multisim

[NavidG]

Hi All,

I am trying to import PA96 model into Multisim but once I try to simulate my circuit I get following spice error. Not sure how I can fix it

SPICE Netlist Error in schematic RefDes 'u1, u2', element 'dmos': Invalid parameter name ')'
SPICE Netlist Error in schematic RefDes 'u1, u2', element 'd3545': Invalid expression 'dmos'

Thanks

Navid

[jcham]

Hi Navid, 

If you are using the model from the Apex website here (https://www.apexanalog.com/support-3/), you need to remove the unmatched closing brace in the two DMOS .model statements: 

.MODEL DMOS NMOS LEVEL=3 VMAX=9E5 THETA=6E-3
+ ETA=2E-4 VTO=-1.53 KP=0.07 RS=2 RD=19) <---

I hope that helps. 

Jeff

National Instruments

[NavidG]

Hi Jeff

I did remove the unmatched ) in both dmos model parts but still I am facing same error:

------ Checking SPICE netlist for ultrasonic_phase_array_phase1_power_components - Monday, July 06, 2015, 1:43:28 PM ------
SPICE Netlist Error, element 'p2450': Redefinition of subckt 'p2450'. Second definition ignored.
SPICE Netlist Error, element 'dmos:p2450': Invalid parameter name ')'
SPICE Netlist Error, element 'p2450': Invalid expression 'dmos'
SPICE Netlist Error in schematic RefDes 'u2', element 'xu2': Unable to interpret 'vcc'
======= SPICE Netlist check completed, 4 error(s), 0 warning(s) =======

Thanks

Navid

[jcham]

What version of Multisim are you using? Could you attach the model data and / or your Multisim design file so I can take a closer look?

Thanks,

Jeff 

National Instruments

[NavidG]

I am using version 13 Education Edition. I have attahced the Apex Power Amp model file with the fix I did for the unmatched paranthesis. I have also attatched my design file.

Thanks

Navid

[jcham]

The model you are using has two "child" .subckt statements (P2450 and D3545), these need to be encapsulated by the top-level .subckt (PA96). If you move the PA96 .ends statement (".ends PA96") to the end of the entire model, you should be able to simulate correctly. 

Let me know if you need any more help. 

Jeff

National Instruments

[NavidG]

Hi Jeff,

I don't know why I still get the same errors ( copied below). I again attached my model file and my design file. Please note I did all your fixes.

------ Checking SPICE netlist for ultrasonic_phase_array_phase1_power_components - Tuesday, July 07, 2015, 11:42:46 AM ------
SPICE Netlist Error, element 'dmos:p2450': Invalid parameter name ')'
SPICE Netlist Error, element 'p2450': Invalid expression 'dmos'
SPICE Netlist Error, element 'm1:p2450': Unable to interpret 'dmos'
SPICE Netlist Error, element 'p2450': Due to errors, the component 'm1' will be omitted from the simulation
SPICE Netlist Error in schematic RefDes 'u2', element 'xu2': Unable to interpret 'vcc'
======= SPICE Netlist check completed, 5 error(s), 0 warning(s) =======

[jcham]

Hi Navid,

It seems that the file you sent is still using different models for U1 and U2. In U2, there is still problems with an unmatched .ends statement and brackets in the second DMOS .model statement. 

I was able to get ride of the errors by editing the model for U2 and moving the first .ENDS statement to the very end of the model and fixing the unmatched bracket on:

.MODEL DMOS PMOS LEVEL=3 VMAX=9E5 THETA=60E-3
+ ETA=2E-3 VTO=-2 KP=0.07 RS=3 RD=10)

Jeff

National Instruments

[NavidG]

Hi Jeff,

When I open U1 and U2 they have same models and same files. Can You please send me your design and model file?

Thanks

Navid

[jcham]

Here is the working version of your circuit. Note it is not complete, but no longer runs into the simulation errors. 

I created this by saving component U1 to my user database and then replacing U2 with the saved version of the PA96 from my user database. 

Jeff

National Instruments