• State Resolved
  • Locked Locked
  • Replies 7 replies
  • Subscribers 37 subscribers
  • Views 3007 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

TINA-TI : spice model for SI7850DP mosfet

stephlaulau
Prodigy 220 points
Other Parts Discussed in Thread: TINA-TI

Hi,

I want to use simulation spice model SI7850DP.txt found on VISHAY web site. How can convert *txt file in a format understood by TINA-TI. I have tryed to do a macro but the simulation result seem to be not good.

Fullscreen 4682.si7850dp.txt Download 
*Feb 20, 2006
*Doc. ID: 76222, S-60244, Rev. B
*File Name: Si7850DP_PS.txt and Si7850DP_PS.lib
*This document is intended as a SPICE modeling guideline and does not
*constitute a commercial product data sheet.  Designers should refer to the
*appropriate data sheet of the same number for guaranteed specification
*limits.
.SUBCKT Si7850DP 4 1 2
M1  3 1 2 2 NMOS W=1611091u L=0.40u 
M2  2 1 2 4 PMOS W=1611091u L=0.62u 
R1  4 3     RTEMP 66E-4
CGS 1 2     520E-12
DBD 2 4     DBD
**************************************************************************
.MODEL  NMOS       NMOS  (LEVEL  = 3               TOX    = 7E-8
+ RS     = 88E-4          RD     = 0               NSUB   = 1.44E17  
+ KP     = 2.1E-5         UO     = 650             
+ VMAX   = 0              XJ     = 5E-7            KAPPA  = 7E-1
+ ETA    = 1E-4           TPG    = 1  
+ IS     = 0              LD     = 0                           
+ CGSO   = 0              CGDO   = 0               CGBO   = 0 
+ NFS    = 0.8E12         DELTA  = 0.1)
*************************************************************************
.MODEL  PMOS       PMOS (LEVEL   = 3               TOX    = 7E-8
+NSUB    = 2E16           TPG    = -1)   
*************************************************************************
.MODEL DBD D (CJO=500E-12     VJ=0.38    M=0.4
+RS=0.1 FC=0.5 IS=1E-12 TT=4.8E-8 N=1 BV=60.5)
*************************************************************************
.MODEL RTEMP RES (TC1=11.5E-3  TC2=5.5E-6)
*************************************************************************
.ENDS

4101.Docs.pdf

Is it possible to use *txt model file under TINA-TI ?

Concerning the Model file provided by VISHAY, is it correct ?

Best regards,

Laurent.

  • 0
    TI__Mastermind 41310 points

    Laurent,

    If you simply rename the subcircuit file to SI7850DP.cir, you can use the New Macro Wizard to create a .TSM file. Here the steps used:

    1.) Start TINA-TI v9

    2.) Use the New Macro Wizard Tools --> New Macro Wizard

    3.) Name the Macro SI7850DP and load the file. Click on Next.

    4.) Click the Show Suggested shapes only off and select Shape Type Field Effect Transistors. Choose the NMOSD symbol. Click Next

    5.) Associate the pins to the symbol, Pin 4 is the drain, Pin 1 is the gate, and pin 2 is the source. Click Next. Save the macro. Place it after you have saved it.

    You can test the device using voltage sources and sweeping VDS to see how it compares to the datasheet curves.

    I am attaching the .TSM file that I created.

    Britt

    6153.si7850dp.TSM

     

     

     

  • 0 in reply to Britt Brooks - Online Design Tools
    Prodigy 220 points

    Thanks Britt,

    If the mosfet spice model is good, then I have another problem with my simulation.

    First, I have done the simulation under switcher pro. I obtained the following result.

    7041.U82_48Vto12V_9A.pdf

    Second, I create schematics on TINA-TI in order to simulate transient response. See the following schematics and result

    1185.TPS40170_48Vto12V_6A.pdf

    We remark the following things :

    - under switcher pro, Vout=12V and Iout = 9A

    - under TINA-TI, Vout=0V and Iout = 0A. The power good doesn't increase.

    Could you help me to find errors under TINA-TI software ? I work on this design one week ago and I don't find where there are errors.

    Best regards,

    Laurent

  • 0 in reply to stephlaulau
    TI__Mastermind 41310 points

    Laurent,

    I do not believe that there are any errors in TINA-TI. I did find a solution for you based on the information provided.

    I have taken a look at your examples. I have used the SwitcherProTM example and created an equivalent TINA-TI schematic. I have attached it here for your reference.

    Please note that I have changed a few items from the SwitcherProTM schematic:

    1. The SS capacitor has been changed per the note in the schematic. A 47n SS capacitor would take approx. 30ms of simulation time (150minutes).
    2. The Input voltage is 46V. I have tested the test bench at 24V as well. Vout is 12V.
    3. I have changed the Load capacitor (C22) and Input capacitor (C1) values to those of the SwitcherProTM design. The X value is the number of capacitors in parallel in the subcircuit, just as shown in the SwitcherProTM schematic.
    4. The transistors have been changed to reflect the parameters of the SI7850DP, per its datasheet. I am not using the mfg provided model. I did not rename the devices from the reference design on the Web.

    Please note that I cannot debug or comment on the accuracy of the SI7850DP model from Vishay. The circuit does not function properly when adding these models, however, I did not try to tune the simulator parameters to see if the issue was simulation or model related.

    Britt

  • 0 in reply to Britt Brooks - Online Design Tools
    Prodigy 220 points

    Hi Britt,

    Thanks a lot for your answer. With your spice model for the Mosfet, the TINA-TI simulation runs.

    Just a last question, how could you find the parameter "switching point voltage Vsp" in mosfet datasheet ?

    Best regards,

    Laurent

  • 0 in reply to stephlaulau
    TI__Mastermind 41310 points

    Laurent,

    In this case, I used the max value of VGS(th). You could use a typical value (if one was specified), but in this case I used the max value. I also noticed that the current was very low when VGS was 3V in the ID vs. VDS curves. There were no plots below this value, so my assumption is that the device did not really start acting like a PowerFET until VGS was 3V.

    You may also change the RDSon value to a more appropriate value based on the conduction current.

    Britt

  • 0 in reply to Britt Brooks - Online Design Tools
    Prodigy 220 points

    Hi Britt,

    Thanks a lot for your answer and your availability.

    This request can be closed.

    Best regards.

    Laurent