Synthesizer Extra's No.7: KICAD 9.0 - MAKING MULTIPLE PCB's ON ONE BOARD.

This article was kindly 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.

Check out the PCBWay website

I'll take the most popular project on my website as an example, the AS3340 VCO and hopefully teach you how to make the PCB's and front panel inside KiCad 9 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. I'll have a link for a cool plugin for KiCad that you can download for free and it'll order the boards with just one click of the mouse, right within KiCad itself. More on that further down the article.

Before we continue I want to mention that the method I use here was 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 worked for me so it'll work for you.

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 PCB's 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 square and click again. This square represents a new page, you'll see it indicated underneath the Root page on the left. We're going to use this to draw in the main circuit of the VCO. When you click a second time, to finished the square, 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.

Draw an other square 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 square for that. The size of these squares doesn't matter. This is what my Root page looked like:

Fig.3

USING GLOBAL LABELS.

You can click on each of these squares and that will open the respective schematic page that square represents.

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. Instead of drawing those in we're going to attach a 'Global Label' to represent that specific in- or output or potmeter/switch.

To do this 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 or bi-directional. 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. 

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. 

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 a Global Label attached to them. 

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.

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 PCB's 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.

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 if the pins. Before adding the labels I 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. 

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 in connectors or with a screwdriver when tuning the VCO and these points must have some pinheaders underneath them so they don't bend when you apply force to put in a power cable or tune the VCO. 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 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, run the Electrical Rules Checker and make sure you get two green zero's showing all is good with your schematics.

DESIGNING THE PCB's.

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.

Proceed to draw two squares in the Edge Cuts layer and double click on them. This will open a dialog box where you can type in the exact dimensions of the PCB's. 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 of the module to fit it into a eurorack case.

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 PCB's.

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. You can run the checker and see which mistake is due to it being on two PCB's 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.

Here's what my final design looked like after I put them together. I will explain how to do that, next.

Fig.7

PUTTING MULTIPLE PCB's TOGETHER WITH A V-GROOVE IN BETWEEN.

When you finished your PCB layouts, making sure the pinheaders are aligned so they will fit together, you can start connecting them.

To do that select the F.Fab layer and draw a line with a width of 2mm from top to bottom at the right side of the left PCB. You can set the width of a line by double clicking on it.

Drag the line against the edge of the 'Fill Zone' (ground plane) of the PCB if it has one. See image below. Now drag and select the right PCB and drag it next to the line as is shown below:

Fig.8

Delete the individual Edge Cut lines that were drawn around each of the PCB's and draw a new Edge Cut rectangle around the two PCB's together.

In the F.Fab layer, use the 'Draw Leaders' tool to draw an arrow at the top and name it 'V-score' to make it extra clear to the PCB factory that you want a V-groove at the position of the line.

The draw leaders tool is the 4th from the bottom. You'll have to click on the 'Draw Orthogonal Dimensions' button and keep the mouse button pressed in and then select the right most icon. That's the draw leaders tool.

Fig.9 Draw Leaders button.

GERBERS and ORDERING from PCBWay.

Now you can save your project and make the Gerber files for it. Make sure you check on the F.Fab layer when making the Gerber files to include the V-score information. You'll end up with 15 files instead of the normal 14 files in your Gerber folder. 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)

Fig.10

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 can type that this is a PCB design with a V-groove in the middle. Just to be sure.

Fig.11

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 PCB's 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. 

If you order from them 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 plugin for KiCad that makes the ordering proces a lot easier. You just click the link and everything will be explained:

https://www.pcbway.com/blog/News/PCBWay_Plug_In_for_KiCad_3ea6219c.html

MAKING A FACEPLATE.

Now we need to make a faceplate for our project.

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. 

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 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 faceplate overlap at the top and bottom. This should be obvious. (see PCB-Editor screenshot below)

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 and under 'Size' enter the dimensions, in this case 71.12mm by 128.5mm for an 14hp faceplate. Click OK to finish.

Fig.12

One hp in Eurorack is 5.08mm so 14hp is 5.08 x 14 = 71.12mm

Now select the 'User Drawings' layer and with the line tool start making horizontal lines from the exact middle of your potmeters on the PCB to the left, over the panel square. Do this for everything that needs a hole in the faceplate.

Here's an image of what that looks like. It's not accurate because I made it after I finished the Panel design so the lines are not in the right place anymore but it's to give you an idea of what I mean:

Fig.13

When you've done that you need to use the X/Y coördinates to determin the distance from side of the panel to the middle of the hole in the panel, for each of the controls and sockets. Remember to add 2mm to your results because the overlap of the panel over the PCB's is 2mm on each side!

Before starting to draw in the holes, go to the Footprint Editor and draw a custom footprint for each of the different size holes you'll need. I made custom footprints for potmeter holes, socket holes and also a stretched circular one for the screwholes at the top and bottom of the panel. I made a new library for this named 'Panel Elements' and put them all in there. The Screwholes must have an inner diameter of 3.2mm. I left a little copper edge around the holes because it reinforces the hole and it looks cool.

Using these footprints will make it so much easier to place the holes accurately on the panel because they will snap in place over the position crosses you've drawn in the User Drawings layer.

To place the screw hole footprints, draw a horizontal line 3mm under the top and 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.

FINAL CHECK!

After placing all the holes in the correct place, 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. 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.

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 solder layer attached to it so it comes out nice and shiny silver coloured.

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.

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.14

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 one on top of the other.

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 and CTRL buttons on your keyboard pushed down while you drag with the mouse.

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. 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 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.

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. 

CUSTOM DECALS

In the image above you can see a custom made scale decal around one potmeter hole which I custom made. 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 and CTRL 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 on the B.Cu layer. I always do this to provide a copper shield for the circuit. I will later connect it to ground via a socket and 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.15

3D viewer version:

Fig.16

Everything you see in yellow and orange will come out in silver on the panel. You can see my panel doesn't have any Silkscreen (white ink) on it so when I make my Gerber files I can switch the F.Silkscreen and B.Silkscreen layers off. This is important otherwise PCBWay will message you to say 'The silkscreen layer is switched on but there is no silkscreen present. Do you want silkscreen?' This will delay the start of production so beware of this.

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! The quality is really good. There are no imperfections on the faceplate which I did have with other manufacturers:

Fig.17

The PCB's with the V-groove. It's executed just like I wanted it to.

Fig.18

The V-groove 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 would do to make it smooth. I'm really pleased with the result.

Fig.19

Look how nicely the potmeter fit into the footprint:

Fig.20

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.21

(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 that the version 2 boards will be perfect.

Fig.22

The space between the boards, separated by pinheaders, is exactly 11mm.

Fig.23

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.

Finally I would like to leave you with the YouTube video that showed me how to make faceplates for modules in KiCad. I learned it all from this video, I can really recommend watching this:

How to Design a Synth Interface in KiCad.

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

Plugin: https://www.pcbway.com/blog/News/PCBWay_Plug_In_for_KiCad_3ea6219c.html.

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.

Synthesizer Extra's No.6: HOW TO MAKE PCB's USING KICAD 9.0

A short introduction to KiCad 9.0 and step by step guide to making PCB's in KiCad. I go through the steps with you and tell you my learning experience.

For some time now I've been watching how many of my website followers have been producing awesome PCB's from the schematics I posted instead of doing them on stripboard. In early May 2025 I decided the time had finally come for me to really get to grips with KiCad because I really wanted to be able to do that too. I had tried KiCad before and I also tried EasyEDA but found both sort of overwhelming. There's so much coming at you that it can seem impossible to get through but that's not true. You just have to know where to start. In this article I will try to explain how I learned KiCad in less than a week. I was advised to go with KiCad over EasyEDA and I'm glad I listened ^___^

Sadly, now I know how to make PCB's this will probably mean the end for the stripboard projects. Naturally, what's on this website will stay here and it will remain free for everyone to use but new projects will now be made with PCB's. More on this later.

First step: what is KiCad?

It's a free software that you can download from here.  (The name KiCad actually comes from the first letters of a company of Jean-Pierre Charras' friend "Ki", being combined with Cad which stands for Computer Aided Design. It was created in 1992 by Jean-Pierre Charras.)

The software consists of two destinct steps. In the first one you're going to draw a schematic and in the second step you're going to turn that schematic into a PCB design.

Once you downloaded KiCad and successfully installed it on your Mac or Windows 10 or 11 PC or your LINUX PC you can open it.

You'll be presented with a small start screen that shows all the options.

Go to the top left FILE section and click on 'New Project'. Choose a name for your project and confirm.

In the screen shown above there will now appear a project file with a schematic symbol and a PCB symbol. Click on the one with the schematic symbol in front of it. You can see my last project in this screen was the TB303 filter.

DRAWING A SCHEMATIC

Now you need to draw a schematic. 

In the Schematic editor, go to 'FILE' and choose page settings. Here you can fill in all the data that will appear in that little text box at the bottom right of the schematic drawing. It's not necessary to do this but it's good practise. 

In this box you can also set the size of the schematic drawing area which is important. You can choose a standard A* size or a custom size.

One more step before you can start drawing. We're going to import all the different components that we're going to need in our schematic like the transistors, the chips, the resistors etc.

To do that you click on the little opamp symbol on the right, 3rd from the top. Now the component library opens up. Actually, it's called the 'Symbol Library' and components are called symbols.

You can search in this library for anything you need. If the specific part you need isn't available, just choose a part that looks the same and has the same pinout. For instance, for the TB303 filter I needed 2SC945 transistors but they're not listed. So I chose the 2SC1815 which has the same pinout and was available. This is not simulation software so that doesn't matter as long as the pinout is the same!

Drag your components somewhere into the drawing. 

You can make your own symbols in the symbol editor if there are for instance rare vintage components that you can't find, you can draw it yourself and assign it electrical characteristics. But I'm not going into that here. And in this tutorial I will keep calling symbols components.

CHOOSING A FOOTPRINT.

Each component needs a footprint assigned to it so the PCB editor knows how big it is and where the solder-pads need to go.

To do this click on your component until it lights up blue. Now it's selected, type 'E' on your keyboard or 'right-click' and go to 'PROPERTIES'. Now a pop-up appears where you can change the value of the component, the designator and there's also a field called 'Footprint'.  It's probably empty. Click on it and you'll see three little books appear at the right of the footprints field, with one book leaning against two others. That's the symbol for the footprint library.

Click on the little books. Now the Footprint library opens. 

Look for your component name and find the footprint with the dimensions you want. This is going to be a bit of a task in the beginning because there's a lot to choose from. Most footprints have PDF datasheets attached to them that you can click and see for which components they were made. You don't have to choose the exact same component name to get a usable footprint. You can assign any footprint to any component, as long as they have the same number of pins. Once you found a footprint you like, save it in your own library so you can quickly find it again. You can edit any footprint in the 'Footprint Editor' which is the symbol that looks like a DIP6 chip with blue blocks on the legs in the top middle of the page.

You can give it bigger pads for instance. There you can also make your own footprints from scratch.

You can create your own footprint library by right clicking in the Footprint Editor, on the footprint name. A pop-up will appear where you can give it a new name and save it, and at the bottom left is a button called 'New Library'. Click that to make your own library that will appear in the list in alphabetical order, depending on the name you gave it. You can not save an alterred footprint back into its original folder because they are 'read only'.

Above is the footprint I use for resistors. 

You need to assign a footprint to one component first and then, when drawing the schematic, when you need more of them you just duplicate the first one by selecting it and clicking CTRL + D. That way all the changes you made and the footprint you chose will be duplicated with the component and you don't have to set one for every little component in your schematic. This saves a lot of work and it's the reason why we import the components/symbols first, before we start drawing.

START DRAWING

When you imported all your components and gave them all footprints you can start drawing. Place the components where you want them and connect them together with the wire tool which is the thin line symbol on the right, 4th from the top. Use CTRL+D to duplicate any component if you need more of them. Like I mentioned before, this will save you having to enter a footprint for every component you use, because it will be duplicated with the component.

Press 'R' to rotate a component. Press 'Y' to switch the pinout of a component in the vertical plane, Press 'X' to switch the pinout of a component in the horizontal plane. For instance the pin numbers of a potentiometer or the inputs of an opamp.

If you have a component that has pins that are not used in your circuit, Like a µA741 IC for instance with pins 1 and 5 that are often not used, then you need to use the 'Place No Connect Flags' tool (Q on your keyboard) and place an X on each of the pins that are not used. That's the 8th icon from the top on the righthand side, shaped like an -X

ABOUT THE POWER SECTION

Now you need to add a little drawing of the power input to your circuit, separate from the main schematic. You need to select a connector with 2 pins (for + and GND) or 3 pins (for + GND and -) or a Eurorack connector or something else and choose a footprint for it. Click on the 'GROUND' symbol (the one with one vertical and 3 horizontal lines under it, you know) on the right and choose for instance the +12V and attach it to the plus line. Choose the GND symbol for ground and for instance the -12V for the negative voltage rail. 

Now go to the ground symbol again and choose the PWR_FLAG symbol and connect a power flag to each of your power lines. +, gnd and -. They must be connected right to the wire that comes out of the power input connector. They may not be connected to wires after components that are connected to the power input connector. They must be directly connected to the input. That way the software knows were the power comes from. You don't have to connect this part to the rest of the schematic. When you use, for instance, +12V symbols anywhere in the schematic, the software will know it connects to the power input section when you used the same symbol.

If you use a voltage regulator on the board, for instance for an extra +5V powerrails, you don't have to connect a power flag to that +5V line. It's only for power that comes into the board from outside.

A little note on placing multiple opamp chips in your schematic. If you place, for instance, a quad opamp like the TL074 in your schematic you choose the symbol and click once to place the first opamp (U1A). Then you click again for the second, third and fourth opamp (U1B,C and D) and then you click again to add the power connections to the opamp. Note that when you click the 5th time you also get a U1E label suggesting there's a 5th opamp that's part of your chip. You must delete this label. I don't know why this happens but be aware of it when you start out.

When you completed your drawing you need to check it for mistakes. You do that by clicking on the Electrical Rules Checker. That's the 6th symbol from the right on the top menu bar. The one that looks like a list with a red circle with a check mark in it.

ANNOTATING YOUR SCHEMATIC

Every schematic needs to be annotated to make sure every component has a name the PCB editor understands. It puts a 1 after the name of potmeters and in- and outputs. If there are sub circuits that work independently of eachother they will be assigned different numbers to tell them apart.

To annotate a schematic, go to the TOOLS menu and click on 'Annotate Schematic'. You can also do this after you changed the footprint of a component for an other one, to update the schematic.

After the schematic is finished and has zero errors you can go over to the PCB editor to turn it into a PCB design. Don't forget to save it first of course.

MAKE SURE YOUR SCHEMATIC HAS NO WRONG CONNECTIONS IN IT BECAUSE THOSE ERRORS WILL BE CARRIED OVER TO THE PCB LATER.

Pay special attention to the power connections of any opamps in your schematic! I went wrong there many times and had components connected to the wrong polarization. The + and - of the opamp inputs are shown very close to the + and - of the power connections so you really need to look carefully to check you got it right.

Also pay attention to the pinout of any potmeters you placed. If the 1,2 and 3 is the wrong way around your potmeter(s) will function in the wrong direction, for instance getting louder when you turn it counter-clockwise. In the case of volume controls pin 1 should be connected to ground. These are easy mistakes to make. (Btw, 1 is left, 2 is middle and 3 is the righthand pin.)

THE PCB EDITOR

Click on the symbol for the PCB editor and let's get designing.

First we're going to go the FILE > 'Page Settings' and again fill in the data for under in the text box of the drawing. It's good practise to do this although not really necessary. 

Now, in the FILE menu, click on Board Settings. Here you can input a ton of things that you want your PCB to comply with. Forget all that for now. I just want you to click on 'Design Rules > Constraints'.

Here you can set the minimum track width and other parameters that influence the copper on the board. I only really change the minimum track width to 0.4 or 0.5mm and leave the rest as it is.

Sometimes when checking a PCB for mistakes you will get a warning that there is a problem with the thermal connection of a ground pad. If you set 'Minimum Thermal Relief Spoke Count' to 1 those warnings will go away.

Now, the moment of truth. 

IMPORTING THE COMPONENTS TO THE PCB

Click on 'Update PCB from Schematic' (the middle symbol of the three shown above) or click F8 to import all your components into the PCB Editor.

You now see all your component outlines in a small space. This is called the rats nest.

Now you need to pull all this out with your mouse and start placing the components on the field in somewhat the same position as they have on the schematic. This way you get the shortest tracks between them. Pull it all out and use as many space as you want. When you have everything ordered you can start placing the components closer together and build up a nice compact PCB layout with the shortest tracks possible. You will see what is connected to what when you drag the components around.

You'll see a thin line that connects the component to other components. Sometimes, when you drag a component around, those connections will jump between different points. Those are usually the power and ground pads and the software chooses the shortest connection.

The Ratsnest:

When I need to place a component I select it and switch back to the schematic to see which components and especially IC's are close to it. Then I switch back to the PCB editor and place the component near those elements. This helps in getting the shortest tracks.

Once you got all this done you can start drawing the traces between the components by hand. There is a plugin that you can install, that will do it automatically, but I want you to do it by hand. This works much better. You must choose the F.Cu layer to draw on the front of the board and you must click on the B.Cu layer to draw on the back side. It is good practise to draw as many of the horizontal tracks on one layer while drawing the vertical tracks on the other layer. This prevents cross-talk and noise.

I have developped the habit of drawing as many of the tracks on the back side of the board and then draw the rest on the front. Do whatever you find works best for you.

If you can't lay a track because the way is blocked by other tracks, attach a 'via' to move to the other side of the board and continue the track there. To place a Via, right click on the active track as you're laying it and choose 'place through via'. Make sure there is no track sticking out in front of the via. That can become an unconnected track later and you'll have to find it and delete it. Before planting the Via in its place I always shake the mouse a little to get rid of bits of track sticking out where I don't want them.

TIP: Leave all the connections marked 'GROUND' unconnected. We're going to use a groundplane to connect all those together at once, later.

AFTER THE TRACKS ARE DONE.

Okay, so you have your first PCB set up. Now you need to define the edge of the board. Select the 'Edge Cuts' layer for that. Now choose the 'Draw Rectangles' tool and draw a square around your board. Leave a few millimeters between the outline and the outer components.

Once you have this done you can choose to round off the corners. For that, right click on the outline of the board and choose 'Shape Modification' from the menu. You can enter the radius of the curves in millimeters. You can also add mounting holes in the corners with the circle tool.

In between all these steps, regularly check your progress with the 'Design Rules Checker'. It will tell you what's wrong with the board. If you don't understand a certain mistake that is listed, just Google it. Many have gone before you and there are solutions to be found for all the possible mistakes you can make.

Checking for mistakes is called running the DRC but I always call it 'Run DMC' after the rappers :)

Oh, very droll sir!

If you need to make a board to a specific measurement, you draw the edge of the board first, before you start drawing the tracks.

ADDING GROUNDPLANES.

One more step is to add groundplanes to fill up the board with copper and connect all the ground points together. Click on the B.Cu layer and now click the 'Draw Fill Zones' symbol or click CTRL+SHIFT+Z.

Take that tool and draw an outline around the board just like the edge cuts outline. Use the mouse wheel to zoom right in on the corners. When the outline is completed, go to EDIT > Fil All Zones or click 'B' to fill in the backside. Now select the F.Cu layer and repeat the proces for the front layer.

Again do the Run DMC, I mean run the DRC to check for errors. The warnings are not vital but the errors need to be fixed before a PCB can be made. But you'll learn soon enough how to fix the warnings too. Google is a great help for this.

You need to be aware that there will be places where the groundplane can't reach because it is blocked by tracks from all sides. In that case you'll have to connect those grounds together with a track and make sure the track reaches a ground pad that is covered by the groundplane. An indicator that such a problem occured is when you get an error without explanation. 

ADDING TEXT.

You will see that the Silkscreen text next to the components (the one in yellow) only shows the designators. It's handy to put the values in too. You could double click on the designators and change them to values but then you'll get a lot of double designator warnings and should you make any changes to the board after that, all your text will flip back to designators and you can start all over again. No, it's better to click on the F.Silkscreen layer and use the TEXT tool to put the values next to the components. Make sure your text doesn't touch any of the solderpads or the yellow lines around the components. That will give problems in production with the soldermask overlapping the silkscreen or text overlapping silkscreen.

Below is the PCB for the very popular Resonant Lowpass Gate module. Note I placed the potmeters right at the top edge so the PCB can be mounted by soldering the potmeters straight in and using them to mount to the front panel. Resistor designators and values are all contained inside the component outline box. I always drag the designators to the top left and write the values in at the bottom right.

You can see what your finished board will look like by clicking on the 3D viewer or clicking 'ALT + 3'. This will even work if you haven't drawn the outline of the board yet.

ADDING LOGOs OR IMAGES TO YOUR PCB.

As you can see the PCB design in the previous picture has a picture of my logo in it.

To add an image to your PCB first measure the space on the PCB where the image will sit in mm. 

Now click in the main start menu we used at the start, on the Image Converter.

Click on 'Load Source Image' at the top right.

Load your image and set the output size to the size you measured.

Choose Footprint Layer F.Silkscreen

Click 'export to clipboard'

Now go back to the PCB editor and click <CTRL + V>. The image appears and you can drag it in place.

You'll see a G*** watermark over your image. Just click on it and press delete on your keyboard.

To place an image on the backside of the PCB just press 'F' on your keyboard to flip sides.

And that's how that works. 

MAKING THE GERBER FILES.

Now all you need to do is make the files necessary for production of the PCB's.

First do a final check and make sure your design is faultless. A few warnings will probably remain in the beginning but they are not crucial but 'errors' must be seen to and repaired.

A common problem will be that you need to move a component a little. To do that you must first go to Edit and choose 'Unfill All Zones'. Then you need to click on all the tracks connected to that component and delete them. Then move the component to its new place and reconnect the tracks. Then refill the zones by clicking 'Refil Zones' and then checking the Run DMC eurrh run the DRC.

Okay, now we want them files, hand them over!

Click on 'FILE > Fabrication Outputs' and choose Gerbers.

You can leave all the settings at their defaults, at least if you order your PCB's at JLCPCB which I recommend. Make sure 'Subtrackt soldermask from silkscreen' is checked on. 

Now at the top, fill in the destination folder for your files. Click on the folder symbol and go into your project folder and make a folder with the name of the project followed by 'gerbers', or something like that. You can give it any name you want.

Next you need to choose that folder as the destination for the Gerber files.

Now click on 'Plot' at the bottom and your folder will be filled up with Gerber files. But we also need to make the drill files so in that same field click on 'Generate Drill Files...'. A new pop-up will appear:

Leave everything as it is in the picture above and click on 'Generate'. Then click 'close'.

You will know when you checked something on that you shouldn't have, because JLCPCB won't accept it. You'll get an 'Parameter Exception' error message when uploading the Gerbers to their website.

Your production folder will now contain 14 files.

Select all these files with CTRL + A and then right-click and put them all in a ZIP file.

ORDERING YOUR PCB's

After you finished your first projects you will be tempted to order the PCB's rightaway. Don't do that just yet. Sleep over it until the next day and then before you order, check your schematic for errors. Believe me I speak from experience. I thought I had been so thorough in checking but when I started out I spent more than €200 on PCB's that could go straight in the bin because they contained hidden errors.

You need a clear head for this and the mistakes will jump out at you. This saves you money and disappointment. If you have discovered errors you need to fix them in the schematic first. Then save the schematic and go to the PCB editor and import the changes from the schematic. Now you must also make the changes in the PCB design en run the DCR checker.

Naturally, if you corrected errors you must make new Gerber files before ordering your PCB's. Delete all the faulty Gerbers before you make new ones to prevent mistakes,

When everything is fine you can go to the JLCPCB website and drag that Gerber ZIP file into the box 'Add Gerber File' and you will instantly see you design appear on their website with how much it'll cost you (usually € 2,- for 5 PCB's). 5 PCB's is the minimum you must order. You can choose between a few colours like purple, yellow, red, blue and green. An other colour does cost a little extra though and it takes 2 more days to produce,

If you choose green boards and use the most cost effective shipping (€1,50) your boards will cost about €0,85 a piece for a minimum of 5 provided they are smaller than 10 x 10 CM. The cheapest shipping option is 'Global Standard Direct Line' which takes 12 to 16 businessdays.

An there you have it. Now you can make PCB's. I found the proces quite addictive and for the last week I've been doing nothing but sit behind my two PC's making PCB's :)  (The schematic on one PC screen and KiCad on the other.) Dispite it being beautiful spring weather outside. I love it! I've already ordered two filter designs and the last one, the TB303 had zero errors and zero warnings and I've only been doing this for a week!!

Make at least 4 test projects before you start thinking of ordering PCB's. I've invested a full week in learning. I spent at least 10 hours a day on this because when I set my teeth into a new project I simply can't stop until I understand it. You'll need to be determined to learn this and then you will see quite soon that it is really not that difficult.

If you have any questions about this proces I'd prefer you this time to post them in the Facebook group first. You'll get answers sooner because a lot of the group use KiCad.

SOME COMMON WARNINGS AND THEIR SOLUTIONS:

Here I will list warnings, and errors and their solutions. I'll add to the list as I come across more.

I've had many different problems to solve when using and learning KiCad but I didn't write them all down but here are some I came across the most in KiCad.

FIRST TRY THIS.

With most errors, it's just a matter of updating from the schematic, so in the PCB editor click 'update changes from schematic' even if you haven't made any changes. Now open the DRC checker and click detele all markers and run the checker again. Errors and warnings that show up now will have a valid reason for why they are there.

INPUT POWER PIN NOT DRIVEN BY ANY OUTPUT POWER PINS:

The input of a component that needs a connection to the powerrails seems not to be connected to any power rails. 

If you are sure your schematic is solid and faultless, you can simply ignore this warning.

"TRACK HAS UNCONNECTED END" warning. This is a warning not an error meaning that if you order your PCB with this issue unresolved, you'll probably still be okay.

This warning comes up when there are little bits of track underneath an other track, maybe from moving a component and reattaching the tracks. Anyway, to solve this, go to TOOLS > 'Clean up tracks and vias'. If that doesn't work, pull the component out of the board and check underneath for bits of track. Delete them and the track that attached to the component so everything is clean and then put the component back in and reattach the tracks.

Now check the Run DMC thing again and your problems will probably be gone. If not, go to that track, delete it and draw it in again.

NO ERROR WARNING BUT THERE'S STILL A RED CIRCLE when I do the DRC.

If, like me, you connect all the grounds together by using groundplanes (fill zones) for the front and back layers then you can get this error. There's no error message but after the test the error circle stays red with a number or errors listed. This usually means that there are connections to ground that can't be made because the fill zone can't reach that component. The component is shielded by tracks. In this case you have to unfill the board and connect those grounds together with tracks. 

It can also be an other track. When you see the red circle with a number inside and no warning text, this can mean there's a track you've forgotten to connect. Go over the board and look for unconnected components.

MISSING FOOTPRINT and EXTRA FOOTPRINT for the same component(s).

I'm not sure what causes this but it happened to me and I went back into the schematic, right clicked on the component the warning applied to and, opened 'Properties' and just clicked on the same footprint I had already chosen for it. Then I updated the PCB from Schematic and the problem was gone.

TIP: If you want to delete all tracks and start again you can do so by going to  EDIT > Global Deletions. There you can check what you want to delete and then it will be deleted for the whole PCB.

HAVE YOU EVER WONDERED HOW THOSE PCBs ARE MADE IN CHINA??

Watch this:

And that's it for this tutorial. I hope it was helpful for you.

Synthesizer Build part-68: VC DELAY by BMC.

This is BMC 83 the voltage controlled delay using the Princeton Technology (PT) 2399 chip. This is a eurorack friendly project.

Dispite the fact I built over 68 projects I never build a digital delay or reverb, except for project 11 but that was a ready made effects unit. This project takes care of that. It can deliver good fidelity delays of up to 1 second. It can actually do delays of upto 4 seconds but then the fidelity drops fast. The PT2399 wasn't made for such long delay times but shorter times, upto a second, sound really good and with the long times you get some cool distortion, sort of a bitcrush effect.

This was quite an easy project to build. You can find the original article on the Barton Musical Circuits website. There are audio demonstrations on that website so you can hear what the delay sounds like. I also made a demo video myself which you can find at the bottom of this article.

This circuit will work fine on both a dual 12V or a dual 15V powersupply.

The finished delay module

Here's the schematic I used to make my layout from. I changed the opamp numbering to match that of the layout.

I didn't use the 10 Ω resistors in the powerrails as shown on the schematic. But if you have problems with hum you can include them. On the layout below, you could put a 10 Ω resistor from K-3 to I-3 and then lead the red wirebridges from there and the purple wirebridge could be replaced with a 10 Ω resistor for the negative voltage rails.

The diode and 1M resistor in combination with the 100nF cap and the top transistor with collector to pin 6 of the PT2399 make up an anti latch-up circuit that presents a high impedance to pin 6 in the first 400mSec after you switch on which gives the internal oscillator time to warm up and prevents the chip from latching up and crashing which can happen if the resistance between pin 6 and ground is less than 2K at start-up. After start-up this resistance can be much lower but not a straight short to ground. In this module the resistance is then controlled by the second transistor which is opened up by the time control potmeter or external CV input. This resistance controls the delay time.

So there are voltage controls with level potmeters for the delay time and the return amount and the module has an audio output that outputs just the delayed signal and a mixed audio output which mixes the original signal in with the delayed signal controlled by the 'Mix' potmeter. There's also a tone control potmeter which also influences the return time I noticed (see demo video below)

The delay time range goes from 60 milliseconds to 4 seconds but like I mentioned earlier the audio fidelity drops quite a bit with longer delay times, mostly at times longer than 2 seconds but that doesn't have to be a bad thing. It has quite a cool distortion effect. With the longest delay times you do get some clicks and artifacts mixed in the audio but it's not much. The delay times are controlled by the two transistors forming a voltage controlled current sink. The 47 Ω resistor at the emitter of the bottom transistor determins the shortest delay time while the 330K in parallel from the collector to ground determins the maximum delay time.

In my own build I did notice quite some dead space at the beginning (ccw side) of the 'Time' potmeter but lowering the value of the 47 Ω resistor didn't do anything. 

I urge you to download the PDF accompanying the original project. It has a comprehensive description of how the circuit works and what all the components do. 

Here's a block diagram of how the delay works. This is also from the PDF that comes with the build instructions on the BMC website. 

Audio in 2 is the Return input and it has the Direct Output normalled to the socket switch. So if you take the direct output into an external effect module and take the output from that module and connect it to the return input you can have an external effects loop going, creating all sorts of possibilities. You can, for instance, lead the direct output into a lowpass filter and have the VCF out connected back to the return input.

HOW TO PATCH UP THE MODULE:

To get the best out of this module you need to make a synthesizer voice in your modular synthesizer where this delay sits behind the VCA at the end of the signal chain. You can also patch it up so that the delay sits inbetween two VCA's and have the second VCA opened by an ADSR with a slow Release time. That way you get more control over the Delay time, but it's not necessary. The minimum Delay time is 60mSeconds so it won't be able to create flanging or chorus effects. But you can mix in the effect with the clean signal by using the Mix control and the Mix output.

LAYOUTS:

Here are the layouts I made for this project. They are verified as always. I used them to build my module. This was almost another hole in one. I made one little mistake. I had all four non inverting inputs of the TL074 grounded only the last opamp with the direct output must not be grounded. Once I corrected that the circuit sprung to life. Pins 5 and 10 of the TL074 are connected through the strip underneath the chip. The 'Tone' control potmeter has pin 1 not connected. It's important to wire it the way you see in the layout or it won't work properly.

Wiring:

Stripboard only:

Cuts and wirebridges. You know the drill, mark the cuts on the component side using this guide and then stick a pin through the marked holes and mark them again on the copper side. Then cut the marked positions with a hand held 6- or 7mm dril bit.

Don't forget to cut position P-8 underneath the ground wirebridge.

Here is the Bill of Materials. 

It might be a good idea to use a logarithmic 100K potmeter (A100K) for the return potmeter. A lot of changes happen quite early in the throw of that potmeter. However I used a linear 100K myself and that works fine too. But the log type would be more convenient. You could use other value potmeters for all but the Tone Control. That has to be a 10K linear potmeter. The other potmeters are just voltage dividers in this circuit.

PICTURES:

Here are some pictures from the build proces:

I left out the two short wirebridges that connect all 3 ground strips at the eurorack connector together. Instead I soldered them together with some extra solder bridging the gaps.

Stripboard all wired up for testing. I normally only wire things up when I have the panel ready so I can keep the wires as short as possible but with this module I had to be sure first that everything worked. Anyway, it made mounting the board behind the panel easier coz no need for soldering and I was able to stuff all the wiring underneath the stripboard out of harms way.

This is the panel with the waterslide paper applied ready to receive a final thick coat of clear lacquer. The panel is 14hp wide (7CM). the width I normally use because it allows me to mount the stripboard flat behind the panel keeping the depth to a minimum.

Here's the panel design I made in Photoshop just in case you want to use it. It's in A-4 format 300pix/Inch resolution.

Module on the test bench:

The rear of the module. It's 3.8 cm deep so it will fit any Eurorack case.

VIDEO DEMO:

Here's a little demo I recorded showing the module in action.

Here's an interesting look at the inside workings of the PT2399 chip: --- click here ---

Okay, that's it for this one. Hope you like it.

If you have any questions or remarks about this project please put them in the comments below. Remember comments are moderated so they don't appear straightaway. Only after I read them.

You can also post questions on the special FaceBook group for this website.