This article was sponsored by PCBWay. This tutorial deals with making more than one PCB design on one board, divided by a V-groove, so you can break the boards into different parts. I'll also show you how to make a faceplate for your module.
The finished module I'll be using as an example in this tutorial.
I'll take the most popular project on my website as an example, the AS3340 VCO and hopefully teach you how to make the PCBs and front panel inside KiCad 9 (and version 10 which has just been released) without the need for any wiring up of potmeters or sockets. So we're going to make a board for all the controls and in- and outputs and one for the actual circuit. I'll also show you how to order the boards on the PCBWay website.
About KiCad 10. The new version 10.0.0, which was released in April 2026, was full of bugs but we're now at version 10.0.4 and many of the bugs have been fixed and it's now perfectly usable again. I've done several projects on this new version and they came out great.
Before we continue I want to mention that the method I use here is my own, it's not the only way to do it and I'm not claiming it's the best way to do it. But it works for me so it'll work for you. This article is added to as my knowledge of KiCad enhances and I learn more tricks. It's all added to the text.
To follow this tutorial you need to be able to draw schematics and make PCB's inside KiCad so you need to have read and mastered the previous tutorial I wrote. We follow on from there.
DRAWING A SCHEMATIC with HIERARCHICAL SHEETS and GLOBAL LABELS
In order to make two PCBs in one go and have them connect together with pinheaders we need to draw each segment of our design separately.
We will make several schematic pages for this. The first will be the Root Page which is sort of the folder that holds all the other drawings. This is the page that normally opens when we click on the schematic symbol. When that page is open you click on the Hierarchical Sheets button which is the 15th button from the top on the right side or you can type 'S' on the keyboard.
Fig.1
Once you selected this tool you left-click on the root page (let go of the mouse button) and drag the mouse diagonally down to make a rectangle and click again. This rectangle represents a new page, you'll see it indicated underneath the Root page on the left.
The rectangle is just something you click on to get to that schematic page. You don't actually draw inside it so it can be very small. When you click a second time, to finished the rectangle, the Sheet Properties dialog will open.
Fig.2
Under 'Sheet Name' Fill in a name for your schematic, in this case Main Circuit, Underneath sheet name is the 'Sheet File' box. For this, fill in a name under which your schematic will be saved in the project file. I had a bit of trouble in the beginning understanding what I had to fill in here but I now use a name with a page number for this. In this case the project uses the 3340 chip so all my sheet files are named: 3340-1, 3340-2 etc. but you can also give them the same name as the sheet name. I'll leave that to you.
Draw an other rectangle on the Root page for the controls and in-/outputs for our VCO and I later added a Triangle to Sinewave converter to this design so I drew a 3rd rectangle for that. Again, the size of these rectangles doesn't matter. This is what my Root page looked like:
Fig.3
Some people draw these rectangles onto a schematic page to be able to click to different parts of a schematic easily if the schematic is divided onto different sheets. I like to have them all on the root page but you don't HAVE to do that.
USING GLOBAL LABELS.
You can double-click on each of these rectangles and that will open the respective schematic page that rectangle represents or click on their names in the 'Schematic Hierarchy' box on the left (see fig.3) If you don't see this box on your screen then go to the very left of the screen and click on the icon above the crossed spanner and screwdriver. Second-last symbol down. It looks like a family tree.
We're going to start with the main circuit of our VCO.
Draw the schematic but leave out any control potmeters, switches and in- or output sockets. In short: anything that goes on the front panel. Instead of drawing those in we're going to attach a 'Global Label' to represent that specific in- or output or potmeter/switch. We need to make labels for each pin of a component on the front panel. So a potmeter will have a label for pins 1,2 and 3 although if pin 1 is a ground connection you can just connect it to ground on the front PCB and use 2 labels for the other pins. This also goes for a pin connected to power. It doesn't need a label, we'll just connect it to power on the front PCB.
To place a global label you select the 'Place Global Labels' icon or click CTRL+L
Fig.4
Select it and place a label in your schematic. Now double click on it and the Options pop-up will appear where you can name your label and select whether it's an in- or an output, bi-directional, Tri/State (High, Low or Unconnected), or Passive (none of the above). Always check in your mind how the current flows in your circuit and imagine if the electrons flow out of the circuit or into the circuit. For instance if you attach a label that represents the wiper of a level potmeter, the electrons will flow out of the wiper into the circuit so it's an input for the circuit and an output for the potmeter itself. IMPORTANT: In order to connect elements from different schematic pages together on the PCB, you must always use labels with the exact same name.
Make sure that two differently labelled sections are not in direct contact with eachother otherwise KiCad will select one of the labels to represent the complete net and it won't use the other, which will create problems.
Also beware that if you named a net in the schematic with the 'Place Net Labels' tool, and you attach a Global Label to that net with a different name than the net label, you will get an error message in the Electrical Rules Checker and it will use the Global Label name. In fact, even if you use the same name as the label you'll get an error message. Nets that have Global Labels attached to them should not be named with the Place Net Labels method.
TIP: What I always do is draw the entire schematic including all the potmeters and sockets etc. and then when I finished that, I select each socket, switch and potmeter and 'cut and paste' it to the schematic page for the control panel (front panel). Then I label the wires that remain behind and copy and paste those labels to the front panel too, to connect the potmeter so I'm sure the labels have the same name. Doing it this way makes sure you don't forget anything.
Here is an example of the 3340 VCO main circuit schematic page:
Fig.5
Everything is there except the potmeters, switch, and in- and output socket connections. They all have Global Labels attached to them.
Power section:
You have to draw in a little section representing the power input, as we learned in the previous tutorial. It doesn't matter on which schematic page you draw it.
Now, in the schematic above I just drew in a simple representation of the power section but it's better to do it as shown in the image below here. I have the power connector at the right and then the bypass caps for all the chips used and the power connections to all the chips at the left.
This image below is obviously NOT from this project. I'm just showing it here as an example of how best to draw a power section:
Notice I have Schottky diodes in the power lines. That means the Powerflags need to be placed before those diodes! I also used different 12V indicators on the outputs namely +12VA and -12VA to differentiate them from the incoming power at the connector before the diodes. This is very important!
All the main circuit connections to power (like the IC's, potmeters etc.) must go to these connections, after the diodes if your circuit used diodes in the power rails. Sometimes resistors are used or ferrite beads but most times it's a straight connection not requiring two different power indicators.
The controls page:
In the next schematic page I drew in all the controls, like the potmeters and the octave ground switch and the in- and output sockets and gave them the same labels I used in the main circuit. Here's what my controls schematic page looked like:
Fig.6
When you finished drawing all the controls; the potmeters and sockets and labelled all the connections then you can count how many different labels you have so you know how many pinheaders you will need to connect the two PCBs together. Don't forget you also need to have pins for the power connections from one PCB to the other and for ground.
For the Global Labels that connect to the pinheaders it doesn't really matter if you specify them as inputs or outputs as long as they have the same name as in the main schematic so they will all connect on the PCB.
I put all the different types of controls into their own box which you can draw in with the 'Draw Rectangles' tool and I used the Text tool to give each box a name. This is just to make it look neat and tidy. It's not something you HAVE to do.
PINHEADERS:
Now, you can see in the lower left I drew in two pinheaders to connect the PCB with all the potmeters and sockets to the PCB with the main circuit on it. I had 16 labels in total, representing connections to the main circuit so I choose two 10 pin connectors from the symbols library and I made custom footprints for them with 10 solderpads each at 2.54mm distance from eachother. I choose one male and one female row of pinheaders and drew the lines to connect them together and then I drew in the vertical lines to connect the Global Labels to each of the pins. Before adding the labels I dragged over it with the mouse and copied and pasted it so I had two of these pinheader arrangements, One for the left side of the PCB and one for the right side giving me 20 connection points in total.
Ground and reinforcements.
I also added extra ground connection pinheaders which you can see in the lower right box. I added these for two reasons: to make sure the ground connections were solid and as structural reinforcement for the PCB connections. You need to check where on your PCB any force is applied by pushing patch cables into sockets or when a screwdriver is pushed onto a trim potmeter when tuning the VCO. These points must have some pinheaders underneath or near them so the PCB doesn't seesaw or bend when you apply force. One 3 pin pinheader in each of the four corners would be the perfect solution but I didn't have space for that. But my extra pinheaders worked out fine.
You can also put the Global labels straight to the pinheaders without drawing lines between them but I thought this would be a bit more logical to follow for beginners. Remember, I'm a beginner too at this and this was the first time I made a multi board design in KiCad. So we're learning together how to do this.
Professional multi layered schematics look much more streamlined but also more complicated so I present it to you as I learned it myself. We will become better at this with experience.
Before continuing, click 'Annotate Schematic' under 'Tools' and then run the Electrical Rules Checker and make sure you get two green zero's showing all is good with your schematics.
CHANGING MULTIPLE FOOTPRINTS AT ONCE.
I'm putting this little section in here, eventhough it's not really part of this project or tutorial but it's a useful feature I want you to be aware of. Say you made your design in through-hole and it's all working fine and now you want to make an SMD version. Instead of changing each footprint from TH to SMD you can do the following. Say you want to change all the resistor footprints. Change the footprint of one of the resistors in the normal way.
Now go to 'Tools' and open 'Edit Symbol Fields'.
Now you see this spreadsheet appear:
Select the footprint of the one resistor you changed and copy it (CTRL + C).
Now select all the resistor footprints you want to change by clicking the top one and then shift + click the bottom one to select all. Now press CTRL + V (paste) to change them all and click on save at the top left.
Now all your resistors footprints are changed. You can change all sorts of things in the spreadsheet which can make your life a lot easier.
And now, one more tip I want to give you:
RE-CONNECTING THE PCB TO THE SCHEMATIC AFTER MOVING THE PROJECT FOLDER.
If you copy and paste or cut and paste your complete project into another folder it will most likely result in the schematic being disconnected from your PCB design so when you make changes in your schematic and try to update the PCB, those changes won't get through.
There's an easy solution for this.
When you click on 'Update PCB from Schematic (F8)' you need to check on the following options in the dialog box:
Check on 'Re-link footprints to schematic symbols based on their reference designators.' (That's the top option in the dialog box.)
Also check on: 'Delete footprints with no symbols' and 'Update footprint fields from symbols.'
Now click on Update PCB and everything will be connected again and PCB components will update with changes made in the schematic.
Here's what the dialog box looks like:
A final short tip before we move on to making the panel. This is how to change a 3D model representing your component in the 3D viewer. Say you made your own symbol with a custom footprint and you want to see that component in the 3D viewer. Here's how to do that.
Go to the Footprint Editor and select your footprint. In the top toolbar, the icon for footprint editor now has a red sprocket wheel in it. It's now called 'Footprint Properties'. Click on it to open it up. Go to the 3D models tab. Click on the folder symbol next the big plus sign and from the library load a model that looks like the one you want but may differ in size. You can change the orientation etc with the X,Y,Z controls on the left of the model. You can drag the model in 3D space with the mouse.
Click save when you're done. You can download extra models from GrabCAD.com
DESIGNING THE PCBs.
Now that all schematics are drawn and properly labelled, we can go on to making the PCB designs.
I won't go into the details because I covered all that in the first tutorial so you should know how to lay tracks and make ground planes etc.
First we're going to determin the size of the PCB(s) we want to make.
Proceed to draw a rectangle in the Edge Cuts layer and double click on it. This will open a dialog box. Choose 'by corner and size' (see fig. 12) and type in the exact dimensions of the PCB. I wanted the VCO to be 14hp wide in eurorack terms. So this means 14 x 5.08mm = 71.12mm.
But beware! That is the width of the Faceplate so I made my circuitboards 4mm less wide at 67mm with a length of 105mm. The faceplate length of a Eurorack panel is always 128.5mm so this will create enough overlap at the top and bottom for the front panel of the module to fit it into a eurorack case. When you've done one rectangle you can simply click on it and duplicate it for PCB 2.
Now you have two PCB outlines you can import the components with the 'Update PCB from Schematic' button. Start placing the components using the left PCB for all the potmeter controls and in- and outputs and the right PCB for the main circuit of the VCO. Place the pinheaders and draw in the tracks etc and finish the PCBs.
Beware that the DRC check tool won't work properly when your making more then one PCB at once. So you must be very thorough with checking for mistakes and making sure all the groundplanes actually connect to ground. Do run the checker and see which mistake is due to it being on two PCBs and which mistakes are real mistakes. After some training it becomes easy to see which are the real mistakes that need attention. You will be left with many thin blue lines indicating connections that according to the software are not made but you'll see they run from one board to the other so they'll be represented by the pinheaders. HOWEVER, do check all the mistakes listed in the DRC checker and make sure.
One more thing about groundplanes: although it is fine to have more than one point on a PCB where the power comes in, for instance a power connection to more than one pinheader, it is not advisable to do this with groundplanes. Groundplanes should all connect to eachother and preferably via one route otherwise you can get so called ground loops which can cause a lot of noise or hum. Beware of that.
You must also make sure all ground points connect to the ground planes and are not cut off by tracks. Sometimes you'll need to lay a track for ground or use via's to make sure it all connects to eachother. It's also wise to use multiple via's to connect pieces of groundplane together to decrease the resistance (impedance) between them.
Here's what my final design looked like after I put them together. I will explain how to do that, next.
Fig.7
Fun fact: In a recent video I saw that Jason (from Instruo) designs the PCB layouts as he is drawing the schematic. I saw him drawing in little sections of the schematic and then placing them on the PCB to keep all the connections as short as possible. Of course his projects are much bigger and more complicated and he does SMD instead of through-hole PCB's.
What I do is to check for every component where in the circuit it belongs by looking at the schematic and then try to place everything as close to where it belongs as possible.
There's also a plugin you can use for that called 'Place by Schematic'.
PUTTING MULTIPLE PCB's TOGETHER WITH A V-CUT IN BETWEEN.
When you finished your PCB layouts, making sure the pinheaders are aligned so they will fit together, you can start connecting the PCBs together. Please note your total PCB size has to be at least 70 by 70mm in order to do the V-Cut process. The individual PCBs can be much smaller.
Place the PCBs in line with a 2mm gap between them.
Delete the individual Edge.Cuts outlines of the boards and draw one Edge.Cuts outline around all the boards. Leave the 'Filled Zones' in place if you used them.
Now select the User.Eco1 layer and in the top left menu go to FILE -> BOARD SETUP...
When you open this you see an overview of all the layers. Click on the User.Eco1 layer and change the name to 'V-CUT'.
Fig.8
Click OK and with the V-CUT layer selected draw a line in the 2mm gap between your two PCBs from top to bottom. Now click on the line and set the width to 2mm.
Although the eventual V-cut will have a width of about half a millimeter, the manufacturer of the PCBs wants to see a 2mm line on your design in the V-CUT layer to indicate a V-cut. This gives enough clearance from the copper near the edge of the board. There must be no copper in the area that is covered by the 2mm V-CUT indicating line!
Fig.9
In the same V-CUT layer, use the 'Draw Leaders' tool to draw an arrow at the top, pointing down, and name it 'V-cut' to make it clear to the PCB factory that you want a V-cut at the position of the line. Do the same at the bottom of the line(s).
The draw leaders tool is the 4th from the bottom. You'll have to click on the 'Draw Orthogonal Dimensions' button (with the V-CUT layer selected) and keep the mouse button pressed in and then select the right most icon. That's the draw leaders tool.
Fig.10 Draw Leaders button.
Before you ZIP up your Gerber files, add a little Readme.txt file with the text: "V-Cuts are in the V-CUT layer (User.Eco1)." Don't forget to click the V-Cut layer on when you make your Gerbers.
This will prevent delays with them sending you an email to confirm where the V-Cuts need to be. This makes it machine recognizable which saves a lot of time in pre-production.
I used this method with JLCPCB multiple times now and my PCBs went into production without any questions from the production team.
Here's a link to a YouTube video that explains the whole proces and also shows you two plugin options for KiCad that do the V-Cut work for you: https://www.youtube.com/watch?v=ph2jV5HMxfQ
GERBERS and ORDERING PCB's
Now you can save your project and make the Gerber files for it. Make sure you check on the V-Cut layer when making the Gerber files to include the V-Cut information. You'll end up with 15 files instead of the normal 14 files in your Gerber folder (actually 16 files with the 'readme' file included.) Turn them into a ZIP file. Now you can upload them to a website like PCBWay to have them made.
In the upload page of the PCBWay website, under 'Board type' choose the 'Panel by Customer' option to indicate we have more than one PCB design in one file.
Next click 'accept' for the 'X-out allowance in panel' option. If one PCB in your multiple PCB panel tests as being faulty, they will mark it with an X in white.
Finally under 'Different design in panel' select the number of different PCB designs that your Gerber file contains. In this case it's 2.
Here's what that looks like on the PCBWay website: (It works the same on the JLCPCB website but you don't have to fill in the 'X-out allowance in panel' option there).
Fig.11
Scroll down the rest of the page and make sure everything is as you want it. At the bottom there's a text field where you can type in anything that you feel the PCB producers need to know so in this field you could type that this is a PCB design with a V-cut in the middle represented by the V-Cut line but it shouldn't be necessary.
Fig.12
When all is as you want it to be, you can press 'Save to Cart' and proceed to checkout after you get confirmation your designs are approved. The PCBs are usually approved within 10 minutes if everything is okay and if not they will contact you by email pretty quickly. The service of PCBWay is really good. With PCBWay you get confirmation before payment. With JLCPCB you'll receive confirmation after payment, but if there are faults detected you can upload new Gerber files to them.
If you order from PCBWay for the first time, make an account on the website and make sure you enter your shipping details like name and address etc.
Here's a special little extra for readers of this website. It's a free plug-in for KiCad that makes the ordering proces a lot easier. You just click the link and everything will be explained:
MAKING A FACEPLATE.
Now we need to make a faceplate for our project.
I'm going to refer to the faceplate as the 'panel' in this section.
For this, we don't have to use the schematic section of KiCad at all, just the PCB Editor.
To make a panel, make a new project in KiCad and name it the same as the PCB project with the term PANEL behind the name. At least, that's how I always name them. Of course you can choose whatever name you want.
Now close that panel project and go back to the previous PCB project and open the PCB editor.
Click and drag over your PCB design to select it and copy it. (CRTL + C)
Close that project and open the Panel project you just made and select the PCB editor.
Now Paste the PCB design into the PCB editor by clicking CTRL + V. Now SAVE the project.
Now your PCB design appears in your panel project. What good is that, you may ask. Well, we're going to use the PCB design, or more precisely that part of it that has the potmeters and sockets on it, as a template for our Panel design, to make sure all the holes are in the right position.
Drag the PCB design a bit to the right to make room for the panel design. Also make sure you place it vertically in the middle so you have some panel overlap at the top and bottom. This should be obvious.
The image below shows the finished panel design with the PCB design underneath with all the holes lining up as a final test that it all fits. Note the panel sticks out at the top and bottom and a little bit on the sides aswell.
Fig. 13-A Selected PCB overlaps with the panel holes.
To make a panel we first draw the outline in the Edge.Cuts layer. This outline must fit the exact standardized dimensions of a Eurorack panel with a height of 128.5mm and a width that corresponds with the hp size that's one size wider than your PCB design. We can type these parameters straight in the Rectangle Properties box.
In the Edge.Cuts layer, choose the Draw Rectangles tool and draw a rectangle. Put your mouse cursor on one of the lines of the rectangle and double click on it. Now a dialog box opens where you can enter the Rectangle Properties. Choose the 'By Corner and Size' option at the top and under 'Size' enter the dimensions, in this case 71.12mm by 128.5mm for an 14hp faceplate. Click OK to finish.
Fig.13-B
One hp in Eurorack is 5.08mm so 14hp is 5.08 x 14 = 71.12mm
Our PCB design should be a few millimeters smaller in width than our panel rectangle. Now drag the PCB template we copied in, into our front-panel rectangle and in the 'User Drawings' layer draw position crosses over the center of the holes that need to be made. The cursor should be magnetically attracted to the middle of most footprints most of the time, which helps with accuracy.
When you have drawn position crosses over the center of every hole that needs to be made in the panel, switch off the User Drawings layer, carefully drag-over and select the whole PCB inside your panel (without selecting the front-panel edge cuts layer) and drag it out of the Faceplate area again. Turn on the User Drawings layer again and all the positions for the holes should now be visible.
After you started placing the holes and other design elements, this method can no longer be used to add new positions for holes afterwards. The placement of holes by using marking crosses should be the first thing you do when making a panel. You can drag the PCB design over the panel design again later, to check if everything is still in the right place, but you must make sure it doesn't get de-selected because then you can't drag it out of the panel area and you can start all over. The undo button might help you out but don't take the risk. Select your PCB and drag it over the panel to do a visual inspection for the correct alignment of the holes and keep the mouse button pressed down while you do that and when you're satisfied drag the PCB straight out of the panel again.
MAKING THE HOLES:
To make the holes for the potmeters and screws and switches I mostly use solderpads and adapt them to the right dimensions.
Go into the footprint editor and choose 'new footprint'. Choose the solderpad tool and place a solderpad. Double click on it and change the dimensions to your needs. For instance, below is a screenshot showing how I made the elongated screwholes:
Fig.15
I always leave a copper edge of about 1mm around the hole to reinforce the hole. It disappears underneath the potmeter nuts anyway, you won't see it.
An other way to make holes is to draw a circle (or which ever shape you need) in the Edge.Cuts layer. With this method there will be no copper on the sides of the hole, just a clean hole in the PCB. This is the method to use if you need square or rectangular holes with sharp edges because that's something you can't do by using solderpads for holes.
I have a special library folder for all the things I use on Front Panels called 'Panel Elements'. It also includes all the Art Deco scrolls and things I use to improve the look of the faceplate. I also have custom made decals, the lines that represent the potmeter scale in that folder.
I don't always turn the artwork images into footprints because I usually need to scale them down to different sizes which is easier to do in the Image Converter.
I look for good looking designs online, copy them into a folder mostly using the Screen Cut and Paste tool that's included in Windows-10. I then import them into the Image Converter and I choose the size I need and 'copy to clipboard'. One copy for the F.Cu layer and one for the F.Mask layer. They need to be placed on top of eachother. (Don't forget to delete the G*** watermarks.)
I go a bit further into this in the 'Decorating... segment' below.
PLACING SCREWHOLES.
To place the screw hole footprints, draw a horizontal line 3mm under the top and one 3mm above the bottom of the panel outline. To determin where to place the vertical line that will make up the placement cross for the screwholes you must do a calculation:
Take 7.5mm and add to it 5.08mm and keep adding 5.08 until you're as close as can be to where you want the screwholes to be placed. The minimum distance from the left side is always 7.5mm.
In the case of a 14hp panel with 4 screwholes I placed them at 12.58mm (7.5+5.08) and 58.3mm (7.5+(10x5.08)) from the left edge of the panel. Always calculate from the left edge of the panel.
DECORATING YOUR FRONT-PANEL DESIGN.
You can use the line tool and other drawing tools to decorate your panel with copper lines and you can also download images, change them into footprints and use them on your panel design.
We make most designs inside the F.Cu layer, the front copper layer which, in production, will get a coating of solder over it so it comes out nice and shiny silver coloured. You can have it gold covered if you wish but you'll have to choose that option when you order them and it will cost a lot more.
You can add Text and other elements in the F.Silkscreen layer too if you wish. They will come out in white on the end product. Don't forget to choose the overall colour you want the panel to have when you order them online. I usually choose black.
To add text to your panel use the text tool. You can select any font you want and type the text you want to add. Then you must duplicate the text layer and double click on it to open the text dialog box.
Now change the layer from F.Cu to F.Mask.
ANYTHING THAT MUST NOT BE COVERED BY THE SOLDERMASK MUST BE REPRESENTED IN THE F.MASK LAYER!
Fig.16
In this image I've moved the text copper layer to reveal the text mask layer in blue underneath. Normally they must of course be placed exactly over top of eachother.To add lines or circles to your design is a bit easier than text. Draw the lines with the line tool and then double click on it. Now check the box at the bottom that says Soldermask. Now your line won't be covered by the soldermask. To stop the cursor from sticking to certain angles and grid lines, and to move freely, keep the SHIFT button on your keyboard pushed down while you drag with the mouse.
Check your progress with the 3D viewer to make sure your designs actually shows up on the panel.
To use an image or design you downloaded from the internet, first use the cursor coördinates to measure the space your design must fill up on the panel. Make a note of it.
Now go to the start menu of KiCad and open the 'Image Converter'.
Load in your image and enter the size you want it to be. Make sure to choose the F.Cu layer for the footprint. Also decide whether you want the image to be in negative or normal. Sometimes negative makes it show up better but that's up to you. Select the correct contrast level.
Now click 'Export to Clipboard'.
Go to the panel and click CTRL + V (paste) and place your design on the panel. Now repeat this but now make the image for the F. Mask layer and place it over the one for the F.Cu layer.
If you want to save the image as a footprint then go to the Footprint Editor and click 'Make a new footprint' in your custom panel designs library. If you don't have one, make one.
Click 'make a new footprint' and paste the image into the footprint editor with the F.Cu layer selected.
Now click on your footprint design and in the dialog that pops up check the 'Solder mask' check box.
You must do this for every unconnected element in your footprint design. You'll see the bezier lines light up white when you click on one. After that is done you can save it.
Now you can go to your panel design in the PCB editor and use the 'Place Footprints' tool to import your design and place it on the panel. It's a shame you can not scale images this way so if it doesn't fit you have to import it again into the Image Converter and enter an other size.
Therefore it's often easier to just use the image from the Image Converter straight on to the panel making sure you have one for the F.Cu and one for the F.Mask layer placed on top of eachother. You can easily change the scale this way and make it fit. This is what I usually do.
CUSTOM DECALS
In the image above you can see a custom made scale decal around one potmeter hole. I made a circle first in the User Drawings layer and then I used the 'Draw Arcs' tool to mark the degrees on the decal scale with grey lines. Then I drew them in on the F.Cu layer with the line tool, holding down the Shift button to make sure I could move the line in any direction I wanted. I then double clicked on every line I drew in and checked the Soldermask box.
When I had my design finished I drew in a ground plane for the back side of the panel on the B.Cu layer. I always do this to provide a copper shield for the circuit. Designate it as a GND layer so it provides shielding against radio waves and other unwanted signals.
My final Front Panel design for the AS3340 (Digisound-80) VCO. It's 14hp wide.
Fig.17
3D viewer version:
Fig.18
So, if you haven't used any silkscreen in your design, turn the F.Silkscreen and B.Silkscreen layers off when you make the Gerber files.
FINAL CHECK!
After placing all the holes in the correct place, Save your work, turn off the User Drawings layer and drag-select the PCB we used as a template and while it's selected drag it overtop of your panel and see if all the holes line up with the locations on the PCB. This will instantly show if something is wrong. Make sure it stays selected as long as you use it. After that you can delete the PCB template, we no longer need it. You can also delete the lines in the User Drawings layer now.
If you're working with a bigger project you can make a new project called 'TEST' and copy your PCB designs and Panel design all into the PCB editor of the new project and in that project you can select and drag your PCB designs on top of eachother and see if all the pinheaders align. Check if the holes in your panel align with the position of the potmeters. When you're finished you can just delete that project. that makes the testing a bit safer than using the originals because if you have a PCB selected and placed on top of your panel design and it becomes unselected for a reason. You have a BIG problem! Maybe the 'undo' button can save you but chance is you'll have to start over or recover using a back-up saved earlier.
END RESULT:
And here's how the final product came back from PCBWay. Shipping with the Global Shipping option took 10 days to The Netherlands which is good going by todays standards.
They look amazing although they are matt black and I would have preferred satin gloss! I later sprayed a layer of clear lacquer over it which made if look nicely deep black and shiny.
The quality is really good. There are no imperfections on the faceplate which I did have with other manufacturers:
Fig.19
Below are the PCB's with the V-cut. It's executed just like I wanted it to.
Fig.20
The V-cut is just 0.5mm wide and is applied from both sides. The PCB's can be very easily broken appart and they break very cleanly, leaving just a slightly rough edge. Just a light sanding down will do to make it smooth. I'm really pleased with the result.
Fig.21
Look how nicely the potmeter fits into the footprint:
Fig.22
I started building the project early afternoon and by 19:00h I had it finished except for the sockets, but it was good enough to test it and it all worked straight away! I have included a new version of the triangle to sinewave converter on this board too and look at what a wonderful sinewave it produces:
Fig.23
(Go to Project 3 and scroll down to see the updated Triangle to Sinewave converter schematics)
THE FINISHED PRODUCT.
It's awesome. Everything worked out as I planned it and I'm glad I sat on the design for a full week, checking for errors, before sending it of because I did find some ground points that were not connected and other small mistakes but I got them all out luckily. However I did come across an error once I got the boards back. I had the wiring of the Octaves grounding switch the wrong way around and that caused a short circuit every time I turned the potmeter fully to one side with the switch in the ground position. I fried two potmeters before I discovered the mistake and I had to cut the tracks and re-wire that switch. An easy fix though.
The moral of the story is that mistakes are very difficult to rule out completely but you must take your time to do the best you can. It would be a shame to have to bin the PCB's you made. At least I know now that the version 2 boards will be perfect.
Fig.24
The space between the boards, separated by pinheaders, is exactly 11mm.
Fig.25
I just finished tuning this VCO and it gave me the best result I ever had with a VCO. In tune over 6 octaves within a few cents over the complete range. Notes C0 to C5: max deviation +/-2 cents. C6 was 3 cents low. Rock solid results.
In December 2025 I made a new version of the X4046 VCO and I sat on that design for a full month before sending it off. Constantly checking for errors and I found a few and also came up with improvements. So it pays not to be too hasty.
Finally I would like to leave you with two YouTube videos. The first showed me how to make faceplates for modules in KiCad. I learned it all from this video, I can really recommend watching this:
And here's the second, a video that goes through the whole proces of what happens after you submit your Gerber files to the production firm. A very interesting video to watch!
I would like to thank PCBWay for sponsoring this article. Please check out their website and the free plug-in for KiCad.
PCBWay order page: https://www.pcbway.com/QuickOrderOnline.aspx
If you have any questions or comments then please post them below. Please note comments are moderated and don't appear until I approved them.
PLEASE CONSIDER DONATING.
If you learned something from this website, please consider making a small donation. It really goes a long way to help me maintain the website and to finance new projects. There's a button for that underneath the main menu if you're on a PC or Mac. Otherwise you can use this Paypal.Me link and cut out the middle man. Thank you very much!
