kicad-developers team mailing list archive

[Maciej Sumiński <maciej.suminski@xxxxxxx>]

I believe it should not be necessary. No matter what, the problematic
settings are overridden after loading the default and custom
configuration files. Sure, you can add a Spice directive in the
schematic sheet which enable them, but then you are really shooting your
own foot on purpose.

Regards,
Orson

On 10/13/2016 06:22 PM, Simon Wells wrote:
> If the user file is loaded is it worth adding this to the copy version
> info or something to make it easy to see and ask someone about a
> custom init file if they experience issues with it?
> 
> On Fri, Oct 14, 2016 at 4:13 AM, Maciej Sumiński
> <maciej.suminski@xxxxxxx> wrote:
>> It still loads the original configuration files (when possible) and
>> afterwards it checks a few extra locations (relative to the executed
>> binary path). This gives a chance to package maintainers to provide a
>> proper spinit file. If it fails to find a custom spinit file, but it
>> detects a path to codemodel libraries correctly, it will just load them.
>>
>> Regards,
>> Orson
>>
>> On 10/13/2016 04:08 PM, Wayne Stambaugh wrote:
>>> 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
>>>>>>>
>>>>
>>
>>
>>
>> _______________________________________________
>> 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
>>

Attachment: signature.asc
Description: OpenPGP digital signature