schematic components get a ~ in front of their names and behave strangely when their value-text is hidden

[Jan Krieger]

Take any component, e.g. TEST from device.lib. It's definition in the file looks like this:

#
# TEST
#
DEF TEST P 0 40 N N 1 F N
F0 "TP" 0 300 50 H V C BNN
F1 "TEST" 0 250 50 H V C CNN
F2 "" 0 0 50 H V C CNN
F3 "" 0 0 50 H V C CNN
DRAW
P 6 0 1 0 0 200 -50 150 0 100 50 150 0 200 0 200 N
X ~ 1 0 0 100 U 50 50 1 1 P
ENDDRAW
ENDDEF

and then hide its VALUE-field and save the lib in the symbol editr. The component becomes:

#
# TEST
#
DEF ~TEST TP 0 40 N N 1 F N
F0 "TP" 0 300 50 H V C BNN
F1 "TEST" 0 250 50 H I C CNN
F2 "" 0 0 50 H V C CNN
F3 "" 0 0 50 H V C CNN
DRAW
P 6 0 1 0 0 200 -50 150 0 100 50 150 0 200 0 200 N
X ~ 1 0 0 100 U 50 50 1 1 P
ENDDRAW
ENDDEF

Note that now we have "DEF ~TEST" instead of "DEF TEST" before.

Best,
JAN

[Wayne Stambaugh (stambaughw)]

Please paste the kicad version information into this bug report.

[jean-pierre charras (jp-charras)]

I never noticed that, but for some strange reason, this is the case for all version, including the 2013 stable version.
The strange reason could be a relic of very old code.

[Jon Evans (craftyjon)]

Seems to still be the case

Application: eeschema
Version: (2018-02-04 revision 141ef0c4b)-master, debug build
Libraries:
    wxWidgets 3.0.3
    libcurl/7.55.1 OpenSSL/1.0.2g zlib/1.2.11 libidn2/2.0.2 libpsl/0.18.0 (+libidn2/2.0.2) librtmp/2.3
Platform: Linux 4.13.0-31-generic x86_64, 64 bit, Little endian, wxGTK
Build Info:
    wxWidgets: 3.0.3 (wchar_t,wx containers,compatible with 2.8) GTK+ 2.24
    Boost: 1.62.0
    Curl: 7.55.1
    Compiler: GCC 7.2.0 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=OFF
    BUILD_GITHUB_PLUGIN=ON
    KICAD_USE_OCE=ON
    KICAD_SPICE=ON

[Wayne Stambaugh (stambaughw)]

This is by design but I'm not sure why. I don't see it being specifically used in the LIB_PART code. It may be a relic left over from older symbol library file formatting. Maybe JP can shed some light on

[jean-pierre charras (jp-charras)]

I am pretty sure this is a relic (and perhaps the relic of a relic).

[Wayne Stambaugh (stambaughw)]

@JP, judging from what I can tell, we can remove the write part of this. The read part will have to remain in order to read older schematics that used the ~ prefix to indicate the field was hidden.

[jean-pierre charras (jp-charras)]

Yes, we can remove the write part of this.
We also can remove the read part, because Eeschema does not actually take in account this visibility control (I tested that) because the F0 or F1 field definition overwrites it, and nobody has complained until now.
Moreover, the older Kicad version I have (2007) stores the visibility in F0 or F1 fields.

[Wayne Stambaugh (stambaughw)]

@JP, I will remove the write part. There is no harm in leaving the read part in there just in case there is some really old schematic version that requires it.

[KiCad Janitor (kicad-janitor)]

Fixed in revision ee14da3093858ab9eee1a17f02e1f3488b0c797c
https://git.launchpad.net/kicad/patch/?id=ee14da3093858ab9eee1a17f02e1f3488b0c797c