Third Party Model Import Fatal error: Unknown device type: a

In trying to import the model for the LT1028 op-amp, I get this error:

Fatal error: Unknown device type:a

There is no item A in the Device Reference of the current QSPICE Documentation.
Is it correct to understand that it is currently under development and is in a pending state?

View > Netlist
may be easier to identify problem from netlist for schematic with subckt
also consider to share the .subckt you are using for LT1028

Hi,thank you for your advice.
The netlist is here.


R1 N03 N01 1K
R2 N01 N02 10K
R3 0 OUT 2K
V1 N03 0 AC 1
V2 +15V 0 15
V3 -15V 0 -15
L1 N02 OUT L
.subckt X1畢T1028 1 2 3 4 5
A1 2 1 0 0 0 0 0 0 OTA g=0 in=.9p ink=250 incm=2.4p incmk=250
M1 3 N012 5 5 N temp=27
M2 4 N012 5 5 P temp=27
C3 3 5 .5p
C4 5 4 .5p
B1 0 N011 I=10udnlim(uplim(V(1),V(3)-2.7,.1), V(4)+2.7, .1)+1nV(1)
B2 N011 0 I=10udnlim(uplim(V(2),V(3)-2.69,.1), V(4)+2.69, .1)+1nV(2)
C6 3 1 2.5p Rpar=1.2G noiseless
C7 1 4 2.5p noiseless Rpar=1.2G
C8 2 4 2.5p Rpar=1.2G noiseless
C9 3 2 2.5p Rpar=1.2G noiseless
A2 0 N011 0 0 0 0 N021 0 OTA g=630u Iout=17.51u en=.85n+freq36u/(8kfreq+(freq-400k)**2) Vlow=-1e308 Vhigh=1e308 Cout= 1.7p enk=3
C10 N011 0 1f Rpar=100K noiseless
D4 N021 3 X
D5 4 N021 X
D1 N012 5 Y
D6 5 N012 Y
D7 3 4 DP
C11 2 1 12.5p Rpar=20k noiseless
G4 0 N014 N021 0 1オ
D2 2 1 DIN
R3 N014 0 1Meg Noiseless
C1 N014 0 {Cfp1}
R4 N005 N006 {R1a_Avo} Noiseless
R5 N006 0 {R2a_Avo} Noiseless
G1 0 N007 N006 0 {G2_Avo}
C2 N006 N005 {C1a_Avo}
G2 0 N005 N015 0 1
R7 N005 0 1 Noiseless
G3 0 N015 N014 0 1オ
R8 N015 0 1Meg Noiseless
C5 N015 0 {Cfp1}
R9 N009 N010 {R1b_Avo} Noiseless
R10 N010 0 {R2b_Avo} Noiseless
G5 0 N004 N010 0 {G3_Avo}
C12 N010 N009 {C1b_Avo}
R11 N004 0 1 Noiseless
R12 N009 0 1 Noiseless
R14 N002 N001 {R2x_Avo} Noiseless
R15 N001 N004 {R1x_Avo} Noiseless
Rx1 N016 N004 {Rx_Avo} Noiseless
Cx1 N016 0 {Cx_Avo}
G8 0 N002 N016 N001 1Meg
R16 0 N002 1 Noiseless
G6 0 N017 N002 0 1オ
R6 N017 0 1Meg Noiseless
C13 N017 0 {Cfp2}
G7 0 N018 N017 0 1オ
R13 N018 0 1Meg Noiseless
C14 N018 0 {Cfp2}
R17 N007 N008 {R1a_Avo} Noiseless
R18 N008 0 {R2a_Avo} Noiseless
G9 0 N009 N008 0 {G2_Avo}
C15 N008 N007 {C1a_Avo}
R19 N007 0 1 Noiseless
G10 0 N019 N018 0 1オ
R20 N019 0 1Meg Noiseless
C16 N019 0 {Cfp3}
G11 0 N020 N019 0 1オ
R21 N020 0 1Meg Noiseless
C17 N020 0 {Cfp3}
G12 0 N012 N020 0 1オ
R22 N012 0 1Meg Noiseless
C18 N012 0 {Cfp3}
.model X D(Ron=1K Roff=100G Vfwd=-2 epsilon=.1 noiseless)
.model Y D(Ron=500 Roff=1T Vfwd=1.18 epsilon=.1 noiseless)
.model N VDMOS(Vto=-200m Kp=40m)
.model P VDMOS(Vto=200m Kp=40m pchan)
.model DP D(Roff=1T Ron=1k Vfwd=0.5 ilimit=6.602m noiseless)
.model DIN D(Ron=100 Roff=1T Vfwd=1.8 Vrev=1.8 noiseless)
.param fp1=1.5Meg fp2=50Meg fp3=300Meg
.param Cfp1={1 / (2 * pi * fp1 * 1Meg)}
.param Cfp2={1 / (2 * pi * fp2 * 1Meg)}
.param Cfp3={1 / (2 * pi * fp3 * 1Meg)}
.param R1a_Avo=10k
.param fz1_Avo=3.5Meg
.param fp1_Avo=100G
.param C1a_Avo = {1 / (2 * pi * R1a_Avo * fz1_Avo)}
.param R2a_Avo = {R1a_Avo/ ((2 * pi * fp1_Avo * C1a_Avo * R1a_Avo) - 1)}
.param actual1_Avo = {R2a_Avo / (R1a_Avo + R2a_Avo)}
.param G2_Avo = {1/actual1_Avo}
.param Rx_Avo=1k
.param R2x_Avo=10k
.param fpx_Avo=99G
.param fzx_Avo=45Meg
.param Cx_Avo={1/(2piRx_Avofpx_Avo)}
.param R1x_Avo={(fzx_Avo
R2x_Avo)/fpx_Avo}
.param R1b_Avo=10k
.param fz2_Avo=5.5Meg
.param fp2_Avo=17Meg
.param C1b_Avo = {1 / (2 * pi * R1b_Avo * fz2_Avo)}
.param R2b_Avo = {R1b_Avo/ ((2 * pi * fp2_Avo * C1b_Avo * R1b_Avo) - 1)}
.param actual2_Avo = {R2b_Avo / (R1b_Avo + R2b_Avo)}
.param G3_Avo = {1/actual2_Avo}
.ends LT1028
X1 0 N01 +15V -15V OUT X1畢T1028
.ac dec 100 1 10Meg
.param L=1オ
.step param L list 1オ 1000G
.options gmin=0
.end

LT1028 contains two A-devices

A-device is undocumented in LTspice, please refer to this link for detail
Undocumented LTspice - LTwiki-Wiki for LTspice

A-devices are Linear Technology Corporation’s proprietary special function/mixed mode circuit simulation elements. Not sure if Qspice can support that, let see Mike’s response.

LTspice has the A-device as an OTA building block for Op-Amps. It’s dated and unique to LTspice, so I didn’t implement it for QSPICE.

The next generation, in QSPICE, is the à device. It solves the hardest part of Op-Amp modeling, a transconductance that draws power from the appropriate rail. It also supports an extension that is a compete Rail-To-Rail Op-Amp as a native circuit element. I’m generating a notes on how to use it and illustrate its value.

As far as the LT1028, that is a device I’ve used extensively for signal conditioning down hole in oil exploration.

The trick to modeling it is that it has about 30pF capacitance between the inputs which makes stability challenging. The datasheet isn’t lying when it talks about just a few pF input capacitance. That’s on the non-inverting input while in voltage-follower configuration. You don’t see the 30pF because it’s bootstrapped due to the voltage follower configuration.

If you can find a PSpice LT1028 model, use that. If it’s missing the input to input capacitance add it.

1 Like

Thank you very much for your clear explanation.
I understand that you have incorporated a new device to replace the A device.
So I researched and found one in the PSpice library for the old LT1028.

The following is from the PSpice Model.

Netlist

R1 N03 N01 1K
R2 N01 N02 10K
R3 0 OUT 2K
V1 N03 0 AC 1
V2 +15V 0 15
V3 -15V 0 -15
L1 N02 OUT L
.SUBCKT X1畢T1028/LT 3 2 7 4 6
RC1 7 80 7.0736E+01
RC2 7 90 7.0736E+01
Q1 80 2 10 QM1
Q2 90 3 11 QM2
C1 80 91 750E-12
RXC1 91 90 50
CXC1 91 90 400E-12
C2 1 98 30.000E-12
RXC2 98 8 1K
CXC2 98 8 10.000E-12
CIN 2 3 15E-12
RIN 2 3 2E4
DDM1 2 104 DM2
DDM3 104 3 DM2
DDM2 3 105 DM2
DDM4 105 2 DM2
RE1 10 12 -4.4157E+01
RE2 11 12 -4.4157E+01
IEE 12 4 4.5006E-04
RE 12 0 4.4439E+05
CE 12 0 1.5789E-12
GCM 0 8 12 0 7.0854E-09
GA 8 0 80 90 1.4137E-02
R2 8 0 1.0000E+05
GB 1 0 8 0 2.6731E+02
RO2 1 0 7.9000E+01
RS 1 6 1
ECL 18 0 1 6 2.7910E+01
GCL 0 8 20 0 1
RCL 20 0 1E3
D1 18 20 DM1
D2 20 18 DM1
D3A 131 70 DM3
D3B 13 131 DM3
GPL 0 8 70 7 1
VC 13 6 3.6394
RPLA 7 70 1E4
RPLB 7 131 1E5
D4A 60 141 DM3
D4B 141 14 DM3
GNL 0 8 60 4 1
VE 6 14 3.6394
RNLA 60 4 1E4
RNLB 141 4 1E5
IP 7 4 7.450E-03
DSUB 4 7 DM2
.MODEL QM1 NPN (IS=8.0000E-16 BF=5.7692E+03)
.MODEL QM2 NPN (IS=8.0062E-16 BF=1.0714E+04)
.MODEL DM1 D (IS=1.000E-19)
.MODEL DM2 D (IS=8.000E-16)
.MODEL DM3 D (IS=1.000E-20)
.ENDS LT1028/LT
X1 0 N01 +15V -15V OUT X1畢T1028/LT
.ac dec 100 1 10Meg
.param L=1オ
.step param L list 1オ 1000G
.options gmin=0
.end

@ rmruthyun proposed an idea to convert LTspice A-device to Qspice Ã-device or ¥-device. It is a tedious process and requires a lot of knowledge and between these device model.

Support for LTspice A type models (Schmitt, OR, AND, ext)? - QSPICE - Qorvo Tech Forum

Here is a conversion results for LT1028.lib
As Qspice and LTspice are different (or my knowledge limitation), I cannot model all instance parameters and have to give up some of them during conversion, which included incm, incmk, en with equation and ilimit in diode model. But simulation result by compare to LT1082 demo circuit in LTspice is still identical. Up to now, I can successfully convert 3 subckt which include logic or OTA A-device, and with identical or very close simulation results.

5 Likes