DRC check errors

[Derhaegr]

Hi all,

I have a few weird DRC errors that i don’t understand:

The first one says the track is unconnected and you still see this tiny line:
Picture one

I also have 3 that do not show a line but are connected too.
Why does it say this?

The second error is related to a power plane i did:
Picture2
Is says pads not connected as you can see, and is says copper in copper, this is not part of the gnd plane on the layer, but does not show seperation, maybe i did it wrong.

[dchisholm]

@Derhaegr

The first one says the track is unconnected and you still see this tiny line:Picture one

I also have 3 that do not show a line but are connected too.Why does it say this? [/quote]
It looks like the trace does not intersect the center of the pad. Go to the “Render” tab (far right side of the screen) and un-check “Pads Front” and “Pads Back”. You will probably see that the trace enters the pad, then makes a squiggle and does not cover the actual center of the pad.

[quote] The second error is related to a power plane i did:Picture2Is says pads not connected as you can see, and is says copper in copper,

This one might be a simple case of copper-to-copper clearance, or it may be more difficult. Sometimes DRC errors like this mention one cause, but the real problem is something else.

First, add explicit traces connecting all of the pads that are part of the (C66-Pad1) net. I think DRC may get confused when too many pads are connected only by a copper-fill zone.

Then verify that the clearance specified in the design rules for the nets connected to that device (is it Q31?) are compatible with the pad-to-pad spacing. For example, if the gap between those pads is only 0.15mm, then you cannot have a design rule calling for 0.2mm copper-to-copper clearance.

Finally make sure that your schematic has electrical connections to ALL of the pads in that package. Using “hidden pins” on the schematic symbol can cause trouble.

Let us know if none of these suggestions fix the problem.

Dale

[PCB_Wiz]

@Derhaegr

The first one says the track is unconnected and you still see this tiny line:Picture one

KiCad needs only that the trace-end is inside the PAD outline to register connected.
What you have there, is most likely a short bonus trace inside the pad.
These can happen when modifying and moving things, and can be hidden by the filled pad.

You can turn on Pad outlines only, to better see the traces, or just click on the top right rats-nest end, and you should be given a choice of Pad or a short Trace. Select Trace, then delete.

@Derhaegr

The second error is related to a power plane i did:Picture2Is says pads not connected as you can see, and is says copper in copper, this is not part of the gnd plane on the layer, but does not show seperation, maybe i did it wrong.

KiCad pour has some issues around Thermal Connect, and there are some geometries where thermal connect does not register.
Unlike traces, which require just a trace-end inside a Pad to connect, Pour requires the centre of the pad is included, but pour ‘pulls back’ by clearance which can result in what looks ok, not registering as connected.
See also other threads on this, and I have registered a bug report on this effect.
Ideally, Pour outline should use the Pad outline to confirm connects, just like Traces do.
That may have a small speed penalty, but connect seems plenty fast enough now.

Choices to fix/avoid are to

• Move the pour outline, or
• Adjust the pour clearance (helps in finer pin pitch designs)
• Add a trace segment from pad to at least inside the copper pour result.

Many designers choose to fully route the GND tracks, at some default width, and use Pour only for added-copper.
This can also connect in channels where the pour clearance does not place copper, and is safer in that a shift of a via or other trace, cannot accidentally cause a pour island effect. DRC should report that, but not everyone carefully checks all DRC messages

[Derhaegr]

I did have a gnd island that i fixed by moving some tracks to another layer, all other errors are fixed except the Q31 the pads are indeed < 0.2 and that trickers the DRC now. thanks for explaining.