I’m having an issue I can’t seem to solve. Under Board Setup -Constraints, I’ve set the minimum clearance to something obvious like 2 mm, expecting that the router would prevent me from placing tracks closer than that. However, when I use the interactive routing tool, it completely ignores the rule, I can route tracks as close together as I want.
I do see a light gray visual guide indicating what 2 mm spacing would look like, but it doesn’t restrict routing any closer than that. I was under the impression that the clearance setting would be enforced automatically to help maintain spacing.
In the Interactive Router settings, I have selected Walkaround mode. I also updated the default Net Class to set the clearance to 2 mm, but the behaviour hasn’t changed.
Am I missing something, or is this expected behaviour?
Additionally, when I use the Selection tool to manually move tracks closer together, there are no restrictions or even visual guidelines to indicate a clearance violation. This makes it difficult to consistently maintain the required spacing.
Both. You’re missing something, and it is expected behavior.
The settings in the Board Setup are not intended for “actual use” but only to set limits for which DRC will complain if they get exceeded. They are supposed to match (with some generosity tolerance) what your PCB manufacturer can make.
For normal track width and clearance settings there are two options. The most flexible is to work with net classes, and you can work with “pre-defined sizes”. I suggest you start with learning more about the net classes, you can find more info in the manual.
Yeah, I even tried assigning the net properly using net classes, but it’s still completely ignoring my clearance settings. I just can’t figure out why. The track width works though. It shouldn’t be possible to route that close to another track. I can even route across other tracks on the same layer, which really shouldn’t be allowed. I’m wondering what setting I might have enabled that’s allowing this to happen?
the GPIO 7 on the right was just for testing purpose to see what happens if I go across other tracks
Check Route > Interactive Router Settings. You may be in Highlight mode, rather than Shove or Walk around Mode.
Shove and Walk will follow the min. cu to cu board clearance unless a larger Netclass track clearance is used.
Indeed. PCB Editor / Route / Interactive Router Settings / Mode / Highlight Collisions is probably set. This is also the only mode that allows all angle tracks with [v] Free angle mode. Setting the interactive router to Shove is the most common mode for routing tracks.
But also:
Clearance is only enforced between tracks from different nets, and not between tracks from the same net. So there is no clearance between the two shown sections of the 3.3V PWR net.
Yea, it was set to Walkaround Mode. But I think I found the issue, there was something under “custom rules”. I was loading a file to get the right settings for pcbway, but it was writing data into custom rules, which seems to overwrite everything.
Thank so much for your help though
