Crosstalk prevention?

Hi folks. To reduce crosstalk on my board I need certain tracks to mostly have wide clearance. However, the track going close to pads or even close to other tracks for short distance is OK. It shouldn’t run close to another track for a long distance.
If I set net classes and clearances, the rules apply to the whole track, I cannot even connect it to a chip pad because the pads are closer to each other than the desired clearance.
Basically what would be enough is a design rule checker which would check if certain tracks run too close to others for more than N mm.
Are there any solution for that?

I think that the nightly development version 5.99 has a rules base DRC feature which would address this.

There’s no way to do it as a length using rules. But you could set it up with the wider clearance and then override that (using a rule area) for specific regions of the board.

(You will find tokens in the DRC rules language for specifying the min, opt, max, and uncoupled for diff-pairs, but it didn’t make it in to 6.0.)

1 Like

Very important is the layer stackup. For a given spacing between traces, best is to have the tracks on an internal layer with ground planes spaced with the thinnest possible dielectric above and below. Less good is (for example) traces on the top layer of a 4 layer board with ground plane spaced as close underneath. Next step down is traces on top of a 2 layer board with ground plane 1.6 mm away on the bottom. And worst would be no ground all…

I am looking for a reference on this…

Thanks Jeff. Rule area is a new feature of 6.0?
I ended up manually checking all crosstalk-relevant traces.

You could also place a ground track between the signal tracks, this should AFAIK also lower cross talk, if both ends are connected to the ground plane (keeping one end floated may increase or decrease cross talk).

Effectively. Custom DRC rules are new in 6.0, and one way to apply them is to a user-defined area. These used to be called “Keepout Zones” but now they’re called “Rule Areas”.


There is a workaround, using which you can implement net ties to assign varying tolerances to different parts of the same track. You can use a combination of two circular pads and one rectangular polygon pour to form a part of a track with different tolerances. This should be set as a Net tie.

Currently, you have seemed to have issues with the track as it approaches pads of different sizes and clearances, as shown in the image below:

To solve it you will need to use a net tie.

Step 1: Select a Net tie from the symbol library in Schematic mode

Step 2: Create the footprint for the Net tie

Step 3: Assign the footprint

Step 4: Design the net tie using two pads and a polygon pour

Step 5: Update the footprint library

This is not true, other than that putting a ground track between will keep them further apart.

it does work. it is standard practice to put a guard 0V. It’s not as good as full track separation (taking into consideration the track width vs the stackup…) but sometimes if you cannot achieve correct spacing it’s a viable option.

1 Like

Did you even read your reference? Many of their conclusions support my position. For example:

  1. In all high speed digital applications, where –50 dB cross talk is acceptable, there
    is never a need to implement a guard trace. This cross talk can be achieved in
    stripline traces by just increasing the spacing between aggressor and victim to fit a
    guard trace.
  2. In microstrip, if a guard trace is used with the ends terminated open or shorted,
    the noise on the victim line can be higher than if the guard trace were not present.
  3. A guard trace, even “well shorted”, has minimal advantage. To fit the required
    shorting vias means spacing the aggressor and victim lines very far apart which
    by itself reduces the cross talk more.

I did read it thank you, guard traces do work. It doesn’t mean it is the best solution or only solution but they do work

This is false. A GND track between 2 signal tracks can reduce noise if the GND track is properly connected to the GND plane compared to 2 signals with the same space in between and no GND track or a floating track between them.

This does not mean that this is always a good solution. For example it may increase capacity or change impedance of the signal tracks in a bad way.

Your link does not compare to simply separating the traces, only different grounding configurations of the “guard” trace.

Do you agree that connecting floating track, between the signal tracks, to GND in a proper way reduces crosstalk compared to the floating track?
Do you think that bit of floating track makes the crosstalk significantly worse than compared to no copper in between?
Do you think this floating track makes crosstalk so much worse that the benefit of connecting it to GND is canceled out?

Do you have any measurements that support your claim that putting a properly connected GND track in between does not reduce crosstalk?

Read the reference 4 posts up.

I’ll quote some relevant sections from the conclusions:

  1. A guard trace, even “well shorted”, has minimal advantage. To fit the required
    shorting vias means spacing the aggressor and victim lines very far apart which
    by itself reduces the cross talk more.
  2. Using a guard trace with microstrip offers high risk of incorrect termination with
    little potential reward and should never be done. Rather sensitive lines should be
    buried in stripline

How are this quotes relevant for your claims or my claims?

You said it is not true that placing a ground track between the signal tracks reduces crosstalk. We weren’t talking about how much the cross talk is reduced. I wouldn’t disagree with you when your claim would be something like “The benefit of a ground track in between is minimal and not worth it”.

I’m not interested in arguing over infinitesimals.

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