The PCB editor just follows the netlist.
The cause is that you have shorted the +3V3 and the +3V3_MCU nets somewhere in the schematic. Also look at the pads of your ferrite bead. Both have the same +3V3 net name.
Such shorts can sometimes be difficult to find on the schematic. One common error is to draw a wire right through a schematic symbol, so the two pins get connected. Use the net highlight functionand ERC to find the fault in your schematic.
So both of them are the same “Base” net… the one for the mcu side is renamed - but i guess it wont rename the base net when doing so… Or it just doesnt make the distinction properly that it passes thru a component?!
So by changing the MCU base net to a +3.3V global label rather than the +3V3 it sorted it self… thanks 
I was wondering where the +3V3_MCU name comes from. It is not a standard name. In KiCad V7, power symbols are still a bit of a kludge. You can not just take a standard power symbol and change it’s name. For a Power symbol, the net name is derived from the pin (Which is hidden!) of the symbol, and not from it’s name.
If you want to modify a power symbol, you have to change both it’s name, and the pin name. And you can easily verify the new net by looking at the net name (for example on pads or on tracks in the PCB editor.
Yeah, that makes sense… Still learning this software.
The idea here was just to have the seperation between the more… noisy 3v bus and the one closest to the stuff that needs alot of emi filtering
Will look into howto make new power symbols for this project as there is several of these layers of same voltage but passing thru different filterings.
It’s very easy . . . if you already have a custom symbol library, just open an existing power symbol, do a Save As to save it to your custom library, modify it (change the name of the pin) and save it.
It’s a quite silly thing in KiCad. It would be a slight improvement if KiCad would just enforce the names of power symbols to be the same as the pin name. But the problem is already fixed in a better way in KiCad-nightly V7.99. In that upcoming version there are far less power symbols, but you can just directly change it in the schematic.
Ah noice… yeah it would also kinda make sense to be able to set the as input easily i have modified symbols on the fly to define where power in is instead of that power flag thing that just makes everything weird to read… ( imo ). Still great software, just had to mix it a bit with fusion to be able to define edgecuts properly - with dimensions 
But once i figured that out with importing DXF it was like the missing piece for me at least.
This is the only pitfall of KiCad that I also fell into when I started using it in 2017. Before using KiCad I have read all its pdfs but I didn’t read about it or simply forget it.
Mechanical CAD is a whole new subject in itself. KiCad is not good at it, and it also does not pretend to be either. You can easily draw a rectangular PCB, make some cutouts and add mounting holes within KiCad, but when outlines become complicated, DXF import is the way to go. And this is not unique to KiCad either. Having DXF (or other common 2D CAD) import is mandatory for any “decent” PCB design software, and once you have that, there is very little incentive to add complicated mechanical CAD functions too.
I came from Altium and that behaves alot different - but costs a arm, leg, first born child maybe several sacrificed goats… So Kicad does a good job imo.
Agreed - but some basic 2D cad is not that hard to implement, you need proper “dimensions” and a way of cutting existing lines so you can do some circles, boxes, squares and then just “scissor” out the rest… But agreed, dxf files is the way togo… And works flawlessly.
Yes, KiCad has all those.
It does? i only found a way of measuring a line not setting its “length”
Nor have i found a line scissor… care to screenshot?
I was using Protel 3 for years and was used to just put power symbol and change its name.
Yes, that is what a proper dimension does.
I guess you mean parametric drawing capabilities here, and KiCad does not have those. Such things are also not very easy to implement.
You can right click on a line and select Create Corner from the popup menu, or use the **[Ins]**ert key while a graphic line is selected. Note that the popup menu also has a function for “Fillet Lines” which makes it easy to add rounded corners to your PCB.
KiCad’s drawing abilities are limited, but what it has is quite functional.
altium is also not very good for drawing complex shapes … it’s elementary to indicate the already drawn holes for fasteners, you have to select each one and tell him that these are the contours of the cicada holes in this case it understands everything at once without unnecessary movements … in this regard, I like qcad everything is fast and just
For what it’s worth, in 7.99 (future v8.0) it’s possible to set a line’s length in the properties.
In general, there are some tricks in KiCad to make drawing easier. For example, you can press Spacebar to set the “local origin” which you can see in the bottom of the screen. The you will see dx and dy from that point. Set the origin to one end of a line and drag the other end – you can see the length as “dist” interactively. Pressing Shift+Spacebar may be helpful to switch between n*45 degree and free angle drawing. Snapping related settings and tricks are important to learn, so is using the grid for your advantage. There are also several ways to move items a certain distance or relative to something or to some point. These can help you a long way forward.
On the other hand, when it goes complex, you should learn to draw with some more complex drawing tool. Paul mentioned “parametric” drawing, and FreeCAD/StepUp can export sketches to KiCad. A sketch can be “fully constrained” with different kinds of parameters, including lengths, angles, distances etc.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
