Problems with Hspice simulation in Eldo

Hi everyone,

I extract a very simple hspice netlist (of an inverter) from cadence to simulate in Eldo 2010.1. But I have a problem when simulating the netlist as follow:
# Error: (eldo - 1577) In file "./eldo/tsl018.cir" line 3261:
# + OBJECT "X1.C1.XM1.M": Model NHV.NHV not yet defined.
When I delete the line of 3261 in the file tsl018.cir, there is no more problem, but neither does the output wave form appear, though there are input wave forms. Does it mean that I need to add some lines to my tsl018.cir file? Could you please help me with this problem.

BR,
thikgaidep

Re: Hspice simulation in Eldo

You need to show your netlist. From what you have said it just sounds like a misnamed model in the device.

Keith

Re: Hspice simulation in Eldo

Thank you for your reply. This is my net list:

.TEMP 25.0
.OPTION
+ ARTIST=2
+ INGOLD=2
+ PARHIER=LOCAL
+ PSF=2
+ SCALE=1e-06

.LIB "/.../eldo/global.lib" GLOBAL
.LIB "/.../eldo/fet.lib" NOM
.LIB "/.../fethv.lib" NOM
.LIB "/.../eldo/bjt.lib" NOM
.LIB "/.../eldo/accap.lib" NOM
.LIB "/.../eldo/mimcap.lib" NOM
.LIB "/.../eldo/mfc.lib" NOM
.LIB "/.../eldo/res.lib" NOM
.LIB "/.../eldo/diode.lib" NOM
.LIB "/.../eldo/tsl018.cir" NOM


** Library name: 123
** Cell name: analog_block
** View name: schematic
.subckt analog_block supply gnd input output
.connect gnd 0
xm0 output input supply supply phv L=300e-3 W=420e-3 AD=201.6e-3 AS=201.6e-3 PD=1.8 PS=1.8 NRD=1.40909 NRS=1.40909 M=1
xm1 output input gnd gnd nhv L=350e-3 W=420e-3 AD=201.6e-3 AS=201.6e-3 PD=1.8 PS=1.8 NRD=1.40909 NRS=1.40909 M=1
.ends analog_block


And here is the lines of the tsl018.cir:

.subckt nhv d g s b l=1u w=1u nrs=1 nrd=1 as=0 ad=0 ps=0 pd=0
...
m d g s b nhv w=w l=l delvto=sigvtn_hv as=aseff ps=pseff ad=adeff pd=pdeff nrs=nrs nrd=nrd m=m[/I][/I]
.ends nhv

The underlined line is 3261, which is reported as error as followed:

# ** Error: (eldo - 1577) In file "./eldo/tsl018.cir" line 3261:
# + OBJECT "X1.C1.XM1.M": Model NHV.NHV not yet defined.
# ** Error: (eldo - 876) In file "./eldo/tsl018.cir" line 3261:
# + OBJECT "X1.C1.XM1.M": L and W must be specified before M(<param>)
# ** Error: (eldo - 254) In file "./eldo/tsl018.cir" line 3261:
# + OBJECT "X1.C1.XM1.M": Unknown parameter DELVTO
# ** Error: (eldo - 1577) In file "./eldo/tsl018.cir" line 3261:
# + OBJECT "X1.C1.XM1.M": Model NHV.NHV not yet defined.

Re: Hspice simulation in Eldo

You main subcircuit calls another subcircuit called NHV. That has a transistor also called NHV. It is that transistor that is undefined. It should be in your TSMC libraries but it may have a different name. Open them up with a text editor & do a search. It can be risky having both a subcircuit and model with the same name although simulators usually manage. To be on the safe side you could rename the subcircuit something like SUB_NHV. That would also make it easier to understand the errors.

Keith.

Re: Hspice simulation in Eldo

Thank you for your reply, following are brief lines of the tsl018.cir:

.subckt nhv d g s b l=1u w=1u nrs=1 nrd=1 as=0 ad=0 ps=0 pd=0
...
m d g s b nhv w=w l=l delvto=sigvtn_hv as=aseff ps=pseff ad=adeff pd=pdeff nrs=nrs nrd=nrd m=m
.ends nhv

(underlined is where the error reported - line 3261)
Following are definition of models:
.model nhv.1 nmos (...)
.model nhv.2 nmos (...)
...
.model nhv.9 nmos (...)

When I change nhv in line 3261 above into '1', there comes an error report as following which similar to the previous one:

# ** Error: (eldo - 1577) In file "./eldo/tsl018.cir" line 3261:
# + OBJECT "X1.C1.XM1.M": Model NHV.1 not yet defined.
# ** Error: (eldo - 876) In file "./eldo/tsl018.cir" line 3261:
# + OBJECT "X1.C1.XM1.M": L and W must be specified before M(<param>)
# ** Error: (eldo - 254) In file "./eldo/tsl018.cir" line 3261:
# + OBJECT "X1.C1.XM1.M": Unknown parameter DELVTO
# ** Error: (eldo - 1577) In file "./eldo/tsl018.cir" line 3261:
# + OBJECT "X1.C1.XM1.M": Model NHV.1 not yet defined.

When changing 'nhv' into 2,3,...9, same types of error happen.

Re: Hspice simulation in Eldo

OK, I think the problem is to do with "binning". Sometimes the models are grouped where one model is used for small transistors, another for slightly larger ones etc. the models usually have the form nmod.1 nmod.2 nmod.3 etc with each model covering a range of W & L. You will need to look in your manual under binning to fix this (I don't use Eldo). The problem is possibly that your model is trying to call the nhv.1 nhv.2 nhv.3 models which are referenced from another file. Sometimes the file you should call then references the binning file. When you get model files from fabs the directories, paths and environment variables sometimes don't match and need editing.

Keith