A couple of examples of extra clearance options requested https://bugs.launchpad.net/kicad/+bug/1510742
And the following one really bugs me for high power igbt drivers https://bugs.launchpad.net/kicad/+bug/983230 This board would benefit from this. https://endless-sphere.com/forums/viewtopic.php?f=30&t=84930 I've seen the same request in the forum as well. Cheers On Jul 26, 2017 17:01, "Wayne Stambaugh" <[email protected]> wrote: > On 7/26/2017 9:47 AM, hauptmech wrote: > > This is a nice concept. A more generic constraint system. > > > > What I'll be doing and was asking if there was others needing, is the > > pre-net-class approach of a single clearance that is easily adjusted > > while laying tracks. > > What you want is a change to the router to allow you do this not change > the actual netclass. Changing the netclass in the middle of a route if > fraught with peril. If you start out with a netclass with a larger > clearance and then change to a netclass with a smaller clearance, the > DRC will fail every time. I suppose you could add a context menu action > to allow you to increase the route clearance specified by the current > netclass (along with trace width, via, via drill etc as long as the > project minimums are not violated). Allowing the user to decrease the > clearance would result in a DRC violation. > > > > > I think this used to be there. Having it would not affect netclass > > behaviour or drc behaviour, but would allow manual control of clearance > > for the situations where useful. > > > > On 27/07/17 01:17, Maciej Sumiński wrote: > >> Hi hauptmech, > >> > >> I am sure there are many users who would benefit from the suggested DRC > >> improvements, so I would say it is an interesting idea. There is a plan > >> to upgrade it, but I am afraid you will have you board finished before > >> this happens. > >> > >> It is not entirely clear to me what do you propose. At the moment there > >> is an option to set clearance per net class, so I assume you want to be > >> able to set clearance per [net class,layer] pair. How do you want to > >> modify the user interface (Design Rules Editor dialog)? > >> > >> I am not sure how much time are you willing to spend on this, but if I > >> were to implement such feature, then I would: > >> - in the "Net Classes Editor" remove the grid widget where you specify > >> the constraints (clearance, track width, etc.) > >> - add a new tab "Constraints" with a list widget and two buttons: "Add" > >> and "Remove" > >> - the "Add" button invokes a dialog where you can specify the target for > >> the rule (Net/Net Class/Layer) and the type of constraint you want to > >> apply (clearance, track width, etc). For each category used to specify > >> the target (Net/Net Class/Layer) one selects 'Any' or a concrete value. > >> > >> This way the design rules definition become very flexible as you may > >> easily specify exact targets. In case there is more than one rule for an > >> item, the strictest one applies. For items that do not trigger any of > >> the rules, the global design rules are used. > >> > >> To give an rule set example with your case: > >> - global design rules: whatever your PCB house is able to manufacture > >> - inner layers, any net: 0.1 mm width > >> - outer layers, any net: 0.3 mm width > >> > >> Regards, > >> Orson > >> > >> On 07/26/2017 10:05 AM, hauptmech wrote: > >>> I have nets that have different clearance requirements depending on > >>> where they are. There are two situations that are in my designs: > >>> > >>> 1) Technical/Manufacturing limitations: Trace and space limitations > >>> depend on layer copper thickness and whether it's an inner layer or > >>> outer layer. For instance, my current project has 0.1mm trace and space > >>> and a 15um thick copper layer on one pair of inner layers. Outer layers > >>> are 30um and use 0.125mm minimum trace and space because 0.1 can't be > >>> done at that copper thickness. > >>> > >>> 2) Designers preference: I like to move to larger traces and spaces > when > >>> the component spacing allows. Apart from a mild optimization on current > >>> carrying capacity and capacitive coupling, there is not a big technical > >>> reason; it's just the way I like to do things. > >>> > >>> Both of these things have me manually changing the default netclass > >>> clearance constantly, and when I forget to change it back to the larger > >>> trace and space I have to redo chunks of layout. Happens more often > that > >>> I'd like to admit. A sign of aging I guess. > >>> > >>> Running the DRC I first do a pass at the lowest clearance, and then > >>> (doing this now) run the same DRC on a larger clearance and check each > >>> error to see if it's real (many are) or allowed for the layer and > >>> location manually. > >>> > >>> There's a lot of ways to approach this issue and a 'good' way to do > this > >>> has not occured to me yet. Meanwhile I have work to do. I'm seeing a > big > >>> chunk of work in 2013 by Dick on the netclass and vaguely remember > >>> clearance being as settable as trace width once upon a time. > >>> > >>> Pulling forward the old clearance setting widgets and possibly allow > >>> specifying layers for the DRC are what I'm looking at doing in my > >>> personal branch. Probably add a 'netclass' default entry in the > >>> clearance dropdown I am remembering > >>> > >>> All this to ask, does anyone else have issues with the netclass > approach > >>> to clearance and would the mainline want an integration of both > netclass > >>> and manually set clearances? > >>> > >>> -hauptmech > >>> > >>> > >>> > >>> _______________________________________________ > >>> Mailing list: https://launchpad.net/~kicad-developers > >>> Post to : [email protected] > >>> Unsubscribe : https://launchpad.net/~kicad-developers > >>> More help : https://help.launchpad.net/ListHelp > >> > >> > >> > >> _______________________________________________ > >> Mailing list: https://launchpad.net/~kicad-developers > >> Post to : [email protected] > >> Unsubscribe : https://launchpad.net/~kicad-developers > >> More help : https://help.launchpad.net/ListHelp > > > > > > > > > > _______________________________________________ > > Mailing list: https://launchpad.net/~kicad-developers > > Post to : [email protected] > > Unsubscribe : https://launchpad.net/~kicad-developers > > More help : https://help.launchpad.net/ListHelp > > > > _______________________________________________ > Mailing list: https://launchpad.net/~kicad-developers > Post to : [email protected] > Unsubscribe : https://launchpad.net/~kicad-developers > More help : https://help.launchpad.net/ListHelp >
_______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : [email protected] Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
