kicad-developers team mailing list archive

[Maciej Sumiński <maciej.suminski@xxxxxxx>]

Yes, I override three Spice variables:

- unset interactive
Disable interactive mode. You should expect hang ups when the option is
enabled and you get an error during parameter evaluation (it asks you
whether you want to continue, but there is no way to confirm).

- set noaskquit
Do not ask the user whether to quit the simulation.

- set nomoremode
Disables stopping output until a return key is pressed whenever there is
a large number of lines to be displayed.

I hope these three settings are reasonable. I override them as they have
no meaning when ngspice is used as a shared library, but in a different
configuration they cause troubles. Note that I do not put them into any
config files, these options are set only when simulation is run in KiCad.

Regards,
Orson

On 10/14/2016 03:12 PM, Wayne Stambaugh wrote:
> I didn't look that carefully but are you overriding any settings from
> the user config?  I would prefer that you didn't so I don't spend time
> trying to figure out why my config settings are not being respected.
> 
> On 10/13/2016 11:13 AM, Maciej Sumiński 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
>>>>>>>
>>>>
>>
>>
>

Attachment: signature.asc
Description: OpenPGP digital signature