Hi all,
some time ago, I used the nightly build r7176.679eef1 to create a project.
Now, I updated to 4.0.6.
If I want to start PCBnew I get an error message that I should update to a newer version (newer than 08-15-16)…
I thought 4.0.6 is the newest version?!
What’s going wrong? How to avoid to start from scratch?
Thanks for any suggestions.
Nighties are not backwards compatible to the 4.0.x series. Opening the project in a more recent Nightly and saving might solve it as the incompatible extension is only used when needed now.
1 Like
Thank you @davidsrsb for your quick reply.
I reinstalled the nightly build and I’m happy that at least I can open it again. Is there maybe also another way to make it compatible with 4.0.6 without stepping into another nightly adventure?
If you know what new features you have used, then you could find them and make them compatible. If you don’t, it could be along exercise with no guarantee of success.
The nightly builds operate like a ratchet. Once you have moved forward, it can be very hard to go backwards.
2 Likes
Differential pair gap parameter was the main backwards compatibility breaker
1 Like
There could also be problems regarding the lib (symbol libs are up do date in nightly, 4.0.6 libs are quite old now. => missing symbols)
There might also be problems with rounded rectangle pads, …
The error message might help to find what the problem is. @theozh could you post the specific error message you get?
Symbols should be ok so long as the cache file is available
Yes, rounded rectangles are not supported in 4.0.x
We really need 5.0.0
As far as i understand it the symbol table stuff is the reason for the current delay. (I think wayne wants it included in v5.)
I’m looking forward to 5.0.0 as well! It looks like there are some nice new features 
Sadly, my release date estimate continues to slip, maybe Q1 2018.
Thank you all…
@Rene_Poschl, that’s what I get.
That’s info about my nightly build:
Application: kicad
Version: (2016-09-17 revision 679eef1)-makepkg, release build
Libraries: wxWidgets 3.0.2
libcurl/7.46.0 OpenSSL/1.0.2d zlib/1.2.8 libidn/1.32 libssh2/1.6.0 librtmp/2.3
Platform: Windows 7 (build 7601, Service Pack 1), 64-bit edition, 64 bit, Little endian, wxMSW
- Build Info -
wxWidgets: 3.0.2 (wchar_t,wx containers,compatible with 2.8)
Boost: 1.57.0
Curl: 7.46.0
KiCad - Compiler: GCC 5.2.0 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
BUILD_GITHUB_PLUGIN=ON
KICAD_USE_SCH_IO_MANAGER=ON
KICAD_USE_OCE=ON
That’s info about the Version 4.0.6 where I tried to open the file:
Version: 4.0.6, release build
wxWidgets 3.0.2 Unicode and Boost 1.60.0
Platform: Windows 7 (build 7601, Service Pack 1), 64-bit edition, 64 bit
That’s the error message I get:
Error loading board
KiCad was unable to open this file, as it was created with a more recent version than the one you are running. To open it, you'll need to upgrade KiCad to a more recent version.
Date of KiCad version required (or newer): 08/15/16
Full error text:
PARSE_ERROR: Expecting 'clearance, trace_width, via_dia, via_drill, uvia_dia, uvia_drill, or add_net' in input/source
'D:\Data\KiCAD\xxx\xxx.kicad_pcb'
line 114
offset 6
from
C:/Jenkins/workspace/windows-kicad-msys2-stable/src/kicad/common/dsnlexer.cpp: Expecting(): line 369
This doesn’t tell me much…
The board is nothing really complicated. If I remember correctly, the main reason to use the nightly build was the ability to use .step files.
If you change the header of the kicad_pcb file with a text editor to
(kicad_pcb (version 4) (host pcbnew 4.0.6)
that will remove the version warning. I think the other message is to do differential pair settings, you will need to remove those too.
2 Likes
thank you @bobc,
changing the header line and deleting the two following lines seemed to help.
(diff_pair_gap 0.25)
(diff_pair_width 0.2)
At least now I can open the file in 4.0.6. Maybe there will be some more “surprises” later?
Thanks a lot!
1 Like