more productive.

Another new tool that I’ve been hoping for is the Change Symbols tool. You’ll find it under the Edit menu.

This tool allows you to change the symbol used for multiple schematic objects at once. 

Similarly to the Edit Text and Graphics Properties tool, the Change Symbols tool provides a way to select a specific class of items. Items can be matched by reference designator (for example “R?” will match all items with a designator that begins with “R”), a value, and a library identifier. 

Once you have selected the class of items you want to change their symbol, you can specify the new symbol identifier.

In the example below, I am changing the symbol of all resistors (using the “R?” expression) to the resistor’s US symbol.

Context menu

The context menu in KiCad 6 Eeschema is more powerful then ever before. Multiple new functions are available with the click of a button. Several of them are available in KiCad 5, but were accessible elsewhere and with more than one click, or through a shortcut (such as the Rotate function).

For example, in KiCad 5, to edit the value of a symbol you would need to drill into the Properties submenu. In KiCad 6, you can click on the Edit Value function at the root context menu.

In KiCad 5, the Rotate function is also available via a shortcut or through the Orientation submenu. In KiCad 6 it is available at the root of the content menu (all shortcuts work as expected). Most items in the KiCad 5 Properties and Orientation submenus like in the root context menu of KiCad 6 Eeschema.

The Open Documentation function (KiCad 5) is changed to Show Datasheet (KiCad 6).

Here are the KiCad 6 and KiCad 5 versions of the context menu in Eeschema, as it applies on a symbol:

Functions like Move and Drag remain. New ones are added:

• Align Elements to Grid.
  
• DeMorgan Conversion.
  
• Change and Update Symbol.
  
• Show Datasheet.
  
• Edit Page Number.
  
• Select All.
  

Finally, in KiCad 5 Eeschema context menu, the last function is "Close". I never understood the purpose of this function, since to close the context menu you simply click outside the menu. In KiCad 6, the "Close" function is removed.

Enhanced bus handling

In KiCad 6, signal bus handling is vastly improved. Both the user interface used to draw and wire busses, as well as the underlying infrstructure of naming the nets and groups of nets that belong to a bus, are all improved.

Let's begin with the UI. In the screenshot below, I have drawn a bus line. The, I have called the Line Style dialogue box (you can double click on the bus, type "E" as the mouse pointer is over the bus, or use the context menu and select "Properties"). It looks like this:

The ability to configure the visual aspects of a bus means easier to read schematics. For example, you can set your data bus to be red, and your address buss to be blue. In KiCad 5, busses did not have properties at all.

While the ability to visually customise a bus is useful, it represents only a small set of upgrade in the way that busses work in KiCad 6. The bulk of the new features is in the way that nets can be bundled in a bus.

In KiCad 5, it is possible to create a bus that can "carry" signals that are labeled according to a simple convention. Here is an example:

In the example above, I show a typical way in which a bus is used in KiCad. There are many more. In the example, I have a connector on the left side with 4 pins. I have used local labels to name the nets that are connected to the pins. The labels are:

• DATAOUT0
  
• DATAOUT1
  
• DATAOUT2
  
• DATAOUT3
  

I have given membership of those nets to the bus by using the label construct "DATOUT[0..3]". An alternative way would be to use bus entry wires for each of the nets.

On the right side of the example I have placed a second connector. I have labeled the nets that connect to the left connector pins like this:

• DATAIN0
  
• DATAIN1
  
• DATAIN2
  
• DATAIN3
  

Just like with the left connector, I have used the label construct "DATIN[0..3]" to give the DATAINx nets membership to the same bus.

KiCad is smart enough to work out the relations between the nets:

• DATAOUT0 connects to DATAIN0
  
• DATAOUT1 connects to DATAIN1
  
• DATAOUT2 connects to DATAIN2
  
• DATAOUT3 connects to DATAIN3
  

This is a classic example of when you would use a bus, instead of simply relying on net labels.

In KiCad 6, the bus label notation for net membership is far more powerful. You can now use a wide range of label constructs. You can see the valid syntax below:

You can find the Syntax Help window by double-clicking on a bus and then click on the Syntax Help hyperlink.

In the list of Bus definitions from the Syntax Help window, the first two are inherited from KiCad 5, and the rest are brand new. All of the new bus definitions use curly brackets, similar to how we can now define text variables.

Let's look at some of them (drawing from the syntax help examples):

• Mix nets of arbitrary names. For example: {dat1 dat2} would  create nets dat1 and dat2 inside the bus.
  
• Nets that don't have a numerical suffix, such as {SCL SDA} or {DP DM}.
  
• You can have named buses by adding the name on the left side of the opening curly bracket: USB1{DP DM} would create nets USB1.DP and USB1.DM.
  
• Mix nets with different prefixes, and even combine pre-KiCad 6 bus definitions with new definitions : {D[0..7] LATCH} would create nets D0, D1, ..., D7 and LATCH.
  
• You can even use markup symbols, such as "~" for overbar and "_" for subscript.
  

With all these convenient ways to add nets to a bus, you may be wondering how to extract individual wires for each embedded net so that you may connect to to other parts of the schematic graphically, as opposed to using the net labels.

Let me show you a neat new trick.

Here's a bus, with a fairly elaborate net definition:

The bus definition creates a total of 6 nets. To extract individual net wires from the bus, you can use the new "Unfold from Bus" context menu option, drill down to the net that you want to extract, and then draw it as you wish. It looks like this:

As you can see, it is not easy from create buses that bundle together a large number of nets, and just as easy to unfold them graphically. As a consequence, the bus definitions can become long and convoluted. Display the entire definitions in the label attached to a bus may make the schematic look too busy.

In KiCad 6, there is a new way to deal with this complexity. Under the Tools menu, you will find a new option: "Bus Definitions". This will bring up a dialog box in which you can create a bus alias that may contain one ore more alias members. An alias member is a simple of complex net definition.

See my example below, in which I have replaced the complex bus definition from my previous example with a single bus alias named "MEM" that contains two simpler bus definitions. The end result is the same, electrically speaking, but the schematic is easier to read.

To attach a bus alias to a bus, simply create a label with the name of the bus alias in between curly brackets. The member nets are now part of the bus, and they can be unfolded via the context menu.

Pcbnew in KiCad 6

Many of the changes found in Eeschema are also found in Pcbnew. For example, there is a brand-new Board Setup dialogue box which is the equivalent of the Schematic Setup dialogue found in Eeschema. 

Also, Pcbnew in Kicad 6 contains many improvements in the layout drawing capabilities and brand new productivity and convenience features. 

Let’s dive in for a closer look.

(New) right toolset

The most significant visual change in Pcbnew of KiCad 6 is the redesigned right-side toolset.

This toolset contains an updated toolbar and three new groups of widgets: Appearance, Presets, and the Selection Filter.

In the screenshots below you can see a side-by-side comparison between the KiCad 6 (left) and KiCad 5 (right) right toolset in Pcbnew. I have marked the elements of the KiCad 6 Pcbnew right toolset with their names. I will refer to these names in the discussion that follows.

In KiCad 5, the Pcbnew right toolset consisted of a toolbar with various drawing tools and the Layers Manager. The Layers Manager contained two tabs: Layers, useful for selecting the active layer on which editing took place, and Items, useful for hiding and showing layout times.

In KiCad 6, the right toolset is turbo-charged. 

It retains the vertical toolbar, updated with new icons and a few multi-tool buttons (more about this later). 

It also retains the Layers tab in the renamed Appearance box. The Appearance box takes up most of the real estate of the right toolset, and it also contains the Object tab (which inherits the functionalities of the old Items tab and adds a few new ones), and the new Nets tab. 

The Nets tab provides widgets that allow you to control the visibility of individual Nets or Net Classes.

Appearance: Layers

In KiCad 6, the Layers tab works similarly to its namesake in KiCad 5, but it is much improved.

When you select a layer to activate it, this layer’s elements will come to the foreground, and everything else will recede in the background. This makes it much easier to identify elements in a busy circuit.

The foreground/background visual effect is enhanced significantly using the Layer Display Options group’s radio buttons.

See this example:

I have selected the back copper layer (“B.Cu”) from the Layers tab and checked the Dim option from the Layer Display Options group. You can see the effect of this. The blue tracks that belong to the back copper layer stand out, while everything else is dimmed. Even with the busiest of circuits, you will not have much trouble identifying the elements that belong to the currently active layer.

Appearance: Objects

The Objects tab allows you to control the visual aspects of layout objects such as tracks, footprints and ratsnests. 

You can control the opacity of tracks, vias, pads and zones, as well as the visibility and colour of 15 other objects.

Here’s an example:

In this example, I manipulate the opacity of the pads. In the left screenshot, I decrease opacity, while in the right I have increased it. In both screenshots, you can also see a net depicted with a custom green thin line.

Appearance: Nets

The Nets tab allows you to control the colour of nets and ratnests. 

Again, I’ll explain how this works with an example. 

See the screenshot below:

The arrows show the points of interest. 

You can show or hide each net and set its colour individually. In this example, I have set the colour for the GPIO39 net to green, and D1-Pad2 net to red. In the Net Colors radio buttons under the Net Display Options group, I have selected “All”. 

The effect of this is that the colour that I have assigned to these nets is applied to both ratnests, tracks, and pads that belong to these nets.

With the tracks, the custom net colour (red) and the net display options are overriding the default layer colour. This way it is possible, for example, to assign a colour to significant nets, such as the Ground net, so that I can see all traces that belong to this net regardless of which layer they are on. 

That’s neat.

Presets

The Layers, Objects and Nets tabs contain lots of widgets that allow you to fine-tune how your PCB layout is displayed. 

Eventually, you will find your self working with a regular set of configurations. 

This is where the Presets drop-down comes in handy. 

With a single click, you can assign your desired setting to the widgets of all three tabs. There are several defaults presets to choose from, but you can also save your custom settings.

Here’s the expanded Presets menu, showing the default presets:

Here’s how powerful Presets is. In the screenshot of the left side (below), all layers and objects are enabled.  In the left screenshot, I have selected the “All Copper Layers” preset. This preset makes everything disappear except for the objects in the front and back copper layer (tracks, pads, zones, and vias).

Clarity with a single click.

Selection Filter

The last new addition to the right toolset in KiCad 6 Pcbnew is the Selection Filter.

In my time playing with KiCad 6, this is probably the productivity tool I use most often.

The Selection Filter allows you to control which type of object will respond to your mouse clicks or group selections. 

Let’s look at an example of. See the two screenshots below.

In the left screenshot, I have enabled all objects. When I do a right-click on an area where a footprint and a track overlap, Pcbnew will ask me to choose which object I want to select.

In the right screenshot, I have selected on “Tracks” in the Selection Filter. When I right-click on the same area as in the left screenshot, Pcbnew will immediately display the context menu for the track, since it “knows” that I am only interested in tracks.

The Selection Filter also works with multiple selections. See below:

With only Tracks selected from the Selection Filter options, I click and drag to select several tracks (left screenshot). When I release the mouse, the selected track segments remain highlighted. Pcbnew did not ask me for clarification, nor did I have to worry about accidentally moving footprints or other elements.

The last component of the right toolset that I will describe in this article is the vertical toolbar. 

It contains all of the buttons found in the right toolbar from Pcbnew in KiCad 5, with a few additions.

You can see them here, side by side:

The icons are updated, and modern-looking, with several multi-tool buttons and one new function added. 

The multi-tools allow you to access functions that were previously accessible via the menus. Here’s a list:

You can see these multi-tools below:

Vertical toolbar: Rule areas

The vertical toolbar in KiCad 6 Pcbnew contains a brand-new button: the Rule Area tool.

With the Rule Area tool you can create arbitrary keep out areas. You can set the properties of the Rule area to keep out tracks, vias, pads, copper pours or footprints. You can also restrict the application of the rule area to specific copper layers, and give it a name.

The name will help you identify violations in the DRC report.

In the screenshots below I show a small keep-out zone.

First, I try to draw a track inside it (see left screenshot). The push & shove router will correctly prevent me from doing so. Notice that my mouse pointer is well within the keep-out zone, but the track is only drawn up to the edge of the zone.

Second, I place a mounting hole footprint inside the keep-out zone. I did not get a warning in real-time, but when I ran the Design Rules Check, a violation was produced:

Board setup

Pcbnew now has a comprehensive Board Setup dialogue box. You can access it from the File menu and via a button in the top toolbar.

Unlike with the Schematic Setup in Eeschame, the Board Setup in Pcbnew is not new. It was present in KiCad 5. However, in KiCad 6, Board Setup is significantly expanded to contain many new configuration options and provide a new “home” for configuration dialogues that were organised differently in KiCad 5.

For example (see screenshots below), in KiCad 5, the Board Setup dialogue contains the Text & Graphics pane in the Layers group. It allows you to set visual default properties for items such as lines and text. In KiCad 6, the same pane is titled “Defaults” and contains additional configuration options.

As is evident from the screenshots below, the new Board Setup dialogue contains many more configuration options than it did in KiCad 5.

Let’s look at these options as they are grouped.

Board Stackup

The items in the Board Stackup group are not new. 

The KiCad 6 “Board Editor Layers” pane is accessible by clicking on the “Layers” group header in KiCad 5. 

As you can see in the screenshots below, the two panes are almost identical. 

However, one difference stands out: In KiCad 6, you can add custom layers by clicking on the “Add User Defined Layer”.

The new Board Stackup group contains two brand-new panes: Physical Stackup and Solder Maker/Paste (see below):

In Physical Stackup, you can set the board’s thickness and the individual characteristics of each board layer, including the type of material used, its thickness, and the colour to depict it in the editor. 

In Solder Mask/Paste, you can set attributes such as the solder mask clearance and its minimum bridge width. These are numbers that you can obtain from your preferred PCB manufacturer and help ensure that your PCB design will be manufacturable.

In the Text & Graphics group, you will find the Defaults and the Text Variables panes.

The former also existed in KiCad 5 but under a different name. It was “Text & Graphics” in the Layers group:

The two panes share the same fundamentals, but in KiCad 6, there are additional configuration options.

The Text Variables pane is new and performs the same function as its counterpart in Eeschema (which I described earlier under “Text Substitution”). 

You can see an example of how Text Variables work below:

Text variables work with anything that contains text, such as text items, and labels.

Design Rules

The Design Rules group is a “mixed bag” concerning new and updated configuration options.

The Net Classes pane is inherited from KiCad 5 unchanged.

The Solder Mask/Paste pane, which was under Design Rules in KiCad 5, has been moved to the Board Stackup group in KiCad 6. Apart from the move to a new group, this pane is also unchanged.

The rest of the panes in this group are new:

Fillet tracks

In KiCad 6, you can create tracks with rounded corners. This function is titled “Fillet tracks” and is available through the context menu by right-clicking on a track.

The process begins with a single or multiple tracks as you can apply fillet tracks on multiple tracks simultaneously through multiple-selection.

Select the segments of a track (or tracks) that contain the angles that you want to fillet, and click on the right mouse button to reveal the context menu.

Select the Fillet Tracks option. In the popup that appears, set the radius of the fillet in millimetres. Values larger than 1mm produce curvier angles.

Click on OK, and you will see that the original 90-degree angle becomes a more natural-looking curve.

In my testing, I found that the fillet function only works with 90-degree angles. If you have tracks that contain 45-degree angles, you will not be able to convert them to curves.

You can also select multiple 90-degree tracks and fillet them at the same time. Here is an example:

In KiCad 6, filled zones have received two notable upgrades:

In KiCad 5, the only possible fill for filled zones was solid. Solid fills provide are simple and provide good resistive characteristics. But when used with thinner substrates, they can cause warping and even form bubbles under the copper. 

To prevent such defects, you can use hatched fill for the copper zones. This is now possible in KiCad 6.

Here’s a comparison of the fill zone configuration dialogue boxes. KiCad 6 is on the left, and KiCad 5 on the right.

The is a new group of widgets titled “Fill” in the right side of the KiCad 6 Copper Zone Properties window. The Fill Type drop-down allows you to select “Hatch pattern”, and select the various attributes for this fill. I have set 0.5mm for hatch width and gap.

The result of this configuration is below (showing a segment of the fill, compared to the solid fill from KiCad 5):

A second new feature concerning Copper Zone in KiCad 6 is that zone can now have names. You can see the Zone name text field in the widgets General group (see screenshot below).

KiCad 6 introduces curved ratsnest lines! This may not seem like a big deal, but check this out:

Along with the ability to customise the colour of the nets, the curved ratsnest lines on the left (KiCad 6) look much better than those on the right (KiCad 5).

Of course, curved vs straight lines is a personal choice, and KiCad 6 does not take this away from you. You can access this option from the View menu. Here’s a side-by-side comparison:

Interactive router

The interactive router in KiCad 6 has also received a lot of attention. There are several new configuration options available in the Interactive Router Setting dialogue box (see below, KiCad 6 on the left, KiCad 5 on the right).

The new options are:

In my limited testing, I found that the interactive router worked perfectly. My PCBs are relatively simple, and even in KiCad 5, I did not encounter any issues worth mentioning here.

Updated coordinate system

In Pcbnew, the coordinate system has been a source of frustration, especially for people moving in after using other tools. 

I was fortunate enough to start using KiCad after more than 15 years of not having used any other CAD application. During this time, I totally forgot any non-KiCad conventions, so everything in KiCad felt normal, including its coordinate system.

But the KiCad developer team recognises that KiCad is not the only "game" in town. For KiCad to increase its share, it must play better with widely accepted norms and standards. One of those norms is the way that the coordinate system works in Pcbnew.

The coordinate system is a fundamental concept in any drawing application. Pcbnew is, essentially, a drawing application for printed circuit boards. Its coordinate system assumes that the (0,0) coordinate starts at the top left corner of the page (see annotated screenshot below). You can adjust the origin left or right. And that's about it.

But, most (maybe all?) other drawing, mechanical or PCB programs assume that the origin is at the bottom left of a page.

This discrepancy between KiCad and everyone else causes several problems.

First, users coming to KiCad from other tools have to adjust working with the new coordinate system. After years of a bottom-left coordinate system, getting used to top right is easier said then done (example: I still used Netlists in KiCad 5 because muscle memory is hard to forget). 

Second, interoperability with other drawing tools is much harder when coordinate systems don't agree. At the very least, it will cost you a bit of time to translate X and Y numbers. At the worst, you could crash your robotic probe to Mars (doh!).

Here's the difference between KiCad 6 and KiCad 5 handling of the coordinate system configuration:

To set the KiCad 6 Pcbnew coordinate system so that the origin is at the bottom left (which ever point you choose), and for the Y coordinate to increase upwards, follow this process:

1. Go to Preferences --> Preferences, and select the Origins & Axes pane.
2. Select these options (also see screenshot above):
   1. Display Origin --> Grid origin
      
   2. X Axis --> Increases right
      
   3. Y Axis --> Increases up
      
3. Select the "Set grid origin point" tool from the left tool bar (see screenshot below).
   
4. Click at the location where you want to set the origin.
   
5. That's it.
   

Once you have set the new origin point, and the Y coordinate to increase up while the X coordinate increases right, you have a coordinate system that is compatible with most (all?) drawing programs. In the screenshot below you can see that the location of the cursor is reported based on my custom coordinate system rather than KiCad's default.

Create nets in Pcbnew

It is easy to create and use nets in Pcbnew. There's a few ways you can go about doing that.

For example, you can create a new net via the Net Inspector dialogue box (in the "inspect" menu). Once you have a net, you can assign a track to it through the track's (or pin's) properties.

It is also possible to create and assign a net in a single step. See example below. I have drawn a track, and brought up its properties. In the Net drop-down, I type the name of the net I want to create. If the name does not already exist, KiCad will offer to create it, and then assign it to the track.

Board statistics

The Inspect menu contains another useful tool, Board Statistics. It does what the name suggests. The Board Statistics dialogue box will display general information about your board, such as its components, pads, vias, and size, as well as drill hole sizes and locations.

You can also export these statistics in a text file:

Infobar

I have not had the opportunity to explore this feature much, but it did draw my attention a couple of time. 

Its a new, less obstrusive, way for KiCad to communicate with you: the Infobar.

For events that are not important enough to disrupt your workflow, but sufficiently important to warrant a notification, KiCad 6 uses a narrow bar just below the top tool bar. See below:

I did not have much opportunity to see the infobar in action because during my testing I did not trigger it enough. In the example above (left), I managed to trigger it by editing the footprint of a hole. The infobar informed me that I am editing the footprint that exists inside the board file, not the library. Therefore, any changes to this footprint will only apply to the board. 

Good to know, but not earth-shattering, hence the infobar is a good way to handle this information.

Locking

In KiCad 6 Pcbnew, everything can be locked. Footprints, tracks, zones, text items, etc. In KiCad 5, on the other hand, only few items were lockable. Zones, for example, were not. Neither were text items, or graphics.

To lock an item, as was the case in KiCad 5, you can use the context menu or the item properties dialogue box.

Below, I show how a zone is lockable under KiCad 6 (left) but unlockable under KiCad 5 (right):

Here's two more examples. Left, showing a text items, which is lockable in KiCad 6 (not lockable in KiCad 5), and an alternateive way to lock an item via its properties dialogue box.

Groups

In KiCad 6 Pcbnew, it is possible to group any two or more items. Once you have a group, you can move it to a new location. All of the items in the group will move together in the new location.

To select a group, just click on any of the group's items.

The ability to group items together was not available prior to KiCad 6.

When you are finished working with a group, you can ungroup the enclosed items by selecting Grouping --> Ungroup from the contextual menu.

Draw a rectangle

• Line.
  
• Circle.
  
• Arc.
  
• Circle.
  
• Polygon.
  

KiCad 6 adds one more:

• Rectangle.
  

You can draw a rectangle by selecting the tool by that name from the right toobar. Then click where you want to draw the first edge of the rectangle, and click again where you want to draw the last edge. KiCad will finish drawing.

The process looks like this:

In KiCad 6 Pcbnew, the context menu contains functions that can be applied immediately on the selected item. Most of these functions are carried over from the KiCad 5 Pcbnew context menu, but there are a few new items, plus some re-organisation.

At the top of the KiCad 6 Pcbnew context menu is the Select item, which contains a few sub-functions including the selection filter (that is also accessible via the Appearance pane in the right toolset). It is interesting to note that the Select item is present in KiCad 5, but is found towards the middle of the context menu.

Several of the movement function have been moved into sub-menus (such as the Special Tools for functions such as "Move Exactly" and "Move with Reference").

At the time I am writing this, there are a few new items in the Pcbnew context menu in KiCad 6:

• Grouping
  
• Select All
  
• Net Tools
  
• Copy Pad Properties to Default
  
• Paste Default Pad Properties to Selected
  
• Push Pad Properties to Other Pads...
  

The last three tools allow you to quickly propagate pad properties across your PCB. This was not possible prior to KiCad 6, and you would need to manually reset pad properties if you needed to make changes.

3D viewer and models

First, click on the images above to see their full-resolution version.

The KiCad 6 version seems a bit more refined, but using the default settings both renders look great.

Here's the same view with raytracing turned on:

In the KiCad 6 version, notice that the LED are reflecting some of the sorrounding silkscreen. Very impressive!

As with KiCad 5, raytracing is heavy on resources. It is something you will keep turned off and only use it when you want to take a glamour shot of your PCB. But in KiCad 6, you have several options to speed up raytracing that are not available in KiCad 5.

Here's the raytracing display options for KiCad 6 (not available in KiCad 5):

Reducing sampling or turning off options has a significant effect on the rendering time of new frames.

Next, I'll compare the other display options availabe in KiCad 6, and compare with KiCad 5 (you have alread seen the Raytracing options).

Below, the first two screenshots are from KiCad 6, and the last one from KiCad 5.

Here's some of the changes I have noticed:

• The Render Options group contains new options.
  
• The 3D Model Visibility, User Layers and Board Layers groups are unchanged.
  
• There's a new group that provides camera controls, such as the animation speed and the rotation increment.
  
• The OpenGL tab is new and allow you to balance the rendering quality against the framerate. Essentially, this is also the purpose of the Raytracing tab.
  

In terms of the 3D model assigned to the footprints, I did not notice much change. You can still assign a model to a footprint via the footprint's "3D Models" properties tab.

At the bottom left of the KiCad 6 Footprint Properties dialog box, notice a widget that allows you to set the model opacity. This is how you can make a model such as an LED seem semi-transparent. I can imagine applications of this feature in various kinds of displays, and perhaps PCB substrates.

In terms of the types of model files that KiCad 6 can read, clues are available in the 3D model chooser dialog box. You can open the chooser by clicking on the folder icon in the 3D Settings tab of the footprint properties dialog box (you can see this in the screenshots above).

First, here's the KiCad 6 and KiCad 5 versions of the model chooser dialog box:

In both cases, I have clicked on the dropped down widget below the file browser to reveal the supported files. From this comparison, you can see that Kicad 6 can read a large number of 3D model file formats, including IDF, EMN, WRL, X3D, etc.

Below is another screenshot that show the complete list (click to see full resolution version of the image):

The list contains:

• IDF
  
• EMN
  
• WRL
  
• WRZ
  
• X3D
  
• STP
  
• STPZ
  
• STEP
  
• STP.GZ
  
• IGS
  
• IGES
  

Other improvements

In this section I discuss improvements that are introduced in Pcbnew and Eeschema.

Copy/paste

Copy/paste has had a difficult history in KiCad.

In KiCad 5, for example, Eeschema does not even have a copy function. It has "duplicate" instead. Pcbnew does have "copy", but you can only paste in the same Pcbnew instance. This situation is similar to not be able to copy text between two text editors.

This is less then ideal

In KiCad 6, copy and paste works across Pcbnew and Eeschema instances. For example, you can copy a footprint from a project instance of Pcbnew and paste it to a standalone insteance of Pcbnew. 

You can do the same thing with Eeschema.

Here's a couple of examples. First, Eeschema.

In the next three screenshots, I show the copy and paste steps across two Eeschema instances.

Here is a similar example that shows how copy/paste works across separate instances of Pcbnew:

Symbol Editor in KiCad 6

The Symbol Editor in KiCad 6 has also received an overhaul. You will find much of the new functionality of the KiCad 6 Eeschema app in the Symbol Editor. 

Here's what the Symbol Editor looks like in KiCad 6, compared to KiCad 5:

New Symbol format

In the screenshots above, I am editing the same symbol to make comparison easier. At first, not much looks different. But a clue as to an important background change is in the infobox in the KiCad 6 Symbol Editor.

Take a closer look:

In KiCad 6, Symbols and footprints utilize a new format, which is not compatible with the old format. KiCad 6 is able to import and migrate old symbols and footprints so that your existing (as well as legacy public domain) libraries will continue to work.

You can still incorporate symbols and footprints from old libraries into your projects, but you will not be able to edit them without migrating them.

You can easily migrate an old library with all its symbols via the Symbol Library Manager. You can invoke the manager through the Preferences menu item.

It looks like this:

You can select a single or multiple libraries to migrate, and click on the "Migrate Libraries". KiCad will ask you to confirm the migration.

Once KiCad completes the migration, it will remove entries to the old libraries so that you can use the migrated ones exclusively.

A symbol library that uses the new format is noted in the plugin type column as "KiCad", as opposed to "Legacy". Also notice (in the screenshot above) the path for the KiCad 6 symbols. Use a file browser to navigate to the new symbols directory, where you will notice that the new symbol files have the ".kicad_sym" extension.

Top toolbar: Symbol Checker

The new Symbol Checker button brings up a window that provides information about defects in the symbol, such as pins found off-grid, or duplicate pins. For example, when I applied the Symbol Checker to the following symbol I received an appropriate response:

The Symbol Checker is not a new feature. It exists in KiCad 5, but is tacked into the Inspect menu, with the name "Electrical Rules Check". Given that this tool does not really do an electrical rules check, the name change in KiCad 6 to simply "Symbol Checker" seems reasonable. 

In KiCad 6, you can also invoke the Symbol Checked from the Inspect menu.

Top toolbar: Symbol Properties & derivatives

In KiCad 6, the symbol properties pane is extended to include several new configuration options.

Here are the Symbol Properties dialogue boxes for KiCad 6 and KiCad 5:

A notable difference is that in KiCad 6, there is no Aliases tab in the Symbol Properties dialog box. KiCad 5 symbol Aliases have been replaced by derivatives in KiCad 6. More about this in a sec...

The Footprint Filters is identical between the two.

The General tab contains several differences.

There are no changes in the Fields group.

The Symbol group contains two new options:

• Exclude from schematic bill of materials.
  
• Exclude from board.
  

The KiCad 5 Annotations group is renamed to Pin Text Options, without any further changes.

In the middle of the Properties dialoge box you will find the three familiar text boxes from KiCad 5 (Symbol Name, Description, and Keywords), plus a new one: "Derive from symbol". This is a drop-down field that replaces the Aliases tab from KiCad 5. Its purpose is to define the relation of the current symbol to other symbols.

Symbols can either be stand-alone, known as a "root symbol" (as is the in the screenshot above), or derive from another symbol.

To create a symbol that is based (or derives) from an existing symbol, click on the New Symbol button (the first button from the left in the top toolbar) or select File --> New Symbol, and then choose the existing symbol you want from the drop down.

Once you create the new derivative symbol, you cannot edits its graphics. But you can edit general symbol properties, and even the parent symbol through the Symbol Properties dialogue box.

One glitch that I noticed as I am writing this is that the symbol properties button is grayed out, and not clickable. To bring up the symbol properties dialogue box you must double-click on the symbol (I see that someone has already created an issue for this defect). 

Once in the derivative symbol properties dialogue box, you can edit everything, including the parent symbol.

Top toolbar: Add to schematic button

There is another new convenience feature in the Symbol Editor: the "Add Symbol to Schematic" button.

It does what it says: click it, and the symbol you are working on in the editor is added to the schematic.

The Symbol editor left toolbar in KiCad 6 looks almost identical to that of KiCad 5. As with the rest of the apps, the button icons have been re-designed.

There's one new button: you can now use "mil" to set the distance unit to mils, in addition to millimeters and inches.

Right toolbar

Let's wrap-up the review of the Symbol Editor in KiCad 6 with a quick look at the right toolbar.

Again, you'll see updated buttons icons. All buttons from KiCad 5 are present in KiCad 6, except for two:

• Import existing drawing.
  
• Export current drawing.
  

You can still access those functions in KiCad 6 under the File menu.

Footprint Editor in KiCad 6

The KiCad 6 Footprint editor has also received several upgrades. Both user interface elements, as well as drawing tools and how those apply to footprint design have received a lot of attention from the developers. 

As with my review of Eeschema, I will review the changes in the Footprint Editor organised by menu.

Let's start with a side-by-side comparison. Footprint Editor in KiCad 6 is left, KiCad 5 is right.

Right toolset

The Rule Area allows you to include named keep-out areas and constrains in your symbols. This was not possible prior to KiCad 6. You can get a feel of what is possible through the screenshot below:

Rectangle

The Rectangle button is new in both Pcbnew and the Footprint Editor. It allows you to draw a perfect rectangle with two clicks, in any PCB layer.

It looks like this:

The Appeance menu

The Appearance menu is almost identical to the one in Pcbnew. The only difference is that in the Footprint Editor, the Appearance menu does not contain the Nets tab since there are no nets at the footprint level.

Left toolbar

Apart from the updated button icon graphics, the KiCad 6 and KiCad 5 Footprint Editor left toolbar are almost identical. 

In KiCad 6, there is the new "mil" button (which also appears in Pcbnew).

Not much else to see here, moving along...

Top toolbar and menu

There's a few changes in the top toolbar, with new buttons and icons, as well as a new dropdown. The menu items remain the same.

Here's the KiCad 6 (top) and KiCad 5 (bottom) top toolbar and menus:

Pad properties

KiCad 6 offers many more pad configuration options compared to previous versions.

First, the pad properties dialog box in KiCad 6 looks similar to that of KiCad 5.

You will notice new pad and hole configuratioon options once you drill into the drop-down menus.

Here's some screenshots comparing the two versions (click on any image to see it full size):

In KiCad 6, pads are graphical objects that you can interact with as you can with any other graphic element. In the example below, I have configured a pad as a chamgered rectangle, with one corner. Then, I can click on it to select it, and drag any  of its corners to resize it. 

My language is not sufficient to express how much I appreciate improvements such as this. Well done!

Footprint properties

The Footprint Properties dialog box hasn't changed much. See below:

The only change I can see here is in the Fabrication Attributes group (Kicad 6 left, KiCad 5 right):

Text Substitution

I did a quick test of the new text substitution feature and I am please to report that it works with the Footprint Editor!

You can setup your text variables in Pcbnew (File --> Board Setup --> Text & Graphics --> Text Variables), and use them in any footprint. You can reference a text variable in any footprint property text field, or any graphical element of the footprint that contains text.

KiCad will render the variable with the actual value when you add the footprint to the layout (click on any image to see it in full resolution).

How to play with KiCad 6

Step 1: Setup an Ubuntu virtual machine

Step 2: Instal KiCad nightly build (currently, version 5.99)

Close the app (it might ask you to update its cache before it closes, allow it to do so).

Use the Ubuntu Software app to install KiCad nightly:

$ sudo add-apt-repository --yes ppa:kicad/kicad-dev-nightly
$ sudo apt update
$ sudo apt install kicad-nightly

# You can also install debug symbols:
$ sudo apt install kicad-nightly-dbg

# Demo
$ sudo apt install kicad-nightly-demos

# and libraries
$ sudo apt install kicad-nightly-footprints kicad-nightly-libraries kicad-nightly-packages3d kicad-nightly-symbols kicad-nightly-templates

Step 3: Play with KCad 5.99

A launch icon should appear on the desktop, but if not, you can start Kicad from the command line with this:

$ kicad-nightly

Similarly, you can start stand-alone Pcbnew and Eeschema instances from the command line like this:

$ pcbnew-nightly
$ eeschema-nightly

The KiCad application directory is at /usr/share/kicad-nightly.

I started playing with KiCad 5.99 by importing copies of some of my KiCad 5 projects. This gave me confidence that I will be able to continue work on those older projects in KiCad 6. The import process was painless, and both schematics and PCBs worked well in KiCad 5.99. 

Be careful. 

Use a copy of your old projects. 

Don’t try to import and convert an old project “in-place,” by allowing KiCad 5.99 to access the Kicad 5  project directory because KiCad 5.99 will convert project files to a format that is not readable by KiCad 5 (if you ever want to go back). 

That, plus the fact that KiCad 5.99 is a nightly build and not a stable build, means you should be extra cautious.

Recap: use copies of your KiCad projects. Do not risk your work. Make backups.

If you are feeling lucky, why not design a new PCB from scratch? 

The most important component “under the hood” change in KiCad 6 is the schematics and layouts’ file format. My understanding is that work there is complete. This means that any work you do has good chances that will be readable by the official KiCad 6.0. 

However, this is not 100% certain, and that is why I am talking about “playing” instead of “working” with KiCad 5.99.

Also keep in mind that:

Step 4: Update regularly

KiCad 6 (currently known as KiCad 5.99) is in active development. Each nightly release fixes several issues, and so it is a good practice to update your instance every few days.

I do this quickly on the command line like this:

$ sudo apt install --only-upgrade kicad-nightly
$ sudo apt install --only-upgrade kicad-nightly-symbols
$ sudo apt install --only-upgrade kicad-nightly-packages3d

Help make KiCad 6 better

Three segments make up the issue description:

Try to be clear and concise. 

When I report an issue, I use as little text as possible while being straightforward. I use a 2-3 minute video to describe the issue so that it is almost impossible to misunderstand. All this makes it quick for the developers to understand and deal with the issue.

Here’s one of my issue reports:

Conclusion