KiCad

pcbnew, netlist import throws around components

Bug #1795561 reported by Nicholas Savenlid on 2018-10-02

This bug affects 1 person

Affects		Status	Importance	Assigned to	Milestone
	KiCad	Fix Released	Undecided	Jeff Young

Bug Description

When importing a new netlist where some components have been changed, the position of those components are wasted.

I will strongly suggest you keep the position, rotation and side of any refdes that is already in the design even if the part-no has changed.

This problem of resetting position causes a lot of work and time.

Sometimes you need to replace a component because it goes end of life for example.
Size and everything is the same, and even if it was not it will most likely be in its original position nonetheless.

Thanks
/Nicholas

Application: kicad
Version: (6.0.0-rc1-dev-652-gf06bf8165), release build
Libraries:
    wxWidgets 3.0.3
    libcurl/7.54.1 OpenSSL/1.0.2l zlib/1.2.11 libssh2/1.8.0 nghttp2/1.23.1 librtmp/2.3
Platform: Windows 7 (build 7601, Service Pack 1), 64-bit edition, 64 bit, Little endian, wxMSW
Build Info:
    wxWidgets: 3.0.3 (wchar_t,wx containers,compatible with 2.8)
    Boost: 1.60.0
    OpenCASCADE Community Edition: 6.8.0
    Curl: 7.54.1
    Compiler: GCC 7.1.0 with C++ ABI 1011

Build settings:
    USE_WX_GRAPHICS_CONTEXT=OFF
    USE_WX_OVERLAY=OFF
    KICAD_SCRIPTING=ON
    KICAD_SCRIPTING_MODULES=ON
    KICAD_SCRIPTING_WXPYTHON=ON
    KICAD_SCRIPTING_ACTION_MENU=ON
    BUILD_GITHUB_PLUGIN=ON
    KICAD_USE_OCE=ON
    KICAD_USE_OCC=OFF
    KICAD_SPICE=ON

Revision history for this message

Jeff Young (jeyjey) wrote on 2018-10-02:

@Nicholas, are you sure it's not keeping the position? Some parts can have their anchors in different locations, which will make the rest of the part move. But there's not much we can do about that.

If you're seeing movements that aren't explained by that, can you attach a simple project that exhibits it?

Revision history for this message

Nick Østergaard (nickoe) wrote on 2018-10-02:

Please state exactly what import options you are using.

Changed in kicad:
status:	New → Incomplete

Revision history for this message

Nicholas Savenlid (nicholas-z) wrote on 2018-10-02:

Bug30.png Edit (94.1 KiB, image/png)

I attach here a picture of my import settings.

Lately it always jumps around.

Example:
1 resistor in schematic is exchanged for another resistor.
Unique parts.
Same footprint.
Refdes not changed. (new part is hand-edited to same refdes as old part)

replaced/changed part is placed outside PCB.

Revision history for this message

Nicholas Savenlid (nicholas-z) wrote on 2018-10-02:

Ps
Anchors same, as its the exact same footprint used by different parts/symbols.
Ds

Revision history for this message

Nicholas Savenlid (nicholas-z) wrote on 2018-10-02:

More exactly:
Part do not end up outside PCB.
They get imported as new, and are pre-selected and moved around by cursor movements.
Organised in a squared pattern with spacing in-between X and Y

Revision history for this message

Nick Østergaard (nickoe) wrote on 2018-10-02:

Yeah, so the bug is more clearly stated as the updated footprints being grabbed by the cursor when it is expected to update inplace. Right?

Changed in kicad:
status:	Incomplete → New

Revision history for this message

Nicholas Savenlid (nicholas-z) wrote on 2018-10-02:

Even if you escape out from the grabbing (escape-button) they wont drop down into "old" places.

They will just get dropped onto the pcb in an array pattern.

Revision history for this message

Jeff Young (jeyjey) wrote on 2018-10-02:

Hi Nicholas,

By setting "Keep existing footprint associations" you're telling Kicad that any symbol that wasn't associated with a footprint is "new", and it's footprint should therefore be "new".

If you want to update in-place based on RefDes, then set the "Re-associate footprints by reference" radio button. This tells Kicad that you want any footprint which matches the RefDes of a symbol to be associated with that symbol (which will update in-place).

Changed in kicad:
status:	New → Invalid

Revision history for this message

jean-pierre charras (jp-charras) wrote on 2018-10-02:

Hi Jeff,

I reopen the bug because:
"Re-associate footprints by reference"
is really broken (when "Update Footprints" option is on) when importing a netlist by "Load Netlist..." tool.
It fully breaks the association.

However, it works when using "Update PCB from schematic".

Changed in kicad:
status:	Invalid → New

Revision history for this message

Jeff Young (jeyjey) wrote on 2018-10-02:

#10

I thought I already fixed this (CmpNoCase() does not return a boolean for match; it returns 0 if they're equal), but I can't find any evidence of it).

Revision history for this message

Jeff Young (jeyjey) wrote on 2018-10-02:

#11

Well, that should have been obvious. We have duplicated code and I only fixed it on the Update-PCB-from-Schematic side. (And there's another bug I only fixed on the other side.)

Revision history for this message

KiCad Janitor (kicad-janitor) wrote on 2018-10-02:

#12

Fixed in revision 536451138dd931e019ee47bff7cc1e301f83293d
https://git.launchpad.net/kicad/patch/?id=536451138dd931e019ee47bff7cc1e301f83293d