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.

Problem importing .lib to TINA-TI

Other Parts Discussed in Thread: TINA-TI


I'm attempting to create a New Macro for the ALD810027 located in 21XXYY.lib (attached). The PSPICE model looks fine and yet I'm obtaining this error:

Missing syntax element. Line: #7.


I couldn't find anything wrong with the model. Could someone help me out?

Best regards,

Sean Grech


  • Solved the problem (sort of):

    1) First issue was a simple error in the syntax, and is the problem referred to in my earlier post. There were normal brackets where there should have been curly brackets in the model definition at lines containing "tox=(...)". These should have read "tox={...}". Simple fix, shouldn't affect the model.

    2) Had a problem with some .subckt lines of code. "params: vtn=vtn" is not recognised by TINA as proper syntax either. I didn't need those sub-circuits in particular, so I simply put in a random number as follows "params: vtn=0.375V". Hope this doesn't affect the other sub-circuits.

    3) Third problem was that Model: DPS was not recognised by TINA. I'm not sure what this meant, but I have never seen in other PSPICE models anything similar to the last 5 lines of each sub-circuit, e.g. "dbv 4 5 dps 0.8e-8". I am assuming these 5 lines refer to the 5 outward connections made by each sub-circuit. I simply removed these lines, hoping it won't affect the model.

    Everything worked after these changes. If anyone can provide further insight into these issues, especially the second and third ones, feel free to post.


    Sean Grech

  • Sean,

    Actually, items 2 and 3 are quite important. In this case, you have a 5 terminal subcircuit for the device and when you remove the diodes from the subcircuit, pin 5 is not connected to anything. The parameter lines are fine in TINA-TI once you correct the parenthesis error. The VTX is not used, so you could remove it, but the other parameters are needed if you want the model to function correctly. the values are used in the calculations for the model parameters. The vtn is passed from the subcircuit to the model, so you don't need the vtx value.

    Here is what the subcircuit should look like:

    .subckt 810027 1 2 3 4 5 params: vtn=2.663V
    m1 1 2 3 4 NMOS l=4.8e-6 w=138e-6 as=0.603e-8 ps=0.478e-3 ad=0.161e-8
    +                       nrd=0.3 nrs=1 nrg=25 nrb=35
    .param vtx={vtn} cox=1.0 ires=0.41 pox=1.0 M=10
    + level=2
    + gamma=0.035
    + vto={vtn} 
    + Uo=650     
    + Ucrit=0.7e4 Uexp=.1 Vmax=1.6e5
    + phi=0.65 tpg=+1
    + nsub={1e16*ires} neff={10*ires} nss=0.7e11 nfs=4.4e11
    + tox={0.047u*cox}
    + Cgso={.94n*cox} Cgdo={.59n*cox} Cgbo={.138n*pox} Xqc=.42
    + cj=.39m cjsw=264p xj=1.0u
    + ld=0.8u
    + wd=1.05u
    + pb=.9 js=20e-6  mj=.5 mjsw=0.18
    + kf=.75e-28 rsh=10 )

    dbv 4 5 dps 0.8e-8
    dbd 4 1 dps 0.8e-8
    dbs 4 3 dps 0.8e-8
    dbg 4 2 dps 0.8e-8
    dgv 2 5 dps 0.8e-8

    .model dps D (Is=2.61e-7
    +             Isr=1.0e-5
    +             Bv=34 Ibv=1e+4
    +             Rs=2.74e-7 trs1=3e-3
    +             Cjo=1.3e-4 )


    I have removed the additional values for lot, dev, and uniform as those are not defined for use.

    I have imported the model into TINA-TI. Please see the attached .TSM file that can be used with the Insert-->Macro function.