Sure. Nothing wrong with going under a chip.
I have never encountered a situation where it was unacceptable to run a trace under an IC package. (Assuming, of course, that the trace satisfied the requirements for minimum width and spacing.) However, in some organizations the “house rules” prohibit routing traces under common passive components in leadless packages (e.g., resistors and capacitors in 0805, 0603, and similar packages). The justification is that the trace, with its covering of soldermask, is thick enough to lift the body of the component off the board, create a “teeter-totter” effect, and reduce soldering yield.
Dale
1 Like
Great. That means I can use single-sided board.
Thanks to all who have assisted.
My next step, according to Getting started in KiCad is to create a Ground Plane which will be connected to all GND points. There are only two GND points (U1/78 and LED/1) in this circuit
and they are already connected
Is, in this situation, such a Ground Plane necessary?
(If this sounds like a stupid question, remember that I am only a dumbo Mechanical Engineer 
)
No, a ground plane is probably not necessary for your circuit. Even circuits where a ground plane is not essential for proper operation may benefit from a ground plane, and almost any circuit which incorporates a “clock” signal (which includes ALL microcontroller circuits) will have better EMI performance if it includes an effective ground plane.
Keep in mind that you are working through a tutorial exercise. Like any textbook, the examples are often contrived to support the lesson. The goal of this exercise is to demonstrate how some tasks common to circuit board design can be performed in KiCAD. The tutorial does not pretend to teach either circuit theory or product design.
Dale
1 Like
That’s what I figured. Thanks Dale
If possible, I would like to include a ‘logo’ on my board. I have had a look at stuff from Google and have got as far as creating a kicad_mod file which I think will do the job. At present, that file is in my project folder. Question is, what are the steps to get the logo.kicad_mod inserted into the kicad-pcb image?
Passing under IC has nothing to beeing able to use single-sided board. Just use only bottom and not top layer and you need not to pass under IC.
Alternatively plot non-mirrored image, transfer and etch on single-side board, then mount widgets through from non-copper side.
Create a subdirectory of your project directory. You can name it anything, but it has to end in .pretty. I often name it myLibrary.pretty. Move the .kicad_mod file into this directory.
In PCBNew, from the “Preferences” menu, choose “Footprint Libraries Manager”. Then add ${KIPRJMOD}/myLibrary.pretty to the “Project Specific Libraries” tab, like this:
Next, click the “Add footprints” button, which looks like this:
Now click where you want the logo to go. The “Load Footprint” dialog will appear. You can click “List All”, and then choose your logo from the list.
1 Like
Every manufacturing process has a minimum trace width.
If you want to etch at home with minimum tools your minimum tracewidht is probably pretty wide.
Therefore I recommend to make all your traces at least 2x the width they are now.
And put those decoupling & bulk capacitors in.
If they are not in the tutorial, then the tutorial is wrong (for designing a working board).
The tutorial is clearly meant only for having something to do while explaining KiCad.
In the real world these capacators are mandatory. Even much more important than the GND plane.
About Logos:
Somewhere in KiCads foot print library there are some nice “made with KiCad” logo’s.
I think that sums it up.
Thanks very much. I appreciate the work that went into your reply.
Two more things which haven’t worked so far.
- When I plot the board the outer, rectangular, border does not appear. I did intent to use that border as a guide to calculating the size correction scale. How do I get that to print?
- The little circles in the corners were intended to show the location of hold-down screw holes. No luck with them either. How do I indicate where screw holes should go?
Thanks
There is a library called “Mounting_Holes” with footprints for different sized holes.
You can draw the holes on your schematic and then assign footprints, or you can add the footprints to PCBnew as separate compoments.
In the second case you should fix or lock their positon to prevent them from being removed when a new netlist is being imported.
And still:
Put those caps in.
It will give you some practice in modifying schematics and updating the PCB with your revised design.
Especially when edging your own board. As then you typically do not have the luxury of plated through holes.
Would work but that is a dirty bodge. It should not take you too long to remake these few connections on the bottom side.
There is one situation I can think of, if you are using photo-couplers (opto isolators) for isolation tracks under the IC can compromise the isolation clearances.
1 Like
That is correct! I forgot about that one; it’s been over 10 years since I used an optocoupler where that degree of isolation was required.
The requirements can get even more severe than simply traces under the IC body. Sometimes an optoisolator comes in a package which is the size of a 6- or 8-pin DIP, but only the end pairs of pins are present. The center section of the package, where you would expect to find a pair (or two pairs) of pins is empty, to increase the physical isolation distance between conductors. That wide open space is begging to have traces run through it but it’s really a no-man’s land.
And for the most extreme isolation requirements you may be required to cut out a section of the PC board itself under the IC body, so that leakage currents can not flow across the surface of the PCB. At this time, you can not create a footprint of this style in KiCAD, because the Edge.Cuts layer (where the cutout must be placed) is not accessible from the footprint editor. Perhaps this case is adequate justification for removing that limitation . . .
Dale
You tend to remember mistakes…
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.