Can't connect pads & wires of the same type

I cannot seem to be able to wire up this atmega328p (see image)
It also seems to be the case for most pads on this footprint.

Thanks to anyone that can help!

This is also my first time on this forum so I am unaware if this turns out to be a common problem but I have done some research on it and nothing showed up.

I’m also unsure as to which forum topic this would belong.

Kicad version: 5.0.1
Windows 10
Footprint (atmega 328p) : Housings_DFN_QFN:QFN-28-1EP_4x4mm_Pitch0.4mm

This is a problem with tolerances. Those red lines? Those indicate a tolerance envelope. Note how you can draw your trace right up to where it is about to touch them? I’m not sure if these are from the footprint or the general design rules without looking. When I run into these kinds of things I know enough to stumble my way through but never remember which menu.

Bottom line, you need to lessen the clearance distances. A lot of defaults in Kicad are know for being overly generous in terms of ‘safe’ settings.

2 Likes

Found it! here’s a screenshot:

Thanks for the fast response!

1 Like

You changed clearance to 0.1mm. If you don’t use the minimum width given by your board manufacturer I suggest using 0.16 or 0.18mm instead. Most manufacturers can do 0.16 with their economy price but 0.10 can cost much more or even be impossible. And actually you can keep 0.20 in the shown table and change the clearance of the footprint from the footprint properties.

2 Likes

That particular footprint has exactly 0.200000mm clearance between pads. Consequently, the original example posted by @william2 may, or may not, pass DRC. (It depends on whether DRC tests for the condition of “greater than” versus “greater than or equal to”.) At the very least, the track he’s trying to place must be perfectly aligned with the pad before KiCAD will permit it - there’s no place for even half a pixel of misalignment.

@william2 may have been successful at placing his trace if he started it on Pad 4 of the QFN footprint rather than on the decoupling capacitor. A trick I have used when I know there is (just barely) enough clearance for a trace, is to first place a narrower trace, verify that the trace is positioned at exactly the position it needs to be, then increase the trace width.

Dale

1 Like

I’m not sure how it is now, but with 4.0.7 I have done some tests and if I have footprint pads so defined that distance betwean them was 0,6mm then when clearence was defined to be 0,2mm and track width to 0,2mm I was not able to go with that track betwean that pads. My decision was that when I will be using KiCad (I plan to do it shortly) I will use my clearences set to numbers like 0,199 or 0,249 instead of 0,2 or 0,25. But before I will do it I will check once more how it works in V5.

1 Like

Sometimes that works well. I have noticed that sometimes DRC seems to act randomly, some of the items with apparently same values in the same board are caught and some not.

It might also be that the active grid doesn’t let put the track through. I think this can happen if the centerline of the pad isn’t on a grid point. Changing the grid pitch to a small value temporarily may help.

The more comprehensive, philosophical, point is that it takes special skill and attention to work at the very edge of what is possible. Life is generally easier if you leave a little margin around everything you do. That is one foundation beneath the concept of “sabbath” described in the sacred writings of the Hebrews and Christians.

Dale

Right, but it is good to knew the edge of what is possible.
The example (0.6mm, 0.2mm) I gave here was simplified. The truth reason I have checked what is possible was as follows.
My designs are 2 layer PCB with one layer being 100% GND. Because of it I spend relatively much time in placement thinking all the time of which way each wire will go. Because of it I like to switch off GND connections during placement (probably will be possible in V6). I generally use 10mils and sometimes 8 mils tracks and clearances (in KiCad I plan to replace it with 0.25mm and 0.2mm).
When I have installed 4.0.7 I found that KiCad defines completelly different 0603 footprints for resistors and for capacitors (I have never think before of haveing more than one 0603 footprint). It is not true for V5. I noticed that R_0603 has a distance betwean pads of exactly 1mm. Thow I thought I can put two 0.2mm tracks with 0.2mm clearance under 0603 resistor. That would be very helpfull for my 2 layer PCBs. So I have checked it and it was not possible until I changed the clearance to 0.199 or 0.1999 (don’t remember). It was certainly not a problem of tracks put at grid. If it would be the source of problem than changing clearance of 0.0001mm would not help if I used grid of 0.1 or 0.05mm.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.