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
