Group Actions
Engagement
  • Author Author: michaelkellett
  • Date Created: Date Created
  • Views 1233 views
  • Likes 10 likes
  • Comments 10 comments
Related
Recommended

First Design with KiCad (8.0)

michaelkellett

I’ve been using the same PCB design software for over 20 years (Easy PC) and it’s served me well during that time. It’s had an update pretty much every year and it can still load files from 20 years ago. It hardly ever crashes and I’ve probably designed more than 300 boards with it.

So why am I writing this blog about Kicad ?

It’s because there is so much talk about KiCad and how good it is – and two other reasons that are becoming more and more important.

Easy PC is Windows only but Kicad will run on Windows or Linux platforms – this is becoming important to me because I think my patience with Windows is close to exhausted. I feel the weight of the enforced changes of OS, the constant pushing of their AI and cloud stuff and the general customer contempt crushing me. I don’t think I’m ever going to run Windows 11 as my main OS.

The other reason is that the popularity of KiCad means that more and more of my customers are likely to be using it, and because it’s free to install even those who don’t can easily load it to share a design if they wish.

There is a there, slightly off the wall reason. Altium, the biggest player in the mid-price sector I believe, has been bought by Renesas – so as far as I am concerned is no longer a sensible choice of PCB Cad supplier. I expect a lot of other people to react the same way.

So I decided that the next non critical internal (ie not for a customer) design that I would use KiCad.

I installed version 7 on a Linux machine and never quite got a suitable opportunity but recently I was looking at  a broken HP59313A.  This is a 4 channel 12 bit ADC capable of a staggering 12 bit resolution and 200 samples per second with HPIB (GPIB) bus interface. It is very old (47 years), cost me very little and doesn’t work. The first fault I found was a dead LM309 voltage regulator in a TO3 can. These parts are no longer made and although second hand (or even claimed new and unused) parts are available they cost silly money and can’t be trusted.

image

As you can see from the picture I bodged in a 7805 which got the 5V supply up but didn’t get the box working. But I though that making a TO3 shaped PCB with a regulator on it would be nice because this is not the first dead LM309 I’ve seen.

At first I was thinking of a linear regulator but looking on the web I found a design using a switching regulator. It was done a long time ago and used a rather dated switcher. While I was looking an email flyer form Linear Technology/Analog Devices turned up promoting their Silent Switcher 3 parts. These aren’t quite right for my intended spec (won’t take a high enough input voltage) although otherwise very good. So my design is going to use a Silent Switcher 2 part – the LT8640S.

And I’m using Kicad 8.0 to design the board.

First Impressions of KiCad

I bought some books (two, KiCad Fundamentals and Projects and KiCad Advanced Projects and Recipes both by Peter Dalmaris (on offer from Elektor as a bundle !)

I did not read all 590 pages of the Fundamentals before starting !

I dipped and then got on with it.

My biggest problem with KiCad is that it isn’t Easy PC. When you have 20 years experience with some software anything else is bound to feel a bit weird.

The schematic editor isn’t too hard to get used to but I found the part chooser a bit of pain. I was able to find a symbol and footprint for the LT8640s (on SnapMagic) quite easily and rather less easily add it to the library. This later cause a bit of a problem but it was the symbol not KiCad which I think was wrong.

Anyway – it wasn’t that hard to get a schematic done.

image

Translating to a PCB and placing that was OK. This is an odd design in that some parts must be placed in just the right positions and linked with lots of vias to ground or with copper pours rather than tracks. High speed switchers just don’t work right if you ignore this.

It was quite slow going because I had to keep looking up how to do stuff -  but that was to be expected.

The SnapMagic schematic symbol has all ground pins and the 4 little unconnected corner pins on top of each other. I thought this was a KiCad thing and was a bit disappointed by it but when I realised that all that was wrong was a whole load of ground pins being placed on top of each other in the schematic symbol I was soon able to edit it into something sensible. What I can’t understand is how any one could have thought that was a good idea -  not all ground pins are the same – even though they may be linked inside the chip.

Back to the layout – KiCad was a bit easier that EasyPC at allowing me to add vias to the PCB footprint of the LT8640s.

I don’t like the manual routing -  the software still keeps trying to coerce the track into silly shapes. This may be the way I have things set up and I shall experiment more before whinging. I like to route with a snap grid and without 90 or 45 degree constraints and then to adjust things the way I like. I might well break some clearance rules and move things later.

One snag that bit me was trying to set the outline of the TO3. The first problem was that KiCad calls the board outline the “EdgeCut” layer -  logical enough but hard to find when you search for things like “outline”. I had to actually read the book a bit to find that one.

Then I hit a big snag – all the footprints from the library were making solder paste and solder mask apertures exactly the same size as the pad.

I spent the next two days on and off searching for a global way of setting a different default. I could easily change every pad on the board one at a time. I found several hits on the web that suggested that there is not global way to this and advised people to edit the PCB text file or write scripts. The index in the Dalmaris book is very week and while it does tell you in the book you won’t find it in the index.

Having done a good deal of cursing I returned to web searching and found what I needed. I’ll share it here in case it’s useful:

In PCB Editor click the Board Setup button.

Click Solder Mask/Paste under Board Stackup

Enter things for solder mask expansion and solder paste relative clearance.

image

So of course KiCad lets you set these things globally and its actually in a sensible enough place !

image

Now I could make the Gerber files and order the boards. It’ll be couple of weeks before they come back and I get bits on them and I can share some test results.

Conclusions

In conclusion – not too bad an experience. I’m not going to criticise because I haven’t used it enough to be sure that any problems I have are the software rather than me. But I didn’t hit any showstoppers. I think KiCad (on the basis of my limited experience)  is a competent offering in the low - to mid performance sector of the PCB CAD market.

I still paid for this year’s maintenance upgrade for Easy PC !

Parents

  • Hi Michael,

    I was going to point you toward my 50-minute quick-start video https://www.youtube.com/watch?v=5Be7XOMmPQE , but from that PCB screenshot is seems you don't need it. But maybe worth scanning bits of it (e.g. from the contents list there) in case there's anything you spot that you've not tried yet. It is for version 6 but the UI has not changed significantly in version 8. Version 8 has some extra features of course.

    Nice idea to make the board TO-3 shaped! I found KiCad to be a bit weak in the area of making curved board outlines (i.e. Edge.Cuts layer) like that, it is harder sometimes than it ought to be.

    Regarding the Board Setup, a neat thing is that now for all future projects, you can import the settings; there is a place to click that at the bottom of the Board Setup window.

    image

    Regarding grids, the single most useful thing is to go to Preferences->Preferences and under PCB Editor->Origins&Axes,ensure that the Display Origin is set to Drill/place file origin. I have no idea why it should ever be set to anything else, but I believe the default is something different.

    Once that preference is set up, each time I create a new board, what I do is go to Place->Drill/Place File Origin, and then click on (say) the bottom-left position of where I want my board corner, or, for symmetrical boards, I may click on the center of the board. It is effectively my "board origin". Now the X and Y co-ordinates displayed at the bottom of the screen will start from that origin point, and that's handy when positioning connectors etc., since I can precisely type the co-ordinates for them.

    The next very key thing is to go to Place->Grid Origin and then click on the same exact location where you put your Drill/Place File Origin. If you don't do that, then things get crazy when changing grids, because they won't align with your board origin (i.e. the Drill/Place File Origin).

    Now that that is sorted, when laying down copper using the X button, you can set the copper to snap to the grid at any angle, by going to Route->Interactive Router Settings and enabling Highlight collisions->Free angle mode.

    image

    It's a bit tedious, but if say you want the initial leg of copper to be at precisely 90 degrees (e.g. so it comes off an IC pad squarely) for a short distance, and then have the complete free angle, then the only method I know is to start off with the Free angle mode box unchecked in the Interactive Router Settings, and draw the first part of the trace, which will inevitably have the 90 degree line followed by a 45-degree line often. Once the mouse left-button has been clicked to place those two lines, then hit ESC twice to exit the trace drawing mode, and then click on the unwanted 45-degree like, press DEL to delete it, then, hover over the end of the 90-degree trace, press X again and hopefully it will connect to the end, and then right-click the mouse and in the pop-up menu, select Interactive Router Settings, and then enable Free angle mode. Now you can continue the trace, drawing at any angle.
    The 45-degree mode does have an advantage in that the 'Shove' mode can be selected in the Interactive Router Settings, which might be useful when trying to route wires close to each other. Personally I don't use the Shove mode often, but it's interesting to try it out in case the need arises.

    The many ground pins stacked on each other thing is really bizarre to me too. I don't use that technique in my own component symbols.

Comment

  • Hi Michael,

    I was going to point you toward my 50-minute quick-start video https://www.youtube.com/watch?v=5Be7XOMmPQE , but from that PCB screenshot is seems you don't need it. But maybe worth scanning bits of it (e.g. from the contents list there) in case there's anything you spot that you've not tried yet. It is for version 6 but the UI has not changed significantly in version 8. Version 8 has some extra features of course.

    Nice idea to make the board TO-3 shaped! I found KiCad to be a bit weak in the area of making curved board outlines (i.e. Edge.Cuts layer) like that, it is harder sometimes than it ought to be.

    Regarding the Board Setup, a neat thing is that now for all future projects, you can import the settings; there is a place to click that at the bottom of the Board Setup window.

    image

    Regarding grids, the single most useful thing is to go to Preferences->Preferences and under PCB Editor->Origins&Axes,ensure that the Display Origin is set to Drill/place file origin. I have no idea why it should ever be set to anything else, but I believe the default is something different.

    Once that preference is set up, each time I create a new board, what I do is go to Place->Drill/Place File Origin, and then click on (say) the bottom-left position of where I want my board corner, or, for symmetrical boards, I may click on the center of the board. It is effectively my "board origin". Now the X and Y co-ordinates displayed at the bottom of the screen will start from that origin point, and that's handy when positioning connectors etc., since I can precisely type the co-ordinates for them.

    The next very key thing is to go to Place->Grid Origin and then click on the same exact location where you put your Drill/Place File Origin. If you don't do that, then things get crazy when changing grids, because they won't align with your board origin (i.e. the Drill/Place File Origin).

    Now that that is sorted, when laying down copper using the X button, you can set the copper to snap to the grid at any angle, by going to Route->Interactive Router Settings and enabling Highlight collisions->Free angle mode.

    image

    It's a bit tedious, but if say you want the initial leg of copper to be at precisely 90 degrees (e.g. so it comes off an IC pad squarely) for a short distance, and then have the complete free angle, then the only method I know is to start off with the Free angle mode box unchecked in the Interactive Router Settings, and draw the first part of the trace, which will inevitably have the 90 degree line followed by a 45-degree line often. Once the mouse left-button has been clicked to place those two lines, then hit ESC twice to exit the trace drawing mode, and then click on the unwanted 45-degree like, press DEL to delete it, then, hover over the end of the 90-degree trace, press X again and hopefully it will connect to the end, and then right-click the mouse and in the pop-up menu, select Interactive Router Settings, and then enable Free angle mode. Now you can continue the trace, drawing at any angle.
    The 45-degree mode does have an advantage in that the 'Shove' mode can be selected in the Interactive Router Settings, which might be useful when trying to route wires close to each other. Personally I don't use the Shove mode often, but it's interesting to try it out in case the need arises.

    The many ground pins stacked on each other thing is really bizarre to me too. I don't use that technique in my own component symbols.

Children
  • in reply to shabaz

    Hello Shabaz,

    Thanks for the useful tips !

    I did the TO3 outline by drawing it in SolidWorks because the drawing tools in KicCad are very poor (or I didn't find the right ones).

    In SolidWorks you draw the 4 circles of the curves that make up the TO3 outline.

    Draw 4 lines more or less any where for the straight bits and set them to be tangential to the circles which make them ove to the right places.

    Then use the PowerTrim tool to get rid of the bits of line and curve you don't want.

    Then make it ito a drawing and print as a .dxf.

    KiCad can import a .dxf file to use as an edge cut.

    The only downside of this approach is the need for a SolidWorks license Slight frown

    MK