KiCad 7 Tutorial: PCB Constraints, Net Classes & Directive Tool

[00:00:00]In this video, we'll start with adding some  design constraint to the PCB layout editor, so we don't design something that's very expensive or very difficult to manufacture  in a fabrication plant.

[00:00:17]For this, we'll go to the board setup and then  click on constraints. Here we need to fill in the values that a fabrication plant can handle. So,  anytime we go above this threshold value, Kicad will warn us and try to keep our design within the  manufacturing limit. Usually all fabrication plant will provide a capability list which we can use to  fill in this data. If you're just getting started and not sure which fabrication plan to choose, we  have a whole section of articles dedicated to that.

[00:00:49]For now, I'll use this capability list, because  most of the manufacturers can handle these values very easily. In Kicad, we have these  default constraints, let me quickly explain what and why we have these constraints using some  examples. First we have the minimum clearance, This would be the minimum distance between 2 tracks  and when we go below this value we might see some weird artifacts or shorting of the tracks. This  is because of the process called etching which is done during the production. To avoid this  we can always design the board a little above the fabrications capable value to be on the safer  side. So in this case, the capable value is 0.1 mm but 0.15 is a good value and also is recommended  by the fabrication plant, so we'll go with that.

[00:01:40]Then we have the minimum track width,  which is basically the thickness of the track and similar to the previous value,  this thickness is greatly affected by the etching process, if it's anything below the  threshold value, the tracks might cause open circuits in the PCB. And according to  the capabilities list it is 0.15 mm.

[00:02:02]Then we have minimum connection width which  is similar to the track width but this is the connection between 2 components or connection  between a component and a track. Similar to the track width, if it's less than the threshold  value the PCB etching process might break the connection, so we'll enter the similar  value. Then we have the minimum hole size, In this case it's 0.3 mm. You can go well below  this value but it would make the PCB very expensive as they have to use different process  to make the hole instead of just using a drill bit.

[00:02:37]Next we have the via size of 0.5  mm and the annular clearance is 0.1 mm.

[00:02:43]Sorry for throwing random words at you, but  the video would get longer and longer if I explain each one of them. To solve this we have  created a cheatsheet of all the terminologies into a single page which you can always refer  to when you don't understand these terminologies.

[00:03:00]So I entered those values over here, 0.3, 0.5 and 0.1 mm. Finally we have 2 more clearance  values, minimum track distance and minimum track distance between the edge of the PCB. The first  value will help in making sure we don't take the tracks too close to the holes, so the tracks  won't be damaged while drilling during production.

[00:03:23]Similarly the second value will help in making  sure we don't take the tracks too close to the edge of the board so it won't be damaged or  chipped off during the final stage of production.

[00:03:35]The hole to hole clearance just makes  sense you can't have two holes close to each other during drilling so they don't form  a single slot instead of two different holes.

[00:03:45]Then we have Micro Vias, these are very little  to advance for the current circuit that we are working on, so we just skip this and go to the  Silkscreen. Here most of the terminologies are self-explanatory. So I'll just take the values from  the capability list and just enter them over there.

[00:04:03]We'll come back to these values when we are  doing Zone filling at the end of PCB design.

[00:04:09]Then we have length tuning which we can just  keep it checked. Next we have predefined sizes.

[00:04:17]Let's predefine some track width which we  can use in the circuits, it's very similar to how we choose a wire to make the connection  based on the current rating of the circuit.

[00:04:27]For this circuit we are working, we'll just  need 2 different sizes, one for signals and the other one for power tracks. To calculate this,  we can use the calculator that's within Kicad.

[00:04:39]Just go to the Kicad project  window and click on calculator tools.

[00:04:47]Then click on track width. If you like to know how  the calculation is done you can see the formula is given here with some explanation. Since  our circuit is very simple we can just enter the maximum current it would carry during  operation. I'll just enter 1A for now.

[00:05:03]I know the circuit we built in the previous videos  won't even be close to 0.5 A but decreasing the current consumption decreases the track width  which will make the track width less than our clearance value that we just set a while ago.  Then for the temperature rise and trace length I'll just let them be default. As our circuit is  simple and small these factors won't affect much.

[00:05:27]Then finally there is one more factor to include,  that is the trace thickness and for this value we have to pull up the capability list again. And if  you look at outer layer copper thickness, we have 35 micrometer, 70 micrometer and  105 micrometer. In our case, we'll just go with 35 micrometer which is  also the default setting on Kicad.

[00:05:50]Now based on the information we gave Kicad, it  gives the track width of 0.3 mm which will include in the predefined sizes. There is also something  called as Internal Layer Traces, these values we can consider when we are trying to build a  multi-layer PCB, so this won't be much of help now.

[00:06:07]Since now we know the track width, I'll create a  0.3 mm track width for signal and additionally I'll create a 0.5 mm track width for power. I'm  doing this just to show the difference between power and signal tracks, but theoretically 0.3mm  would be good for signal and power in our circuit.

[00:06:25]Then we have Net Classes, if you remember from  our fourth video about schematics and adding net labels, we discussed how we can give name to few  connections for easier understanding. Similarly we can use Net classes and create a group of  connections that will share similar properties.

[00:06:43]For example we can create 2 net classes  one for signal and other for power. Now using these two classes, we can assign the  thickness to the traces automatically, Instead of using the predefined sizes each  time you switch between power and signal tracks.

[00:07:01]So far we have just created the classes  but never really assigned the classes to the connections that we made in the schematics.  We can do this in two ways, we can either do the assignment here on both setup or we can do the  same on the schematic setup. Personally I would prefer using the schematic setup. So let me close  this. So let me open the schematic editor. Now if you click on any connection and see the bottom  status bar, you can see we have the connection name but the net class is set to default. But  in our case we want to change this to signal.

[00:07:35]We can do this in multiple ways but the  easiest way would be just do a right click on the connection and click on assign net class and  under this the current name is set to slash LDR.

[00:07:47]This is just the net label that we assigned  and here we can set what kind of net class we need to assign for this connection. In this  case we'll set it to signal and click on OK.

[00:07:57]Now if I click on the same connection again, you  can see the net class is set to signal. Now if I click on any connections that's related to LDR,  you can see the net class is automatically set to signal. We can either do this process for all the  connections or we can go to the schematic setup and here we can just enter the name of the  connection and Kicad will try to automatically assign the net classes for these labels. So  let me do that for MIC and set it to signal and similarly let me do it for LED and signal.  Then we have ground, that'll be the power.

[00:08:38]Then we have plus 3.3 V that will be power as  well. Now there is a slight bit of a problem here. We have assigned the net classes only to  the connections that have names but what about the ones that's unlabeled? For example, this  connection which has the default connection name net d1k and net class is default. Since  they are unlabeled there is no way to search for the pattern without a name that we manually  assigned. So how about we manually try to assign.

[00:09:09]Seems like we can't assign the net to  this connection without adding a net label.

[00:09:14]We can fix this quickly by adding a net label, but this process would become very difficult  when we are trying to make a complicated circuit.

[00:09:26]In Kicad 7, we can solve this by using net class  derivative tool to assign net classes to unlabeled connections. Click on the icon here, add in a class  derivative label. On this menu select the net class that we want to assign to the connection. In our  case it's the signal. We can use the below settings to show how they appear on the schematic diagram.  In my case, I'll keep it very simple select the dot and also I'll cut down the length by half and then  hit OK, and now we'll place it on the connections.

[00:10:03]And personally I don't like the names that's  sticking out so I'll click the net class label and press the letter E and under here you have  the option called show and I'll just uncheck this and click on OK. Now with this when we click  back on the connection we can see on the status bar that the net class has been assigned to  this connection. Now I explain how to assign the class name for labeled and unlabeled connections,  let me quickly do that for the whole circuit.

[00:10:37]Now I have assigned all the net classes.  To just make sure the schematic editor is reflecting all the changes to the PCB editor,  I'll close this and open the PCB layout editor.

[00:10:50]And here I'll open the board setup, and here we can verify both setup net classes  and the schematic setup net classes match up.

[00:11:01]I know this is an insane amount of work for  a very simple circuit but you need to trust the process. These settings will really help a  lot in making a very good PCB at the first try.

[00:11:12]I keep using these sentences from the past two  videos that will be bringing the footprints that we assigned into the PCB layout editor but so  far we took so much time just talking about the constraints, PC layout editor and so many other  things but in the next video we'll make sure we get all the footprints into the PCB layout editor  and we'll finally start working on our first PCB.

[00:11:35]And we really appreciate any doubts or questions  related to the topic that we are making and we are always thrilled to answer each one of your  questions but please try to consider PCB Cupid QnA for a few of the questions, all you have to do  is just a one-click login and ask your questions.

[00:11:53]It'll really help us in producing more videos  frequently also it will help many users who are just getting started with Kicad. So until next  video, keep learning and keep creating.