Original page created on 19/03/2020; updated on 22/11/2021.
Circuit Design
Launching PcbNew
Let’s start by clicking the appropriate button, either in the project manager…
… or in Eeschema
We can notice some inconsistency in this tool’s description…
The working screen appears. First observation: the frame of the “sheet”, in very dark red, is almost invisible. I find this quite annoying, if only to read the title block of the drawing. We can improve things a little by asking Show page limits in the Preferences menu, which gives a white frame, but which does nothing for readability.
Curiously, we can modify the colours in Eeschema, but not in PcbNew…
While we are in Preferences, I recommend that you change the cursor so that it spans the entire screen, which makes it much easier to align the devices relative to each other.
Import of AutoCAD diagram
First of all, let’s fix the origin of the work grid, which will correspond to the origin of the AutoCAD drawing. The button is located in the right-hand bar, where, as in Eeschema, the placement controls are located.
Let’s place it towards the middle vertically, and to the left of the sheet.
This way, this origin will correspond to the axis of the board. Note the X-Y position of this point, here 7.6 and 100.0 (let’s neglect the 1/100…).
Before importing the DXF drawing, let’s select the layer that will receive it. It will be an xxx.User layer, reserved for this use. Let’s choose a layer of a well contrasted colour, yellow for example. Note that you can change this colour with a right click. Leave this and click the desired box.
Now select File / Import / Graphic…
Several things are to be defined here:
- The name of the DXF file to import;
- The insertion point abscissa: type in the value previously noted;
- The ordinate of this point;
- The line width. It is advantageous to put a low value for more accuracy;
- The layer in which the drawing will be placed. Be careful not to put it in a “reserved” layer.
Let’s validate. The drawing appears at the expected point.
Drawing of the outline
You would think that it is already here, since it is part of the previously imported diagram. I thought at the beginning that it would be easy to select this outline in the User layer, then change layer using the properties. Unfortunately, it doesn’t work: you would have to select each line in turn to do so. When it’s a simple rectangle, that’s fine. But if the outline is more complex, it quickly becomes very painful.
I found it faster to take the AutoCAD diagram, erase everything except the outline, export it to DXF under another filename, and import it again, but this time of course on the Edge.Cuts layer.
It’s still a shame that we cannot edit a set of objects together, however of the same kind (lines or texts). However, you can select several objects, either by framing them with the mouse, or one by one, by clicking them with the Shift key pressed. For texts, you cannot change their size for example in a global way…
Note about selection with the mouse. It is done in the same way as with AutoCAD: if you drag the selection rectangle from left to right, only the objects fully included in this rectangle will be taken. If you drag from right to left, even objects crossing the rectangle will be included. It can be useful for selecting a single object, a line for example, which cannot be captured with a single click…
It’s good to be inspired by AutoCAD, a little more would be better: In my opinion, it lacks an orthogonal mode and an object snap mode, even simplified. Admittedly, the outline drawing hooks a line to the previous one, but it is often random and it doesn’t work on all the layers.
Importing devices
The netlist will allow us to import the devices.
After validation by Update PCB:
A bunch of devices appears, which we place haphazardly, near the layout drawing.
At the moment, they are highlighted, which means they are selected to be moved or rotated, etc. Let’s click (or Esc) to fix them. We will now have to position them one by one. Let’s be patient! With the preparation already done, it will go quite fast. For the moment, let’s choose a fairly rough layout grid, say 5 mm.
Placing the devices
Let’s start with the easiest one: the LEDs. Let’s do Edit / Find (or Ctrl + F), and type in the part number, in order to select it. Here, I have asked for H1, which is the reference of the first LED.
Bad luck! KiCad selects the name of the device, on the Dwgs.User layer (circled in red), not the device itself (circled in green)! No problem, we know where the device is, we can delete its name. Just press Delete, as it is already selected. Let’s search again (Ctrl + F). This time the device is highlighted, ready to be moved.
To do this, we will proceed in two steps. Firstly, type M (Move). The cursor is now at the centre of the device: move it to the origin of the drawing.
In a second step, do Ctrl + M to request a relative move. Do you see what I mean? Just type the horizontal displacement, here 7.4.
The device moves to exactly the right place!
Even better: before moving the next device (here C1), select its dimension text, type E (Edit), then Ctrl + C (Copy). The text is then copied to the clipboard.
When we get to the second, relative, move, we’ll simply paste the text into the Move Item window. When the dimension text is a bit complex, this can avoid a copying error. With practice, it’is very quick.
Here is the current displacement of the capacitor. In the Move Element dialog box, I typed 14.3 for Move X: and 3.28 for Move Y:. There is a little problem here: the location point is not the centre, but a pad. We’ll have to correct the position of this device, whose location is not critical anyway.
Personally, for each device placed, I remove its dimension text from the Dwgs.User layer as well as its reference if not already done. The less the drawing is filled, the better.
Place devices on the other side of the circuit
The LEDs and the capacitor must be located under the board, the other devices above. For the moment, everything is above. To change a device’s side, just press the F (Flip) key. So put the LEDs under the board. We see that the texts are reversed, which is logical.
What is less logical is that the side change, which is in fact a rotation in space, is always carried out along the X axis, regardless of the position of the devices. So a polarized device (diode, capacitor) will see its polarity reversed if it is arranged vertically, along the Y axis. This can be annoying especially if we have already routed the tracks.
Here you have to press R twice, so make two 90° rotations to find back the correct position.
Track routing
First of all, we have to decide the track width. The default, 0.25 mm, seems a bit weak to me (old reflex from someone who etches — etched — his circuits himself and who fears that such a thin line will be eaten). I choose 0.5 mm. This value doesn’t exist by default: you must type it in the box that opens when you click Edit predefined sizes.
Then, we must (1) designate the copper layer on which you are going to draw, F.Cu (front) or B.Cu (bottom), and (2) click the Route track button.
To draw the tracks, it is obviously necessary to be based on the ratsnest. It is best to start with the shortest and therefore most obvious links. Here we are going to connect series of LEDs and resistors. But since some are above and others below, we will have to go from one side to the other by installing vias, which are small diameter holes used to make the two sides communicate electrically.
I start by clicking the starting pad, which is on the top side. When I reach halfway, I type V: a via appears. I can move it if necessary then I click at the desired position.
The track then automatically changes sides, and therefore turns green. I finish by clicking the destination pad. Notice the track highlight. That’s it: the first equipotential is connected!
I pass on the continuation of the routing, which requires a certain experience, but which is not too difficult for such a simple circuit. I come to this:
