Stats

  • Locked Locked
  • Replies 5
  • Subscribers 125
  • Views 15542
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Netlisting error when using hspiceD simulator in cadence 5.14

isazulkc

 Hi,

I want to use hspiceD simulator to run some basics noise analysis on a single NMOS M1, but the netlist and simulation fail.

 the switch view list in  the simulator is : hspiceD spice cmos_sch cmos.sch schematic

 the stop view list  in the simulator is:hspiceD spice. And I created a hspiceD view of the nfet by copy+paste+rename the symbol view.

  I get this error:

**** "Begin incrementl netlisting

Netlist Error: cannot find any info on instance "M1" in cell  "LibraryName" "Cellname" "Schematic" 

End netlisting

ERROR (OSSHNL): Error(s) found during netlisting. the netlist  may be corrupt or may not be produced at all"

 

I tried many thing but no one works:

 ***** When I add symbol view at the beginning of the switch list I got this error:

WARNING: Netlister: The switch view symbol of cell nfet in library cmosp18 has no instance, hence is being ignored.

To netlist this cell, add this view to the stop list and to ignore any particular instance use nlAction="ignore"

The same message is for the cell Vdc from analogLib.

 Then when I add symbol view to the stop list, I got the same error as the first presented.

 

How can I fix this problem and run a simulation with hspiceD in Cadence 5.14?? any help will be very very appreciated. I don't what to try anymore.

 Thx!

 

 

 

  • If you do Tools->CDF->Edit CDF, and pick the nfet component, is there anything set up in the hspiceD simulation information? My guess is that nothing is defined in this part of the CDF and as a result the netlister does not know how to netlist this component.

    Adding symbol to the beginning of the switch list makes no sense, because it will then try to traverse hierarchy in the symbol views (assuming it is not in the stop list) and there won't be any, hence the error. If you were to add it ("symbol") to the stop list too, it would never traverse any hierarchy. Not really sure why you tried doing this, because it doesn't make any sense.

    Anyway, the most likely cause is the lack of hspiceD CDF simInfo.

    Regards,

    Andrew

  •  Hi Andrew,

    thanks for your answer! As you said there were no simInfo for hspiceD in the CDF. I never edited CDF before, and I see now how important it is. Now the netlist pass but the simulation still fails.

    What I have done is: Edit nfet SimInfo CDFfor hspiceD  in "Effective CDF type" . The information edited for hspiceD  and the error message can be on the attached image.

     It seems like it doesn't see the nch model of the Nfet even if this is defined in the include file icfhspice.init.(I put W=500n and L= 400n)

     is it a bad setting problem?? what changes are needed?

     Thanks you!! 

    Best Regards

    CDF_edit.doc

  • Generally speaking you're better off cutting and pasting the messages into the post, rather than using screenshots in documents - when travelling, it's much harder to see otherwise.

    Anyway, first thing is that the netlist procedure is probably wrong - ansSpiceDevPrim is really for socket netlisters, such as hspiceS. Either leave the netlistProcedure blank, or put hspiceDCompPrim, which is the netlist procedure for nmos4 in analogLib (amongst others).

    The simulator message either means that you've not included the model files, under Setup->Model Libraries (in the ADE window), or that the dimensions are wrong. Or that you're not netlisting the w and l for some reason - I couldn't see your complete instParameters from the screenshot.

    Better to post the hspiceD info from running cdfDump("yourLib" "yourTran.cdf" ?cellName "yourTran")  where yourLib is your library name, and yourTran is the name of the component.

    Also, show what's in the netlist - usually looking at the netlist makes it pretty obvious what is wrong.

    Regards,

    Andrew.

  • Hi Andrew,

    the HspiceD info is:                                                           
    netlistProcedure: hspiceDCompPrim                                                       
    otherParameters: model                                        
    instParameters: ps ps nrd nrs rsc off Vds Vgs Vbs dtemp geo                                               
    componentName: hnmos                                                        
    namePrefix:                                         
    termOrder: D G S B                                                        
    termMapping:                                                         
    propMapping: nil vds Vds vgs Vgs vbs Vbs                                      
    optParamExprList:                                     

    I saw that the nfet is not netlisted (the schematic is only an nfet in common source configuration) :

    .GLOBAL vssa! vdda!

    .AC DEC 30 1.0 1e9
    .DC v17 0.0 2.0 1e-3
    .NOISE V(out) v17 10
    .PRINT NOISE ONOISE INOISE
    .TRAN 100e-9 2e-3 START=0.0
    .OP

    .TEMP 25
    .OPTION
    +    ARTIST=2
    +    INGOLD=2
    +    MEASOUT=1
    +    PARHIER=LOCAL
    +    PSF=2
    .INCLUDE "./icfhspice.init"

    ** Library name: design_lib
    ** Cell name: source_tension_1_8V_3_3V
    ** View name: schematic
    .subckt source_tension_1_8V_3_3V vcc_3_3 vdd vss
    v2 vcc_3_3 0 DC=3.3
    v1 vdd 0 DC=1.8
    v0 0 vss DC=0
    .ends source_tension_1_8V_3_3V
    ** End of subcircuit definition.

    ** Library name: Test_LN5
    ** Cell name: essai_MOS_Hspice
    ** View name: schematic
    r0 out vdda! 10e3

    v17 net014 vssa! DC=900e-3 AC 1
    xi85 vcc vdda! vssa! source_tension_1_8V_3_3V
    .END

    which information do I need to change to be able to netlist the transistor?

    Thanks a lot!!

    Best Regards!
  • Oups!! Sorry I don't know why the system didn't consider the layout of the previous post. (the return are not respected) I will reedit it tomorrow to see if it will be more readable.

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.