Automatic Neckdown

I typically try to make most traces 25 or 30 mil unless I need them smaller, because small traces can be fragile. (Feel free to debate this, I can probably tolerate 10 mil traces without any mechanical risk)
However, this becomes an issue when I want to route underneath surface-mount components.

Ideally, I want to neck down the trace width just for
I’ve found and lost a setting where a new track will use the specified track width rather than whatever that net is currently drawn with.
What would be better is to be able to specify a typical and minimum trace width for a net class, so the net would typically be at the typical width, but would neck down up to the minimum in order to route around obstacles.

Is there anything like this?

Just to say that I do similar, at least in one respect.

I try to make (we call them “tracks” in KiCad) much wider than much of what I see many others doing. I generally make them about the same width as the pad to which I am connecting, and I narrow it down when and where needed to save space. Typically my default resistor size is an 0603 chip which I will place on a small-ish 0805 footprint. That makes for relatively easy assembly by hand. I will connect to it with a 40 mil or 1 mm track. Advantages:

  1. Wider traces are more mechanically robust.
  2. At low voltages (under 30V; or maybe the limit is closer to 100V) inductance and mutual inductance is the most common parasitic element and method of stray coupling. Especially with a ground plane closely spaced under the signal layer, wider tracks will reduce these effects somewhat. Capacitance is increased but that seems to be less of an issue at low voltages than does inductance.

In my professional career spanning > 40 years I had one incident where a bad layout caused capacitive coupling which caused a problem with operation of a board. I had some analog circuitry controlling a thyristor controlled voltage regulator. Really…in that case the track was just in the wrong place.

But my track width setting process is almost all manual.

From the manual:

You will find Custom Rules in File > Board Setup > Design Rules. Use the “Syntax Help” to help you create a Custom Rule for Neckdowns. See here also for full explanation.

You can also set up all the track widths you require and scroll through them to change as required, with the W hotkey, or, backwards with Shift + W.

If you want an oddball size while you are placing tracks, you can use the Q hotkey.

Since 20+ years I use 10 mil tracks for signals and 40 mils for VCC (60, 80 mils if current higher than 100mA). Since may be 7 years I sometimes use 8 mils tracks.

I also see very little advantage of those very wide tracks. One exception is home etching or milling, where it parameters are more difficult to control.

For the vast majority of PCB’s made there would not even be room for such wide tracks. And even a 0.25mm (10mil) track can handle a few hundred mA (875mA with a 10 degree temperature rise according to KiCad’s calculator).

Mechanical stress is a serious consideration near high stress connectors (PC104 is a good example), and that is normally handled with teardrops. You can have a look at the Olinuxino A64 Rev-C (on github) as an example. It was made before KiCad had teardrop support, and it uses short wide tracks for the THT connectors, which are made thinner a few mm away from the connectors.

When working with bare PCB’s in your lab, it is common to add standoff’s though the mounting holes, which help both against mechanical damage and from shorts with random stuff lying on your desk. Another method I use is to push a PCB into thick corrugated cardboard, then take it out and make the holes a bit deeper (but not though it) by pushing on the cardboard with a pen or screwdriver (or whatever is available) , and then gluing the cardboard to the PCB. It is also easy to make “feet” on a PCB with blobs of hot glue (Let it cool and then put a 2nd blob on top to make the feet higher)

I suppose I’m satisfied with that.
I’ll quit bumping up the trace width unless I actually need it.


Learning how to, and setting up the design rules using the syntax is a bit of an effort. :slightly_smiling_face:

For simple stuff, not requiring too many neckdowns, I find making a list of track widths in Board setup > Design Rules > Predefined sizes easier.

The workflow is then:

  • W scroll through widths and observe sizes at top LH of screen.
  • X start track
  • Left mouse click to change widths
  • W scroll to new width
  • Continue drawing track without pushing buttons 'till next change required.
  • Left mouse click to change widths

Repeat as necessary.
If one width change is not quite in the correct position, return later and use the drag “D” function to adjust.

1 Like

I feel the need to disagree. This is an image of the top side copper of one of my most recent KiCad designs. The images show most of the board which is 100 x 37 mm. There are many tracks which are 0.5 and 1.0 mm width. Aside from the fact that it is a little more work, I do not see any reason to use a 0.25 mm track where a 0.5 mm track fits easily. Maybe some special circumstances such as controlled impedance?

and the bottom side copper:


Just wanted to add that Shift+W scroll backwards through available widths if needed :wink:

1 Like

You should create your own rules based on the general rules for designing printed circuit boards; this is the main mistake that occurs quite often… In production, usually the technologist does not pass the product for a number of reasons related to installation technology… Developers, in turn, not knowing these rules, do not allow the product to be assembled without marriage…

Not sure which rules you refer to specifically? Design rules must relate to manufacturability or performance of the end product. This board was fabbed by JLCPCB without issues. I assembled a couple of them without issues. And a couple of them were running in our garden last summer, powered by a battery and solar panel, without issues. (go to the end):,vid:w9KBOhPXhds,st:0

You can assemble it on wires or a breadboard and it will most likely work… General rules in this case are needed for a serial product where SMT installation technologies are used… There are many nuances and this is a large, comprehensive topic on many forum pages…

OK. But the topic at hand deals with using wide (such as 0.5 to 1.0 mm) tracks. I think nobody will argue against using wide tracks where they are required for current carrying or voltage drop or thermal reasons.
Really we are discussing wide tracks where there appears to be adequate space for them but they are not specifically required. So I think we can narrow our focus on that question.

Also to say that I have been electrical engineering for many years and have been responsible for pcb layouts since about 1978. I usually worked with a pcb designer when I was at my job. Anyway, this pcb for which I posted images is not my “first rodeo” but it is a home project.

Finally, one more item on the subject of wide tracks:,vid:3F1HHhJyDjg,st:0

the question is not whether the track is wide or narrow, but the way it is connected to the contact pad… I don’t know why my posts are being deleted and who I offended)

if you want to draw a wide trace to the component, then you need to make a narrowing or correct connection to the ground, otherwise it will not be possible to assemble it using SMT technology… there will be defects… this also applies to th installation depending on the class of the board and soldering technology. …

Hello @m852

You have no knowledge of the project.
You have no knowledge of any mechanical constraints
You have no knowledge of any electrical constraints
You have no knowledge of any components used
You have no knowledge if this is a final design
You have no knowledge of the assembly process envisaged
You have no knowledge of anything EXCEPT the picture demonstrates various width tracks attached to various pads, as the poster of the picture comments.

It is absolutely ridiculous to criticize a layout knowing so little information about it.

My gosh, a quick look at that tells me that this is baloney. See this:
image I use google to translate to English.
I see one recommendation for orienting similar components all the same way and on a grid. With all due respects, I have heard (and I agree) that this is the hallmark of someone who does not understand pcb layout.

While it might be the easiest for assembly, many designs simply would not work if laid out that way. Even the best schematic diagram design is garbage if the pcb layout is done without understanding layout priorities. My thing is high frequency power conversion, and that must be laid out for minimum stray inductance in critical paths. For many ICs, (power conversion or digital logic or audio or video or whatever) the bypass capacitor needs to be right at the power pin and tap into the ground plane. You do not place it somewhere near the IC in a grid arrangement.

SMT is a method of mounting electronic components, one of the most common in the microelectronics industry. It involves the use of special components that are soldered to the surface of a printed circuit board or other substrate without wires using reflow or immersion soldering.
I didn’t tell you anything about wiring or electromagnetic compatibility… If you read carefully, the general design rules are followed to meet the requirements of surface-mounting technology… If you solder at home with a soldering iron, a nail or a gas torch, then this is your personal business and has nothing to do with the technology …The question here is how you need it or how you want it…
The picture you didn’t like is a translation of an article (by David Marrakchi) published on the Altium website

I agree that this is just wrong. There was a time when keeping orientation constant really did help in production, but this is largely gone now. I design RF boards where the circuit determines the orientation, not the aesthetics of components in ranks

1 Like