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.sumin...@cern.ch>: >>>>> 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 <stambau...@gmail.com>: >>>>>>> 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@lists.launchpad.net >>>>>>>>> Unsubscribe : https://launchpad.net/~kicad-developers >>>>>>>>> More help : https://help.launchpad.net/ListHelp >>>>>>>>> >>>>>>>> >>>>>>>> >>>>>>> >>>>>>> >>>>>>> _______________________________________________ >>>>>>> Mailing list: https://launchpad.net/~kicad-developers >>>>>>> Post to : kicad-developers@lists.launchpad.net >>>>>>> Unsubscribe : https://launchpad.net/~kicad-developers >>>>>>> More help : https://help.launchpad.net/ListHelp >>>>> >>
signature.asc
Description: OpenPGP digital signature
_______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp