Dragging Trace Problem - Page 1
Forum section: electronics / general

author: PixieDust
author_rank: Frequent Contributor
timestamp: August 12, 2019, 12:03:30 pm
content: 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

author: thinkfat
author_rank: Unknown
timestamp: August 12, 2019, 12:51:18 pm
content: 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.

author: PixieDust
author_rank: Frequent Contributor
timestamp: August 13, 2019, 09:00:51 am
content: I haven't touched design rules. HmmI deleted the PCB layout file and started again and ran into the same problem, same pin is the problem!(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.

author: JackJones
author_rank: Regular Contributor
timestamp: August 13, 2019, 09:28:52 am
content: 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?

author: PixieDust
author_rank: Frequent Contributor
timestamp: August 13, 2019, 09:32:07 am
content: Quote from: JackJones on August 13, 2019, 09:28:52 amThat worked! Thanks. That was the next thing I wanted to try. You beat me to it.

author: grbk
author_rank: Contributor
timestamp: August 13, 2019, 02:16:31 pm
content: 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).

author: bson
author_rank: Unknown
timestamp: August 17, 2019, 03:39:56 pm
content: 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!

author: thinkfat
author_rank: Unknown
timestamp: August 18, 2019, 12:54:16 pm
content: Wow. That doesn't sound very useful, does it? I think I never had the situation where my pads were strictly grid-aligned.

author: Rerouter
author_rank: Super Contributor
timestamp: August 18, 2019, 01:05:46 pm
content: 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.

author: pierreraymondrondelle
author_rank: Contributor
timestamp: August 19, 2019, 09:48:21 am
content: Quote from: thinkfat on August 18, 2019, 12:54:16 pmit does ! most of modern chips are following metric units. RIP to medieval ones !regards

author: sethhillbrand
author_rank: Newbie
timestamp: September 07, 2019, 08:30:02 pm
content: Quote from: Rerouter on August 18, 2019, 01:05:46 pmAs 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.