kicad-developers team mailing list archive

[Michael Kavanagh <michael@xxxxxxxxxxxxxxxxxx>]

I think there was a bug report filed for this:
https://bugs.launchpad.net/kicad/+bug/1827002

On Mon, 22 Jul 2019 at 20:59, Jeff Young <jeff@xxxxxxxxx> wrote:
>
> I was thinking all attributes would be user-defined, and you’d write rules to map to Kicad functionality.  Something like:
>
> virtual: ~BOM
> board-only: ~symbol
> logo: ~symbol, locked
>
> But maybe that’s over-the-top….
>
> > On 22 Jul 2019, at 13:23, Seth Hillbrand <seth@xxxxxxxxxxxxx> wrote:
> >
> > Hmm...  I was thinking that section would not have any reserved values with special meaning to KiCad.  That way users can add any data they want there and we don't have to check it for validity before allowing.  Is there any reason not to put the flag with the other component-specific flags?
> >
> > On 2019-07-22 15:10, Jeff Young wrote:
> >> I was thinking we’d handle it under:
> >> https://bugs.launchpad.net/kicad/+bug/980919
> >>> On 22 Jul 2019, at 12:53, Seth Hillbrand <seth@xxxxxxxxxxxxx> wrote:
> >>> Hi Jeff and JP-
> >>> Should we consider a new flag for board-only items?  These would be
> >>> items that exist on the board but not the schematic.  Would be
> >>> useful for NTPH mounting holes, logos, etc, that get added in pcbnew
> >>> and shouldn't be removed when updating, even if they are not locked.
> >>> This could help to separate the locked flag into flags that mean
> >>> "don't move without warning" and don't delete automatically (as part
> >>> of [1])
> >>> Best-
> >>> Seth
> >>> [1] https://bugs.launchpad.net/kicad/+bug/1745627
> >>> On 2019-07-22 10:27, Jeff Young wrote:
> >>> And just to add one more (which was the instance that prompted my
> >>> question):
> >>> Logos, certifications, etc.: symbol: no, footprint: yes, virtual:
> >>> yes.
> >>> But I see now that we can’t use virtual as a proxy for “don’t
> >>> treat as ‘extra’ when deleting extra footprints” because if
> >>> you
> >>> delete a symbol in one of the symbol:yes cases, then you _do_ want
> >>> the
> >>> footprint deleted.
> >>> Cheers,
> >>> Jeff.
> >>> On 22 Jul 2019, at 01:53, Dino Ghilardi <dino.ghilardi@xxxxxxxx>
> >>> wrote:
> >>> Just few examples (expanding jp's answer):
> >>> having a schematic symbol, being virtual, having 3d model are not
> >>> related (you can have any combination of them). As examples:
> >>> First: a virtual footprint that has a schematic symbol (the answer
> >>> to your main question).
> >>> Edge connector: schematic symbol: yes, footprint: yes, virtual: yes
> >>> (the connector is implemented only with tracks on  pcb, without the
> >>> need of additional components so no need to have it in the BOM).
> >>> "regular" component, as a Resistor 0805: has schematic symbol, Has a
> >>> footprint and we want it in BOM. (virtual: no.)
> >>> Hole without screw (yes, I'm copying jp's example): No schemaitc
> >>> symbol (or sometimes yes, depending on user's habits: someone likes
> >>> to have on schematics anything that will be on PCB, including
> >>> holes): Has a footprint but no items in BOM: (virtual: yes)
> >>> Hole with screw: Has a footprint but you want a corresponging item
> >>> in BOM to have the list of screws you need to buy (virtual: no).
> >>> P.S. (little bit off-topic):
> >>> Sometimes also virtual components can have 3d shapes (it is not
> >>> common but it is a way to quick-workaround a 3d view of a
> >>> more-than-one board assembly: export a step file of the board 1 and
> >>> assign that as a 3D shape to a connector or a mounting hole of board
> >>> 2. -very useful to check for mechanical collisions-).
> >>> Cheers,
> >>> Dino.
> >> ---------------------------------------------------------------------
> >>> On 22/07/19 09:02, jp charras wrote:
> >>> Le 22/07/2019 à 06:03, Jeff Young a écrit :
> >>> This flag tells us that there’s no physical object for a
> >>> pick-n-place machine.  But is it also true that there’s no
> >>> corresponding symbol in the schematic, or are there some virtual
> >>> footprints that would have a symbol?
> >>> What about some microwave elements, for instance?  Do they have
> >>> symbols?
> >>> "Virtual" footprint means the physical "component" is made only by
> >>> the
> >>> drawings on the board.
> >>> Therefore:
> >>> - These fp have (usually) no 3D shapes, and the component should be
> >>> not
> >>> in BOM.
> >>> - They of course have a symbol in schematic.
> >>> In fact any footprint connected to a at least one net *should* have
> >>> its
> >>> corresponding symbol in schematic.
> >>> (I am thinking all footprints should have a corresponding symbol
> >>> because
> >>> in many cases these fp need a unique refdes: for instance to import
> >>> them
> >>> to a .dsn file)
> >>> Microwave elements, and edge connector cards are often virtual, if
> >>> only
> >>> a drawing is enough to create them.
> >>> Net ties are virtual and *need* a symbol.
> >>> However, Microwave elements and Net ties connecting 2 or more
> >>> different
> >>> nets are not easy to use in Pcbnew:
> >>> See this thread
> >>> https://lists.launchpad.net/kicad-developers/msg24455.html
> >>> to know what is missing in Pcbnew (the Tomasz's proposal is exactly
> >>> what
> >>> is needed in Eeschema/Pcbnew).
> >>> Mechanical holes can be virtual or not:
> >>> A mechanical hole with a screw inserted inside it should be not
> >>> virtual.
> >>> _______________________________________________
> >>> Mailing list: https://launchpad.net/~kicad-developers
> >>> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> >>> Unsubscribe : https://launchpad.net/~kicad-developers
> >>> More help   : https://help.launchpad.net/ListHelp
> >>> _______________________________________________
> >>> Mailing list: https://launchpad.net/~kicad-developers
> >>> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> >>> Unsubscribe : https://launchpad.net/~kicad-developers
> >>> More help   : https://help.launchpad.net/ListHelp
>
>
> _______________________________________________
> Mailing list: https://launchpad.net/~kicad-developers
> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> Unsubscribe : https://launchpad.net/~kicad-developers
> More help   : https://help.launchpad.net/ListHelp