Two tracks - same signal - different widths

Layout
1

Hi,
How can two tracks of different widths be connected (same signal) ?
I thought that a net tie was the way to do it, however DRC throws:

Error: Clearance violation (zone clearance 0.5000 mm; actual 0.0000 mm)
Polygon on F.Cu
[Zone/Power_uP/VinTPSM365] on F.Cu

Here is the NetTie from the standard library:

Screenshot 2023-10-03 at 21.30.10
Screenshot 2023-10-03 at 21.30.10576×541 25.8 KB

Thanks

2

Similar error: Net Tie Fails DRC - Errors Not Itemized in DRC Dialog

You don’t need a net tie to used different widths per se, but only if you want have different default widths and it’s inconvenient to manually keep two widths in one net. From your text and screenshot I can’t tell if you already know this.

EDIT: here, too: DRC violations / Clearance violation on Bridged Links to filled planes. Maybe this is a bug.

3

I did search in the forum before posting, but did not find the two mentioned posts.
Happy not doing anything wrong, I will ignore these errors.
Thanks for your prompt answers.

4

Same signal means for me same net.
I frequently change track width (‘w’ and Shift+w hotkeys allow to select next/previous width from defined for this PCB set of widths to be used). For example when I have with VCC track that I normally use 1mm width to go under 0603 after clicking before 0603 and then using hotkey Shift+w I select 0.4mm width then on the other side of 0603 using hotkey ‘w’ I get back to 1mm.

5

This is much simpler than NetTies !

6

Besides that: You know that you can choose to ignore DRC violations?

7

As I ‘since always = long before using KiCad’ use many widths at one net I don’t feel what in your opinion is inconvenient in it.
Example 1:
VCC at 2 layer PCB where you don’t have a separate layer for it.
I typically use 1mm, but…

  • if I have to go under TQFP through its corner there I use 0.7mm as I had there no place for 1mm.
  • if I have to route it for longer distance I prefer to use 2mm just to have lover voltage drop,
  • if I have to connect to VCC pull-up 10k resistor I connect it with 0.25mm track. That allows to easily go with such connection under some other 0603 elements,
  • if I have a serie of 8 inputs, each with pull-up and serie resistor I place all these 16 resistors in one row and go with VCC under all of them using the widest track that I have a place for it under 0603 (it will typically be 0.4mm). This allows to jump over VCC with all these inputs,

Example 2.
I prefer to use 0.25mm tracks for signals. If I have element with 0.4mm raster I route each its signals with 0.2mm until the place I can spread them a little. Then I change each of them to 0.25mm for farther go.

Example 3.
If I connect signal track (0.25mm) to 2mm raster pin header I use short 0.5mm width traces just near that pins.

8

As Piotr already wrote, there are plenty of reasons for using different track widths for the same net. Another one is for example connecting some pullup resistors to a power net.

I find that the simplest way to do this, is to first draw at least one track segment, Edit it properties to enter some other width, and then continue drawing it. Depending on KiCad’s configuration, it will continue with the same track width.

9

It is not “Another” :slight_smile: It was on my list.

I use ‘w’ and ‘Shift+w’ hotkeys to select on the go one of predefined track widths.
In Pre-defined Sizes I typically have tracks: 0.2, 0.25, 0.4, 0.5, 0.7, 1, 1.3, 2.

10

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