kicad-developers team mailing list archive

[Wayne Stambaugh <stambaughw@xxxxxxxxx>]

Does this patch override the users configuration or does it just solve
the default configuration issue on windows and osx?  If so, that's not a
good thing.  I'm fine if respects the users config.  I still stand by my
original investigation that this is a package configuration issue, not a
broken code issue but if no one is willing to resolve those issues and
your patch respects the user config, then I'm OK with it.

On 10/13/2016 9:49 AM, Maciej Sumiński wrote:
> Finally, I could get back to the issue. If we really focus about the
> consequences, the real problem is not that spinit is not processed, but
> the codemodel libraries are not loaded.
> 
> Looking at the default spinit file:
> - most of the lines are comments
> - one causes problems ('set interactive', has to be unset later)
> - three others have no special meaning in shared library mode (aliases
> and 'set x11lineararcs')
> - the only meaningful lines are the ones that load codemodel libraries
> 
> To fix the problem, there is a patch which:
> - Allows ngspice to load the default spinit/.spiceinit files (no changes
> here).
> 
> - Looks for codemodel files in a few paths relative to eeschema
> executable. If a valid path is found, then an ngspice variable __CMPATH
> is set.
> 
> - After the default initialization, looks for spiceinit (note it is
> spiceinit not .spiceinit) file in a few paths relative to eeschema
> executable. If one is found, then it is executed. If we decide to
> provide our spiceinit file (see the attachment), then thanks to __CMPATH
> variable we can point to the right codemodel directory.
> 
> - If no spiceinit was found, but we know the correct path to codemodels,
> then they are simply loaded.
> 
> - Unsets a few variables which may cause simulator hangups.
> 
> Once the patch is committed, codemodels should work out of the box for
> the common msys2 builds and nightly Windows installers, even without a
> custom spiceinit. If OSX bundles provide codemodel libraries, then there
> is a chance it will work for them as well, otherwise we can add another
> search path.
> 
> I know it may look like an ugly hack, but sincerely I have no better
> idea at the moment. I am going to leave it here for comments for a few
> days, if there are no objections, I will commit the changes.
> 
> Regards,
> Orson
> 
> On 10/06/2016 05:53 PM, Wayne Stambaugh wrote:
>> I have some additional information that may prove useful:
>>
>> 1) Using relative paths in the spinit file does not work on windows.
>>
>> 2) Placing a spinit file in the path where the ngspice and libngspice
>> binaries reside works with no need to set any environment variables.
>>
>> Option 2 could be used by the installer.  The installer itself would
>> have to create the spinit file by substituting the install path for the
>> path of the .cm files.  I'm not sure if this would work on osx.  Maybe
>> one of our osx devs could test this.  If it does, than that would
>> resolve the simulation init issues.
>>
>> I've attached a simple circuit that demonstrates the issue.  When the
>> .cm files are not located, the simulation will run with the following
>> warnings and cause the output of the op-amp to be an impossibly high 260V:
>>
>> Error on line 0 :
>> a$poly$e.xu1.eos %vd [ xu1.53 xu1.98 ] %vd ( xu1.3 net-_u1-pad1_ )
>> a$poly$e.xu1.eos
>> MIF-ERROR - unable to find definition of model a$poly$e.xu1.eos
>> Warning: Model issue on line 0 :
>> .model a$poly$e.xu1.eos spice2poly coef = [ 1.7e-3 1 ] ...
>> Unknown model type spice2poly - ignored
>> Error on line 0 :
>> a$poly$e.xu1.eref1 %vd [ vdd 0 0 0 ] %vd ( xu1.98 0 ) a$poly$e.xu1.eref1
>> MIF-ERROR - unable to find definition of model a$poly$e.xu1.eref1
>> Warning: Model issue on line 0 :
>> .model a$poly$e.xu1.eref1 spice2poly coef = [ 0 0.5 0.5 ] ...
>> Unknown model type spice2poly - ignored
>> Error on line 0 :
>> a$poly$e.xu1.eref2 %vd [ net-_u1-pad1_ 0 /out 0 ] %vd ( xu1.97 0 )
>> a$poly$e.xu1.eref2
>> MIF-ERROR - unable to find definition of model a$poly$e.xu1.eref2
>> Warning: Model issue on line 0 :
>> .model a$poly$e.xu1.eref2 spice2poly coef = [ 0 0.5 0.5 ] ...
>> Unknown model type spice2poly - ignored
>> Error on line 0 :
>> a$poly$e.xu1.eo3 %vd [ xu1.98 xu1.30 ] %vd ( vdd xu1.42 ) a$poly$e.xu1.eo3
>> MIF-ERROR - unable to find definition of model a$poly$e.xu1.eo3
>> Warning: Model issue on line 0 :
>> .model a$poly$e.xu1.eo3 spice2poly coef = [ 0.7175 0.5 ] ...
>> Unknown model type spice2poly - ignored
>> Error on line 0 :
>> a$poly$e.xu1.eo4 %vd [ xu1.30 xu1.98 ] %vd ( xu1.44 0 ) a$poly$e.xu1.eo4
>> MIF-ERROR - unable to find definition of model a$poly$e.xu1.eo4
>> Warning: Model issue on line 0 :
>> .model a$poly$e.xu1.eo4 spice2poly coef = [ 0.7355 0.5 ] ...
>> Unknown model type spice2poly - ignored
>> Reducing trtol to 1 for xspice 'A' devices
>> Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
>> Warning: vv3: no DC value, transient time 0 value used
>>
>> Let me know if you have any other questions or comments.
>>
>> Cheers,
>>
>> Wayne
>>
>> On 10/6/2016 10:56 AM, Nick Østergaard wrote:
>>> Hi Maciej
>>>
>>> In the latest nightlies they are now stored in lib/ngspice/
>>>
>>> I guess that should equate to a relative path to the executables to
>>> ../lib/ngspice/*.cm, given that the exe's are in the bin folder on the
>>> same level as lib.
>>>
>>> So feel free to submit your fix. Also, are there any demos that make
>>> use of those cm libs such that it can be tested?
>>>
>>> Nick
>>>
>>> 2016-10-05 23:16 GMT+02:00 Maciej Sumiński <maciej.suminski@xxxxxxx>:
>>>> Hi Nick,
>>>>
>>>> Are the .cm files included in the Windows nightlies installer? If so,
>>>> could you tell me what is the relative path to the directory storing
>>>> them? The easiest way to fix the problem is to send a few commands to
>>>> ngspice before a simulation starts.
>>>>
>>>> Regards,
>>>> Orson
>>>>
>>>> On 10/05/2016 10:23 PM, Nick Østergaard wrote:
>>>>> Is this really needed?  What exactly does the .cm files provide?
>>>>>
>>>>> When I run the latest nightly I can run the allen key demo without
>>>>> problems as far as I can see.  Maybe some other simulation modes do
>>>>> not work properly?
>>>>>
>>>>> 2016-09-30 14:37 GMT+02:00 Wayne Stambaugh <stambaughw@xxxxxxxxx>:
>>>>>> That would work as a long term solution as well.  I was trying to at
>>>>>> least prove that it can be done without make changes to the current
>>>>>> code.   Until a full solution is implemented, users (me) will have an
>>>>>> interim solution if they want to use the spice simulator.
>>>>>>
>>>>>> Cheers,
>>>>>>
>>>>>> Wayne
>>>>>>
>>>>>> On 9/30/2016 3:40 AM, Maciej Sumiński wrote:
>>>>>>> We have also discussed on IRC another possibility, which is loading the
>>>>>>> extensions manually instead of having ngspice process its initialization
>>>>>>> file (spinit). This way we can adjust the paths during runtime.
>>>>>>>
>>>>>>> Regards,
>>>>>>> Orson
>>>>>>>
>>>>>>> On 09/29/2016 08:51 PM, Wayne Stambaugh wrote:
>>>>>>>> After much cursing and many config attempts, I finally have a working
>>>>>>>> spice simulation solution on windows.  I'm guessing similar parallels
>>>>>>>> can be applied to osx as well.
>>>>>>>>
>>>>>>>>
>>>>>>>> Option A: running from a mingw32 or mingw64 terminal.
>>>>>>>>
>>>>>>>> 1) copy the installed spinit file (by default will be in
>>>>>>>> ${MINGW-PACKAGE-PREFIX}/share/ngspice/scripts) to ~/.spiceinit.
>>>>>>>> 2) change the msys2 paths (/mingw##) in ~/.spiceinit to absolute windows
>>>>>>>> paths with / not \ (in my case C:/msys64/mingw##).
>>>>>>>> 3) Launch kicad.exe from the terminal.
>>>>>>>>
>>>>>>>> I realize this is not very elegant and will only work with either the 64
>>>>>>>> or 32 bit mingw (not both without editing .spiceinit) but it works and
>>>>>>>> is handy for mingw users.
>>>>>>>>
>>>>>>>>
>>>>>>>> Option B: configuring windows and run kicad from a shortcut.
>>>>>>>>
>>>>>>>> 1) locate the installed spinit file
>>>>>>>> ($INSTALL_PATH/share/ngspice/scripts) and change the msys2 paths
>>>>>>>> (/mingw##) to absolute windows paths with / not \ (in my case
>>>>>>>> C:/msys64/mingw##).
>>>>>>>> 2) Run kicad, open the config paths dialog, and add an environment
>>>>>>>> variable SPICE_LIB_DIR with path to the spinit file minus the last
>>>>>>>> "scripts" path ($INSTALL_PATH/share/ngspice).
>>>>>>>>
>>>>>>>> I also tried copying the .spiceinit file from option A to %USERPROFILE%
>>>>>>>> but that did not work when launching kicad from a shortcut.
>>>>>>>>
>>>>>>>> Option B a cleaner solution but still requires some configuration by the
>>>>>>>> user.  This is going to be an interesting problem to solve for our
>>>>>>>> package devs.  We need to figure out a way to generate or modify the
>>>>>>>> spinit file base on where it gets installed by the installer on
>>>>>>>> platforms where this is relevant.  We will also either have to set an
>>>>>>>> the SPICE_LIB_DIR environment variable or teach ngspice how to find the
>>>>>>>> correct spinit file at run time.
>>>>>>>>
>>>>>>>> At least now windows users have a way to have the same functional spice
>>>>>>>> simulation as linux users.
>>>>>>>>
>>>>>>>> Cheers,
>>>>>>>>
>>>>>>>> Wayne
>>>>>>>>
>>>>>>>> _______________________________________________
>>>>>>>> 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
>>>>
>