Author Topic: Dragging Trace Problem  (Read 685 times)

0 Members and 1 Guest are viewing this topic.

Offline PixieDust

  • Regular Contributor
  • *
  • Posts: 82
  • Country: au
Dragging Trace Problem
« on: August 12, 2019, 12:03:30 pm »
Hi,

I'm doing a simple breakout board and I'm having a problem routing my traces. It doesn't allow me to connect the pads. Not sure what might be causing this. Yesterday before I messed around the mechanical outline all the pads connected just fine.

https://vimeo.com/user101749571/review/353345696/13d981ceef
 

Offline thinkfat

  • Supporter
  • ****
  • Posts: 203
  • Country: de
    • Matthias' Hackerstübchen
Re: Dragging Trace Problem
« Reply #1 on: August 12, 2019, 12:51:18 pm »
That's indeed a bit weird. How do your design rules look like? Any particular classes set up? I've seen stuff like that when I set up the track/track clearance too small for the pitch of the footprint.
 

Offline PixieDust

  • Regular Contributor
  • *
  • Posts: 82
  • Country: au
Re: Dragging Trace Problem
« Reply #2 on: August 13, 2019, 09:00:51 am »
I haven't touched design rules. Hmm

I deleted the PCB layout file and started again and ran into the same problem, same pin is the problem! :palm: (Also looks like the second last pin doesn't want to connect either).

If I try to route other nets and come close to these two pins, they also standoff around the same distance as when I'm trying to route the correct net.
« Last Edit: August 13, 2019, 09:31:07 am by PixieDust »
 

Offline JackJones

  • Regular Contributor
  • *
  • Posts: 132
  • Country: fi
Re: Dragging Trace Problem
« Reply #3 on: August 13, 2019, 09:28:52 am »
What happens if you delete the edge cuts near the pin? I didn't see anything immediately obvious in the video, but I did notice that the outline is curved near the pin that is giving trouble. Maybe there is some conflict there?
 
The following users thanked this post: PixieDust

Offline PixieDust

  • Regular Contributor
  • *
  • Posts: 82
  • Country: au
Re: Dragging Trace Problem
« Reply #4 on: August 13, 2019, 09:32:07 am »
What happens if you delete the edge cuts near the pin? I didn't see anything immediately obvious in the video, but I did notice that the outline is curved near the pin that is giving trouble. Maybe there is some conflict there?

That worked! Thanks. That was the next thing I wanted to try. You beat me to it :box:.
 

Offline grbk

  • Contributor
  • Posts: 40
  • Country: us
Re: Dragging Trace Problem
« Reply #5 on: August 13, 2019, 02:16:31 pm »
I can't see the video but this sounds a lot like a known bug in 5.1.2 where traces explode near curved edge cuts. The workaround is to temporarily delete the curved edge (or move it from the edge cuts layer to a non-fab layer).

It's fixed in 5.1.4, which should be out in the next day or two (although depending on your OS it could be longer).
 

Offline bson

  • Supporter
  • ****
  • Posts: 1545
  • Country: us
Re: Dragging Trace Problem
« Reply #6 on: August 17, 2019, 03:39:56 pm »
Another thing that can cause failure to connect tracks to pads is if you turn off snapping in the pcbnew preferences.  If pads and tracks aren't perfectly aligned to the grid you won't be able to connect them without snapping enabled.  Guess how I know! :palm:
 

Offline thinkfat

  • Supporter
  • ****
  • Posts: 203
  • Country: de
    • Matthias' Hackerstübchen
Re: Dragging Trace Problem
« Reply #7 on: August 18, 2019, 12:54:16 pm »
Wow. That doesn't sound very useful, does it? I think I never had the situation where my pads were strictly grid-aligned.
 

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 4293
  • Country: au
  • Question Everything... Except This Statement
Re: Dragging Trace Problem
« Reply #8 on: August 18, 2019, 01:05:46 pm »
Now that the edge cut fixed you issue, I should clarify, kicad checks if a pad is connected by looking that the center point of the pad (offset pads move this point) overlaps a trace, not the entire pad geometery just yet, so as long as the trace touches that center point it will register as a connected trace.

 

Offline pierreraymondrondelle

  • Contributor
  • Posts: 8
  • Country: fr
Re: Dragging Trace Problem
« Reply #9 on: August 19, 2019, 09:48:21 am »
Wow. That doesn't sound very useful, does it?

it does ! most of modern chips are following metric units. RIP to medieval ones !
regards
 

Offline sethhillbrand

  • Contributor
  • Posts: 8
  • Country: us
Re: Dragging Trace Problem
« Reply #10 on: September 07, 2019, 08:30:02 pm »
Now that the edge cut fixed you issue, I should clarify, kicad checks if a pad is connected by looking that the center point of the pad (offset pads move this point) overlaps a trace, not the entire pad geometery just yet, so as long as the trace touches that center point it will register as a connected trace.

As a quick note, this is no longer the case for KiCad version 5.1.0 and higher.  All traces that end within the pad geometry are considered connected.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf