Manual annotation causes Netlist to miss connections on schematic

[David Pearce]

Seen on Ubuntu and Windows Nightlies

I have created a simple three level hierarchical schematic.
All four parts are in block2a

F1 was a polarised fuse.
I annotated, ran netlist, opened in pcb new and saw all parts and nets as expected.
Then I deleted F1 and replaced it with a new F1, different symbol but same footprint.

Pcbnew now shows the F1 pads as unconnected and I see that the nets are not connected to F1, although the schematic does connect.

Application: kicad
Version: no-vcs-found-8f3423b~58~ubuntu16.04.1, release build
Libraries: wxWidgets 3.0.2
           libcurl/7.47.0 OpenSSL/1.0.2g zlib/1.2.8 libidn/1.32 librtmp/2.3
Platform: Linux 4.4.0-70-generic x86_64, 64 bit, Little endian, wxGTK
- Build Info -
wxWidgets: 3.0.2 (wchar_t,wx containers,compatible with 2.8)
Boost: 1.58.0
Curl: 7.47.0
KiCad - Compiler: GCC 5.4.0 with C++ ABI 1009
        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

[Jakob Möderl (jmoederl-deactivatedaccount)]

seems to work in my version.

when i opened the project the connection was missing (the connection is missing in the netlist) but when i changed the symbol back again to a polarized fuse (same value and footprint) and update the PCB the connection reapears.

Application: kicad
Version: (2017-03-05 revision 541b91fd1)-master, release build
Libraries: wxWidgets 3.0.2
           libcurl/7.53.1 OpenSSL/1.0.2k zlib/1.2.11 libpsl/0.17.0 (+libicu/58.2) libssh2/1.8.0
Platform: Linux 4.10.6-1-ARCH x86_64, 64 bit, Little endian, wxGTK
- Build Info -
wxWidgets: 3.0.2 (wchar_t,wx containers,compatible with 2.8)
Boost: 1.63.0
Curl: 7.53.1
KiCad - Compiler: GCC 6.3.1 with C++ ABI 1010
        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=OFF

[Wayne Stambaugh (stambaughw)]

@David, what grid spacing are you using? The components and wires do
not appear to be on a 50mil grid which can cause connection issues if
you are not careful. You should always use 50mil grid spacing when
placing components, wires, and labels to avoid connection issues.

On 3/29/2017 11:19 AM, David Pearce wrote:
> Public bug reported:
>
> Seen on Ubuntu and Windows Nightlies
>
> I have created a simple three level hierarchical schematic.
> All four parts are in block2a
>
> F1 was a polarised fuse.
> I annotated, ran netlist, opened in pcb new and saw all parts and nets as expected.
> Then I deleted F1 and replaced it with a new F1, different symbol but same footprint.
>
> Pcbnew now shows the F1 pads as unconnected and I see that the nets are
> not connected to F1, although the schematic does connect.
>
> Application: kicad
> Version: no-vcs-found-8f3423b~58~ubuntu16.04.1, release build
> Libraries: wxWidgets 3.0.2
> libcurl/7.47.0 OpenSSL/1.0.2g zlib/1.2.8 libidn/1.32 librtmp/2.3
> Platform: Linux 4.4.0-70-generic x86_64, 64 bit, Little endian, wxGTK
> - Build Info -
> wxWidgets: 3.0.2 (wchar_t,wx containers,compatible with 2.8)
> Boost: 1.58.0
> Curl: 7.47.0
> KiCad - Compiler: GCC 5.4.0 with C++ ABI 1009
> 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
>
> ** Affects: kicad
> Importance: Undecided
> Status: New
>
> ** Attachment added: "zip file of simple example project"
> https://bugs.launchpad.net/bugs/1677282/+attachment/4849811/+files/recoverybug.zip
>

[David Pearce (halzia)]

Good point about the grid, but I have been carefully looking for the boxes on wire ends and dragging to check connection.
Anyway I have re-gridded from 10 to 50 mil and ERC finds an unconnected pin on J1 pin 2, although I cannot see why.
I think this is the root cause.
Updated project attached

[David Pearce (halzia)]

I can reproduce the error on a single sheet schematic.
Examining the schematic file does not show anything off grid

Steps
Create simple circuit
Run ERC - All OK
Substitute part by:
 Add new component
 Delete old component
 Connect new component in place of old component
 Manually edit Ref to previous reference
Run ERC - Not connected
Run Netlist - no warnings but result is wrong
Run Annotate (No obvious effect)
Run ERC - Now everything is connected
Run Netlist - Now correct

[David Pearce (halzia)]

Looking at the schematic file I see that Annotate silently changes a "0" to a "1" on two lines
$Comp
L C C1 (Component is a "C", reference "C1")
U 0 1 58DC707A ---> U 1 1 58DC707A
P 6600 3700
F 0 "C1" H 6715 3746 50 0000 L CNN
F 1 "100n" H 6715 3655 50 0000 L CNN
F 2 "" H 6638 3550 50 0001 C CNN
F 3 "" H 6600 3700 50 0001 C CNN
0 6600 3700 ----> 1 6600 3700 (the coordinate of the centre of the substituted part)
1 0 0 -1

[David Pearce (halzia)]

I changed the bug title to be more accurate.
My finding is that adding a component symbol and setting the reference manually using "U" or simply editing the reference on screen, causes the schematic file to have set N in the line:

U N mm timestamp to "0", where N is the unit number.

This causes the Netlist generator and ERC to ignore the part and not connect it
Running automatic annotation then sets the unit number to a "1" and the Netlist can be generated correctly.
I have tested 4.0.6 and the "U" command behaves as expected, generating a "1" (or higher for multi-units) immediately, resulting in a correct netlist.

[KiCad Janitor (kicad-janitor)]

Fixed in revision 40f60c9871949935f2b4f2f856b04234b2ae3440
https://git.launchpad.net/kicad/patch/?id=40f60c9871949935f2b4f2f856b04234b2ae3440

[Wayne Stambaugh (stambaughw)]

@David, thank you for the help in finding this bug. It should be fixed in commit 40f60c987. You will get a warning dialog when unit specifier in the loaded schematic file is 0 and fixed automatically by the file parser. Please let me know if this doesn't solve your issue.

[David Pearce (halzia)]

Thanks, I will test it soon, I am travelling this weekend.
I looked at your patch and was concerned about blindly forcing a detected Unit N = 0 to a "1", but tested a swapping a 7400 Unit B to a 7402 Unit B and the U command does correctly write a "2".
This means the manual annotation bug seems to only affect single unit parts, all the basic R and C etc

[Wayne Stambaugh (stambaughw)]

It was not the manual annotation that caused the issue. It's actually
the placement of the component from the new component chooser dialog
that was incorrectly setting the unit to 0 on components without
multiple units. Apparently the automatic annotation was fixing this by
setting the unit to 1.

On 3/30/2017 7:48 PM, David Pearce wrote:
> Thanks, I will test it soon, I am travelling this weekend.
> I looked at your patch and was concerned about blindly forcing a detected Unit N = 0 to a "1", but tested a swapping a 7400 Unit B to a 7402 Unit B and the U command does correctly write a "2".
> This means the manual annotation bug seems to only affect single unit parts, all the basic R and C etc
>

[David Pearce (halzia)]

Ok, tested working correctly now.
Is the root cause chooser unit error also being fixed?

[Wayne Stambaugh (stambaughw)]

Yes, the component chooser was fixed.

On 4/2/2017 9:25 PM, David Pearce wrote:
> Ok, tested working correctly now.
> Is the root cause chooser unit error also being fixed?
>

[David Pearce (halzia)]

Thanks.
Also, I find the warning about the schematic file being corrected to prevent compatibility problems perfectly clear