Wrong? simulator results

[C4dahl]

I am a new user of MultiSim and I am using the Analog Devices version.

I have a very simple circuit that simulation does not give me right(?) answers (see PDF document attached).  Also attached is the circuit file.

1.) U1, a voltage follower, output pin 6 does not follow input pin 3.

2.) U2 output is not correct for voltages on input pins.

[lacy]

I have been examining you circuit and I have found some things that may be of interest. The voltage follower U1 is working correctly. The problems arise from the AD8611AR ICs. These are ICs that have been created from a spice model. When I unhook everything from them except for VCC I still read the 3Vdc constantly on both inputs. This indicates to me that the model file is not working correctly in Multisim and this is why the circuit isn't working. Not all spice model files will work correctly with Multisim and I just don't have the expertise in order to decipher what about the model files are causing the problem. I would suggest maybe trying to find another spice model (if you can) and try it to see if you can get it to work. Another option would be to find a comparator in the master database that is simular to this one.That way you can at least get close to what this IC will do and your simulation results would be similar to what you would get with it.

I hope this helps somewhat. If someone can figure out what is wrong with the spice model please post it.

[lacy]

I have a question. You say your version is Analog Devices Version. I didn't realize that there was a version of Multisim that was named like this. The versions I am familiar with are the Evaluation Version, Educational Version, Base Version, Full Version, and Power Pro Version.

Where did you get it from? I am just curious.

[C4dahl]

I got to this link from the Analog Devices website:

https://lumen.ni.com/nicif/us/evalmultisimadi/content.xhtml

This is the version I am running.

[lacy]

Thanks for the link to this. I wasn't aware of this version. Apparently, the model for the AD8611 is just not working in this version. I have the Power Pro Edition and this part isn't even in my database so apparently this part has been created specifically for this version from the Spice Model from Analog Devices which doesn't work in my version either and gives the same results that you see.. The NI Team may have to address this as it may be a part defect in this particular version that needs to be corrected.

[C4dahl]

Thanks for the help.

What time is it where you are it is 10:30 PM CT.

I did not think I would get a response this time of night.

Craig

[Maxish]

Hello,

There's a problem with the AD8051 opamp - part of the internal SPICE model is commented out for some reason. I will file a bug report about this. For now, you can replace the model between the ".subckt" and ".ends" statements with the following:

Q1  4  3  5 QPI
Q2  6  2  7 QPI
RC1   50  4 20.5k
RC2   50  6 20.5k
RE1    5  8 5k
RE2    7  8 5k
EOS    3  1 POLY(1) 53 98 1.7E-3 1
IOS    1  2 0.1u
FNOI1  1  0 VMEAS2 1E-4
FNOI2  2  0 VMEAS2 1E-4

CPAR1  3 50 1.7p
CPAR2  2 50 1.7p
VCMH1 99  9 1
VCMH2 99 10 1
D1     5  9  DX
D2     7 10 DX
IBIAS 99  8 73u
*
* INTERNAL VOLTAGE REFERENCE
*
EREF1 98  0 POLY(2) 99 0 50 0 0 0.5 0.5
EREF2 97  0 POLY(2)  1 0 2 0 0 0.5 0.5
GREF2 97 0 97 0 1E-6
*
*VOLTAGE NOISE STAGE
*
DN1 51 52 DNOI1
VN1 51 98 0.61
VMEAS 52 98 0
RNOI1 52 98 6.5E-3

H1 53 98 VMEAS 1
RNOI2 53 98 1
*
*CURRENT NOISE STAGE
*
DN2 61 62 DNOI2
VN2 61 98 0.545
VMEAS2 62 98 0
RNOI3  62 98 2E-4
*
* INTERMEDIATE GAIN STAGE WITH POLE = 96MHz
*
G1   98 20 4 6 1E-3
RP1  98 20 550
CP1  98 20 3p
*
* GAIN STAGE WITH DOMINANT POLE
*
G4   98 30 20 98 2.6E-3
RG1 30 98 155k
CF1  30 45 13.5p
D5 31 99 DX
D6 50 32 DX
V1 31 30 0.6
V2 30 32 0.6
*
* OUTPUT STAGE
*
Q3  45 42 99 QPOX
Q4  45 44 50 QNOX
EO3 99 42 POLY(1) 98 30 0.7175 0.5
EO4 44 50 POLY(1) 30 98 0.7355 0.5
*
* MODELS
*
.MODEL QPI PNP (IS=8.6E-18,BF=91,VAF=30.6)
.MODEL QNOX NPN(IS=6.37E-16,BF=100,VAF=90,RC=3)
.MODEL QPOX PNP(IS=1.19E-15,BF=112,VAF=19.2,RC=6)
.MODEL DX D(IS=1E-16)
.MODEL DZ D(IS=1E-14,BV=6.6)
.MODEL DNOI1 D(KF=9E-10)
.MODEL DNOI2 D(KF=1E-8)


Note that you will get a convergence error after some time. One of the remedies is to change the RELTOL setting to 0.01 for the interactive simulation  (Simulate->Interactive simulation settings->analysis options->customize)

[C4dahl]

Thank you!

I tried changing the spice model and found that that portion is not available with the version I have.

Thanks for the help.

[lacy]

I went back and re-examined this and Max is right. The op amp U1 was the culprit and not the other op amps like I thought. I just missed this one for some reason. Anyway, I edited the model for this part per Max instructions and the circuit works now and this is what we all were shooting for. I will post the updated circuit for you since you cannot edit the models. The circuit has the corrected part in it and the only thing you have to do is to save it to your user database if you can do that with your version.

[gazi]

The AD8502 and AD8500 Spice model downloaded from Analog, when used in MultiSim 7 generate strange result (see attached file) -- output impendence from a opam was very big.

But when use the MultiSim Analog Edition, the AD8500 was simulated correctly (although there is no way? For me to check exactly what Spice model used there because component lib was disabled?)

I also tried AD8500 (guess similar to AD8502 and it is available in your MultiSim Analog Ed.) in both MultiSim 7 w/ downloaded Spice Model from Analog, and under MultiSim Analog Edition (unable to check the Spice details although the part is listed there).

Look at the attached file showing the strange result? In MultiSim 7, gain reported closer to ideal but output impendence far from reasonable; in MultiSim Analog Edition: gain is 0 (wrong!)? And output impendence 0

The circuits used are also attached.