Trying to use MAX40089 spice model with LTSpice

Hello MTarr ,

The spice model that can be seen in the product page for MAX40089 is a macro model. With that, it is recommended to create each symbol per part. Have you tried creating each symbol and try to run it and see if there's still an error?

Thanks,

Mae

Yes, of course.

I saved the spice model, then I made a symbol that looks like a dual opamp. I got the error.

Unknown subcircuit called in:
x:u1:_1 out«:outa» v-«:vss.» n002«:ipa» n001«:ina» ul:vddl ul:opamp

The I had LTSpice auto-generate the symbol and used that in the spice circuit. I got the same error.

Here's the netlist with the auto-generated sybol:

:* D:\Morty\_ Spice Simulations\Test Circuits\MAX40079 Test Circuits\MAX40089 Test Circuit -002.asc
R1 N001 0 10R
R2 out N001 1K
V1 N002 0 SINE({offset} {ampl} {freq}) AC 1V
V2 V+ 0 3.5V
V3 0 V- 2.0V
XU1 out N001 N002 V- 0 out0 out0 V+ MAX40089
.param num_fft_pts 131072
.param timestep {1/((num_fft_pts)*freq/9)}
.tran 0 {10/freq} 0 {timestep}
;ac oct 128 10 1e8
.options plotwinsize=0
.options numdgt=10
.four {freq} 10 9 V(out) V(out+) V(out-)
.param ampl = 10.0mV
.param freq = 1K
.paramp offset = 0V
;noise V(out) V1 oct 256 20 20K
* Symbol in folder\nAutoGenerated
.lib ADI\max40089.lib
.backanno
.end

Try, I think you'll get the same error. This is a Maxim model not compatible with LT Spice. Now that Analog owns both Maxim and LT Spice, would it be possible to fix the model?

Thank you,

-Morty

PS: I tried to upload the .asc file but kept getting invalid URL errors. It would be nice to be able to upload a file so we're talking about exactly the same thing.

Hello MTarr ,

We were able to fix the model issue, but I am still coordinating with the team to upload the updated netlist file. For the mean time, I can send the file in your email/chat since I am having an issue with attaching the file. 

Also, I just want to share that there's an updated LTspice version (Version 24.0.9) in which you can downlink in LTspice Information Center | Analog Devices. 

Thank you!

Regards,

Mae

Hi,

I would appreciate receiving the updated file file by email.

Thank you for looking into this.

Morty Tarr

Hello Morty,

I've encountered an issue with a previous email not getting through. I've attached a .txt file with the updated content; you should be able to copy and paste it into .lib to proceed. Apologies for the inconvenience. 

* MAX40089 MACROMODEL
* ------------------------------
* Revision 0, 11/2017
**************************************************************************************
.SUBCKT MAX40089 OUTA INA IPA VSS IPB INB OUTB VDD
X_1 OUTA VSS IPA INA VDD1 opamp
X_2 OUTB VSS IPB INB VDD1 opamp
Vsh VDD VDD1 0
Gsh VDD 0 VALUE={-I(Vsh)+4.5m*V(ctl)+0.4u}
X_sh 0 SD ctl shutdown
.ends
.SUBCKT shutdown 18 91 cs
**************************************************************************************
V10a 10 18 5
E20 20 18 10 18 0.5
Ecs cs 18 VALUE={V(96)-V(20)}
*SHUTDOWN
RSHIN 91 20 5000K
ESH3 220 20 91 18 1
RSHA 220 221 1K
CSHA 221 20 32P
ESH2 92 20 221 20 1
RSH1 92 93 100
VSH1 93 94 0V
EHYS 95 94 POLY(2) 10 18 96 20 0 0 0 0 0.03
RBL 94 20 10K  
ESH1 95 20 10 18 0.45
****
E96 96 18 value={if(I(vsh1)<0,2.5,3.5)}
.MODEL DA D(N=10M)
.ends
**************************************************************************************
.SUBCKT opamp 202 18 17 15 10 
*111a
***************
So1 201 202 ctl 0 smod1
.model smod1 VSWITCH (Ron=0.1 Roff=10g Von=0.8 Voff=0.5)
X_sh 0 111a ctl shutdown
*INPUT STAGE
VS1 10 11 0V
GBIAS 11 12 304 100 50U 
*L1 202 203 4n
*Rl1 202 203 400
*Vo1 10 500 912m
*Vo2 501 18 915m
*Do1 202 500 DY3
*Ro11 202 2000 1000
*Co11 2000 500 100p
*Do2 501 202 DY3
.model DY2 D(IS=5E-14 N=1 RS=1m TT=0.1p VJ=0.6 FC=0.1 IBV=0.001 CJO=0)
***********************************************************************************
.MODEL DY3    D
+ IS = 2.556412E-12
+ RS = 4.959919E-3
+ N = 1.24864
+ IKF = 2.55086E-3
+ TT = 0
+ CJO = 0
+ VJ = 1
+ M = .5
+ EG = 1.11
+ XTI = 3
+ KF = 0
+ AF = 1
+ FC = .5
+ BV = 1E5
+ IBV = .001
***********************************************************************************
M1 13 16 12 11 MOSFET
M2 14 15 12 11 MOSFET
DBIAS 18 12 DY
VOS 17 16  75u
RD1 13 18 1K    
RD2 14 18 1K
C1 13 14 1P
CIN1 16 100 10P
CIN2 15 100 10P     
DIN1 16 11 DA
DIN2 18 16 DA
DIN3 15 11 DA
DIN4 18 15 DA
FSUP 18 10 VS1 1 
J1 13 14 13 JNC
J2 14 13 14 JNC
.MODEL JNC NJF
**************
*INPUT BIAS CURRENT 
IBIAS1 18 17 2.5p
IBIAS2 18 15 3.5p
GBIAS1 17 18 10 18 1p
GBIAS2 15 18 10 18 1p
RID 15 16 1000G 
**************
**************************************************
*GAIN STAGE 
GA 25 100 14 13 4M  
RO1 25 100 10k
GB 26 100 25 100 180M
RO2 26 100 1K
EF 27 100 26 100 1
CC 25 27 7P
EF2 29 100 28 100 1  
GC 100 28 26 100 22.16M
RO3 28 100 2.7k
CC2 25 29 18.3p
RO4 28 30 0.020
GCMPS 100 25 40 100 393.5U 
**************
*CURRENT LIMIT
DP3 26 38 DY
EP3 38 100 10 18 1
DP4 39 26 DY
EP4 100 39 10 18 1
**************
*INTERNAL GND
EG1 100 18 10 18 0.5
**************
*VOLTAGE LIMITING
VS2 30 31 0V
*****
DP1 30 32 DY 
HP1 34 32 VS2 17.72
EP1 34 36 10 18 0.5
VOFF1 100 36 664M
*****
DP2 33 30 DY
HP2 35 33 VS2 14.43
EP2 37 35 10 18 0.5
VOFF2 37 100 664.8M
***************
*CMRR
RRR 40 100 1
GCMR 40 100 12 18 33u
GPSR 100 40 10 18 28u
***************
*FOR SHUTDOWN
E103 103 18 10 18 1
MEN1 171 172 31 10 MOSFETP
MEN2 171 173 31 18 MOSFETN
EEN3 170 172 304 100 10
EEN4 173 170 304 100 10
RSHUNT 170 171 10MEG
VIS5 171 400 0V
R171 171 18 100k
D401 400 401 DY1
D402 402 400 DY1
D403 201 401 DY1
D404 402 201 DY1
I400 401 402 50m
********************************
RSH 103 18 500MEG
ISH 18 103 10NA
DSH 103 10 DY
CSH 103 18 10P
**************
EEN2 300 100 103 18 1
REN 300 301 10K
VEN 301 302 0V
EHYST 303 302 POLY(2) 10 18 304 100 0 0 0 0 0.4
EEN1 303 100 10 100 0.7
**************
FEN1 100 304 VEN 12
CEN 304 100 1P
DEN1 100 304 DY
DEN2 304 305 DY
VLIM1 305 100 1V
**************************************************
.MODEL DA D(IS=100E-14 RS=0.5k)
.MODEL MOSFET PMOS(VTO=-0.2 KP=29.3E-3 KF=4.4E-26 AF=0.8)
.MODEL DX D(IS=100E-14)
.MODEL DY D(IS=100E-14 N=1)
.MODEL DY1 D(N=10m)
.MODEL MOSFETP PMOS(VTO=-5.0  KP=88E-3 GAMMA=0.01)
.MODEL MOSFETN NMOS(VTO=5  KP=88E-3 GAMMA=0.01)
**************************************************
.ENDS

If you experience an issue, you can ask a question again through posting a new question. Thanks!

Best regards,

Mae

Hi Mae,

Thank you, the model seems to work. It reports distortion lower than expected, but functionality is more important than that.

Just to note -  LT Spice reports 2 warnings when running any simulation with this model:

u1:_1:dy1: Emission coefficient, N=0.01, too small, limited to 0.1
u1:_2:dy1: Emission coefficient, N=0.01, too small, limited to 0.1

One for each instance of the opamp. I get these warnings in my models as well. LT Spice used to accept N = 0.01, now it doesn't.

Thank you,

Morty

Hello Morty,

May we know how did you simulate the part so we can understand where the error is coming from? I tried it on my side and it's working accordingly. I am using the latest version of the LTspice and updated its components. Are you using the same version?

Also, I added LiliPod as assignee since she's the one handling the part to assist you further. 

Thanks,

Mae

Hi Mae, LiliPod,

I am working on an ultra low noise EKG front end for a client. They want to significantly better than the TI ADS1299.

Since the gain will greater than 5, it makes sense to evaluate the MAX40079 and the MAX40089, even though the bandwidth will be under 100Hz. Thank you for making the MAX40089 spice model work.

-Morty

PS: It would be helpful to be able ot insert files in this conversation.

I'm using version 17.1.11. In the past 1 -2 years, there have been too many changes that affect the results obtained from the simulations. I would be willing to try the newest version, but only if I could have both versions concurrently, re-install my current version. I am not sure which version of the installer is v17.1.11. Perhaps you could let me know.

I am now closing this thread as we are taking this issue offline.

-L