Tracks won't draw at net class widths?

I have set up the track width in Board Setup | Design Rules | Net Classes:

If I now route a track belonging to "Vei_IP+ it is drawn with the default (0.2mm) width.
If I now Edit | Edit Track and Via Properties | Set the Action to Net Class Values, the track is redrawn with the correct (1.0mm) width. But no matter what I try, I can’t get the track to start with the required width?

What do I need to do?

Regards, M.

Notice the text in the status bar, (from existing track)? The button next to the track width dropdown overrides the width from the track dropdown.

Click the button to change it.

Easy when you know how :grinning:
Thanks a lot.


Ask me how I know! :slight_smile:

Okay… How do you know :grin:
And. It isn’t so straight forward. Been playing and it still does not make sense!

If I start a track from an existing track (Veh_IP+ lower right) it works.
But if I try to start a track from a pad (Pin 10, Vei_IP-) it is 0.2mm.
Also, it correctly, will not connect to P7,6,5, Vei_IP+). But it will connect to the Zone connected to Vei_IP+.

Your netname Vei_IP+ belongs to a differential pair (all nets with “+” “-” “P” or “N” as last character define a diff-pair net). Looking at your first picture (board setup–>netclass parameters) the width for all diff-pair netclasses is set to 0,2mm (column DP_Width).

Wow. That’s a new one on me! Thanks again.

Hover your Mouse/Cursor over the item @baldengineer showed and Read it…

the key word is “…from…”

Finish routing track and press ‘b’ to rebuild zones and then check if your track is still connected to that zone.

while we’e at it , @mprowe the hole to hole spacing in your screenshot might not be able to be fabricated.
It’s a good idea to look up your proposed PCB fab capabilities, but do not use those without qualification. Like, they all say “oh we can do 22 layers sure”. Some board houses will specify two values - preferred and capability if they really try hard. You want to stick with ‘preferred/easy’.
PCB Manufacturing & Assembly Capabilities - JLCPCB that URL is their maximum capability !
"Hole to hole clearance(Same nets) 0.254mm
But that’s hard for drills above 0.5mm…and thick laminates, you might limit yourself to 50% higher, or 2 x higher depending on the drill size.

1 Like

Why would that be crasy?
Alignment can be an issue in between various stages of the production, but all the drilling is done in a singly cycle, and things like misalignment of the panel in the drilling machine or deformation of the PCB during pressing will not have any effect on the relative locations of drilled holes.

Myabe I will use a different choice of word. I have edited it.
That would be hard.
It depends on the size of the drills, and how much drill wander can be tolerated . Larger drills, less tolerance for wander with low hole to hole clearance.

anyway getting off topic, sorry

I think source of problems is not the relative locations but forces acting on the drill when there is a thin wall on one side that does not provide the same resistance as on other sides. Try to do with a thin drill such close holes yourself - you should notice the problem.

1 Like

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