Issue with Level=3 MOS model in Spectre

I am using an external SPICE model and the model defines a voltage dependent capacitor as follows:

C11 11 12 1E-12
V11 11 0 0Vdc
B11 3 2 I= V(13,0)*I(V11)
E11 12 0 3 2 1
E12 13 0 VCVS PWL(1) 12 0 -20.0,287.92 .......

When I run this Spice model in Spectre with the statement simulator lang=spice I get the following error:

 The instance `B11' does not have a valid master.

From the Spectre User Guide Spice compatibility section it does say that it supports SPICE behavioral sources. Why then it cannot recognize this behavioral source?

I'm not sure which version of Spectre you're using, but in SPECTRE23.1 at least it fails with a different error for me, indicating that the "B" line is modelled as an IBIS source and the IBIS file is missing. From my checks, the "B" prefix is for IBIS sources in other SPICE simulators too so we have followed that when using SPICE syntax.

If you want this to be a behavioural current source, change B11 to I11 and that should do it.

Andrew

I joined your two posts because they appear to be asking the same thing.

Note that the Spectre model for a level 3 MOS is "mos3" (see "spectre -h mos3")

Andrew

Sorry for the incomplete information. I am using quite an old version of Spectre:

Version 15.1.0.803.isr18 64bit

After I change it to I11 it does simulate but the MOS characteristic is totally off. The drain current is orders of magnitude lower so it may be something related to the model. The model I am using is this:

https://assets.nexperia.com/documents/spice-model/PSMN8R5-40MSD.lib

Note however I did have to change the E12 definition from:

E12 13 0 TABLE {V(12)}
+ (-20.0,287.92) .....

to

E12 13 0 VCVS PWL(1) 12 0 -20.0,287.92 .....

to make it work.

I am simulating in an old version of spectre:

Version 15.1.0.803.isr18 64bit -- 21 Jun 2017

I am simulating the following model:

https://assets.nexperia.com/documents/spice-model/PSMN8R5-40MSD.lib

After running it as a Spectre model the MOS characteristic does not look right, i.e. the MOS Ids-Vds characteristic is orders of magnitude different. My translated spectre model is pasted below:

subckt PSMN8R5_40MSD D G S B

* Package impedance
LD (D 5) inductor l=20.00p
RLD2 (D 5) resistor r=25.13m
RLD1 (5 4) resistor r=5.000u
LG (G 1) inductor l=1.509n
RLG (G 1) resistor r=1.896
LS (S 8) inductor l=440.0p
RLS2 (S 8) resistor r=552.9m
RLS1 (8 7) resistor r=450.0u

* Drain,gate and source resistances
RD (3 4) resistor r=5.913m TC1= 6.580m TC2= 1.004n
RG (1 2) resistor r=805.9m
RS (6 7) resistor r=1.000u
RBULK (S B) resistor r=1.000u

* Body Diode
RBD (9 4) resistor r=1.911m TC1= 4.000m TC2= 23.00u
DBD (7 9) D_DBD
RDS (7 4) resistor r=40.00M TC1= -5.000m

* Internal MOS
M1 (3 2 6 6) MINT

* Gate leakage and gate capacitance
RGS (2 6) resistor r=200.0M
CGS (2 6) capacitor c=927.5p

* CGD
C11 (11 12) capacitor c=1E-12
V11 (11 0) vsource dc=0 type=dc
B11 (3 2) bsource I=V(13)*I(V11)
E11 (12 0 3 2) vcvs gain=1
E12 13 0 vsource v = table(v(12), -20.0, 287.92, -16.0, 287.86, -15.0, 287.87, -12.0, 287.87, -10.0, 287.85, -8.0, 287.88, -6.0, 287.86, -5.0, 287.87, -4.0, 287.86, -3.0, 287.69, -2.0, 286.80, -1.0, 275.62, -0.5, 236.32, -0.2, 220.97, -0.1, 220.76, 0.0, 200.6204, 0.1, 180.444, 0.2, 180.7272, 0.5, 164.752, 1.0, 142.2876, 2.0, 108.7704, 3.0, 85.0832, 4.0, 67.9872, 5.0, 57.4872, 6.0, 51.7236, 8.0, 47.49, 10.0, 46.824, 12.0, 46.364, 15.0, 45.4972, 16.0, 45.2384, 20.0, 44.1484, 25.0, 43.1592, 30.0, 42.5252, 32.0, 42.3004)

* E12 (13 0) TABLE {V(12)}
* + (-20.0,287.92) (-16.0,287.86) (-15.0,287.87) (-12.0,287.87) (-10.0,287.84999999999997) (-8.0,287.88) (-6.0,287.86) (-5.0,287.87) (-4.0,287.86) (-3.0,287.69) (-2.0,286.79999999999995) (-1.0,275.61999999999995) (-0.5,236.31999999999996) (-0.2,220.97) (-0.1,220.76) (0.0,200.6204) (0.1,180.444) (0.2,180.72719999999995) (0.5,164.75200000000004) (1.0,142.2876) (2.0,108.7704) (3.0,85.08319999999999) (4.0,67.98720000000002) (5.0,57.4872) (6.0,51.72359999999999) (8.0,47.49) (10.0,46.824) (12.0,46.364000000000004) (15.0,45.4972) (16.0,45.23840000000001) (20.0,44.1484) (25.0,43.1592) (30.0,42.525199999999984) (32.0,42.300399999999996)

model MINT mos3 Vto= 4.100 Kp= 167.8 Nfs= 1.062T Eta= 0.000
+ Level= 3 Gamma= 0.000 Phi= 600.0m Is= 1.000E-24 UO= 600.0
+ Js= 0.000 Pb= 800.0m Cj= 0.000 Cjsw= 0.000 Cgso= 0.000 Cgdo= 0.000 Cgbo= 0.000
+ Tox= 100.0n Xj= 0.000
+ Vmax= 403.3

model D_DBD diode Bv= 44.00 Ibv= 250.0u Rs= 1.000u Is= 385.9f
+ N= 1.000 M= 392.5m VJ= 621.9m Fc= 500.0m Cjo= 1.592n Tt= 13.61n

ends PSMN8R5_40MSD

Using Spectre version:

Version 15.1.0.803.isr18 64bit -- 21 Jun 2017

The SPICE model I am using is of PSMN8R5-40MSD from the nexperia website

It did work after changing B11 to I11 but the MOS characteristics are order of magnitude off. So somehow the model is not being interpreted correctly.

Note that I also had to change the E12 definition from TABLE to PWL to make it work.

It did simulate after I converted the whole model to Spectre but the characteristic of the MOS is very off. My converted model to Spectre looks like this:

subckt PSMN8R5_40MSD D G S B

* Package impedance
LD (D 5) inductor l=20.00p
RLD2 (D 5) resistor r=25.13m
RLD1 (5 4) resistor r=5.000u
LG (G 1) inductor l=1.509n
RLG (G 1) resistor r=1.896
LS (S 8) inductor l=440.0p
RLS2 (S 8) resistor r=552.9m
RLS1 (8 7) resistor r=450.0u

* Drain,gate and source resistances
RD (3 4) resistor r=5.913m TC1= 6.580m TC2= 1.004n
RG (1 2) resistor r=805.9m
RS (6 7) resistor r=1.000u
RBULK (S B) resistor r=1.000u

* Body Diode
RBD (9 4) resistor r=1.911m TC1= 4.000m TC2= 23.00u
DBD (7 9) D_DBD
RDS (7 4) resistor r=40.00M TC1= -5.000m

* Internal MOS
M1 (3 2 6 6) MINT

* Gate leakage and gate capacitance
RGS (2 6) resistor r=200.0M
CGS (2 6) capacitor c=927.5p

* CGD
C11 (11 12) capacitor c=1E-12
V11 (11 0) vsource dc=0 type=dc
B11 (3 2) bsource I=V(13)*I(V11)
E11 (12 0 3 2) vcvs gain=1
E12 13 0 vsource v = table(v(12), -20.0, 287.92, -16.0, 287.86, -15.0, 287.87, -12.0, 287.87, -10.0, 287.85, -8.0, 287.88, -6.0, 287.86, -5.0, 287.87, -4.0, 287.86, -3.0, 287.69, -2.0, 286.80, -1.0, 275.62, -0.5, 236.32, -0.2, 220.97, -0.1, 220.76, 0.0, 200.6204, 0.1, 180.444, 0.2, 180.7272, 0.5, 164.752, 1.0, 142.2876, 2.0, 108.7704, 3.0, 85.0832, 4.0, 67.9872, 5.0, 57.4872, 6.0, 51.7236, 8.0, 47.49, 10.0, 46.824, 12.0, 46.364, 15.0, 45.4972, 16.0, 45.2384, 20.0, 44.1484, 25.0, 43.1592, 30.0, 42.5252, 32.0, 42.3004)

* E12 (13 0) TABLE {V(12)}
* + (-20.0,287.92) (-16.0,287.86) (-15.0,287.87) (-12.0,287.87) (-10.0,287.84999999999997) (-8.0,287.88) (-6.0,287.86) (-5.0,287.87) (-4.0,287.86) (-3.0,287.69) (-2.0,286.79999999999995) (-1.0,275.61999999999995) (-0.5,236.31999999999996) (-0.2,220.97) (-0.1,220.76) (0.0,200.6204) (0.1,180.444) (0.2,180.72719999999995) (0.5,164.75200000000004) (1.0,142.2876) (2.0,108.7704) (3.0,85.08319999999999) (4.0,67.98720000000002) (5.0,57.4872) (6.0,51.72359999999999) (8.0,47.49) (10.0,46.824) (12.0,46.364000000000004) (15.0,45.4972) (16.0,45.23840000000001) (20.0,44.1484) (25.0,43.1592) (30.0,42.525199999999984) (32.0,42.300399999999996)

model MINT mos3 Vto= 4.100 Kp= 167.8 Nfs= 1.062T Eta= 0.000
+ Level= 3 Gamma= 0.000 Phi= 600.0m Is= 1.000E-24 UO= 600.0
+ Js= 0.000 Pb= 800.0m Cj= 0.000 Cjsw= 0.000 Cgso= 0.000 Cgdo= 0.000 Cgbo= 0.000
+ Tox= 100.0n Xj= 0.000
+ Vmax= 403.3

model D_DBD diode Bv= 44.00 Ibv= 250.0u Rs= 1.000u Is= 385.9f
+ N= 1.000 M= 392.5m VJ= 621.9m Fc= 500.0m Cjo= 1.592n Tt= 13.61n

ends PSMN8R5_40MSD

Some more information. I reduced the model to just the MOS model:

simulator lang=spice

.SUBCKT MYMOS D G S

* Internal MOS
M1 D G S S MINT

.MODEL MINT NMOS Vto= 4.100 Kp= 167.8 Nfs= 1.062T Eta= 0.000
+ Level= 3 Gamma= 0.000 Phi= 600.0m Is= 1.000E-24 UO= 600.0
+ Js= 0.000 Pb= 800.0m Cj= 0.000 Cjsw= 0.000 Cgso= 0.000 Cgdo= 0.000 Cgbo= 0.000
+ Tox= 100.0n Xj= 0.000
+ Vmax= 403.3

.ENDS

I just used this model to do a DC Vds sweep (VGS=5V) in Spectre and compare it to a Spice simulator.

The Spice simulation output looks like this:

while the Spectre simulation looks like this:

So something is not right in just the model simulation for level 3 mos model in Spectre. I don't know what am I doing wrong. Any guidance will be helpful.

Thanks.

For a start, there is no W and L specified on the MOS instance line, so I'm assuming some default values must be being used. With Spectre, these are 3um for both W and L, and my guess is that it must be larger (especially if the currents are that high). I don't know which SPICE simulator you are comparing against.

That said, just increasing the W and L to something much larger doesn't match (I set them to 1 each as I found some reference that this might be happening with LTSPICE, but elsewhere it said 100u was the default). With 1 I needed to set wmax and lmax in the model to a bit higher to prevent a warning. This is all guesswork though since I don't know what you're trying to be compatible with and if it's even feasible to be compatible.

You might want to contact the model provider to see if they provide a Spectre-compatible model or at least one for PSPICE (we have pspice_include in Spectre which gives a good level of compatibility).

Andrew

Thanks for this information. I simulated it in Qspice. I am trying to dig what are the default W/L this would use. So this is something that is different even though we are importing a Spice model I did not know that the Spice defaults are not known by Spectre. So this is a good caution for me for the future.

I am trying to see if I can get an alternate model or a Pspice model from somewhere and try that. If I create a Pspice cell view would that be equivalent to pspice_include?