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.

TLV9052

Other Parts Discussed in Thread: TLV9052, TLV9102, TINA-TI

I use Orcad Pspice i have down loaded TLV9052.cir and have tried to make a part and use the orcad tools as suggested by  a Ti app note SLOA070 i get this error in Orcad when I try to use it in a design

INFO(ORPROBE-3183): Simulation running...
** Profile: "SCHEMATIC1-test1" [ X:\prerel\Gregg\SPICE_test\spice1\spice_test-1-PSpiceFiles\SCHEMATIC1\test1.sim ]
Reading and checking circuit
ERROR(ORPSIM-15108): Subcircuit VCCS_LIM_CLAW+_0 used by X_U10.XCLAWp is undefined
ERROR(ORPSIM-15108): Subcircuit VCCS_LIM_CLAW-_0 used by X_U10.XCLAWn is undefined
ERROR(ORPSIM-15108): Subcircuit VOS_DRIFT_0 used by X_U10.XU1 is undefined
ERROR(ORPSIM-15108): Subcircuit VCCS_LIM_2_0 used by X_U10.XVCCS_LIM_2 is undefined
ERROR(ORPSIM-15108): Subcircuit VOS_SRC_0 used by X_U10.XVOS_VCM is undefined
ERROR(ORPSIM-15108): Subcircuit VCCS_LIM_ZO_0 used by X_U10.XZo is undefined
ERROR(ORPSIM-15108): Subcircuit VNSE_0 used by X_U10.Xe_n is undefined
ERROR(ORPSIM-15108): Subcircuit FEMT_0 used by X_U10.Xi_nn is undefined
ERROR(ORPSIM-15108): Subcircuit FEMT_0 used by X_U10.Xi_np is undefined
ERROR(ORPSIM-15108): Subcircuit VCCS_LIM_1_0 used by X_U10.XVCCS_LIM_1 is undefined
ERROR(ORPSIM-15108): Subcircuit VCCS_LIMIT_IQ_0 used by X_U10.XIQp is undefined
ERROR(ORPSIM-15108): Subcircuit VCCS_LIMIT_IQ_0 used by X_U10.XIQn is undefined
ERROR(ORPSIM-15108): Subcircuit CLAMP_AMP_LO_0 used by X_U10.XCL_AMP is undefined
ERROR(ORPSIM-15108): Subcircuit CLAMP_AMP_HI_0 used by X_U10.XGR_AMP is undefined
ERROR(ORPSIM-15108): Subcircuit VCCS_LIM_GR_0 used by X_U10.XGR_SRC is undefined
ERROR(ORPSIM-15108): Subcircuit VCCS_LIM_4_0 used by X_U10.XCL_SRC is undefined
ERROR(ORPSIM-15108): Subcircuit CLAMP_AMP_LO_0 used by X_U10.XCLAW_AMP is undefined
ERROR(ORPSIM-15108): Subcircuit VCCS_LIM_3_0 used by X_U10.XCLAW_SRC is undefined
ERROR(ORPSIM-15108): Subcircuit OL_SENSE_0 used by X_U10.XOL_SENSE is undefined
ERROR(ORPSIM-15108): Subcircuit VCCS_EXT_LIM_0 used by X_U10.XVCM_CLAMP is undefined
Circuit has errors ... run aborted
See output file for details
INFO(ORPROBE-3188): Simulation aborted

any thoughts

I am using 17.420190latest build

have the same problem with TLV9102 

  • Former Member
    0 Former Member

    Hi Greg,

    Here's another customer that ran into the same issue with the TLV9102 and got very similar, if not the same, errors.  I would recommend reading through this first to see if this helps.

    Let us know if you need further assistance.

    Regards,

    Daniel

  • I read through the information but there was no answer i get it that the model is more complex but i can't switch to tina. they only say due to the complexity the can not use model import they do not explain there work around.

  • Former Member
    0 Former Member in reply to Gregg Granville

    Hello Gregg,

    Understood.  Then I'm assuming you followed this process from that thread as part of SLOA070:

    If you choose to use OrCAD, you need to first convert the PSpice .cir file to .lib, then you can create a symbol for this using the "Model Editor" tool. After that you should be able to add this symbol under library. The last step is to add the netlist .lib file to your simulation profile under "configuration files".

    The only other potentially useful information from that thread then is probably this, "Due to it is a complex model, we can't use 'model'->'import' in Model Editor."

    I've reached out to the engineer that was working on this thread to see if he can help here.  I'm expecting to have an update for you on Monday, at the latest.

    Regards,

    Daniel

  • as you can see i have already checked that

  • Former Member
    0 Former Member in reply to Gregg Granville

    Hi Gregg,

    Thanks for checking.  Let's see what Bala has to say regarding the matter.  He's dealt with this type of issue several times before.

    Regards,

    Daniel

  • Former Member
    0 Former Member in reply to Gregg Granville

    Gregg,

    Thanks for your patience.

    From Bala, "So the issue here is that our [latest] models have multiple subroutines in each model. These subroutines call each other and that’s how they are connected as a whole, somehow PSPICE recognizes the top level but not any other subroutines."

    This gives me a better understanding of what is probably the issue.  I'm still unsure as to how to solve it.  I'm now going to see if I can recreate the problem.  I'll get back to you here as soon as I have an update.

    Regards,

    Daniel

  • Former Member
    0 Former Member in reply to Gregg Granville

    Hi Gregg,

    Sorry for the delay.  I've had to get a different version of PSPICE and am now finishing the install.  Would you mind sharing your schematic?

    Regards,

    Daniel

  • Hi Dan 

    i got a response from cadence and they told me the problem is i can not import the CIR file they told me to just change the file extension to lib and that would work and it did but then i got another error saying i had to upgrade my version to the advanced version because basic has a limit of 250 devices. so your new models count as many devices because of all the sub-circuits. I am looking at using your software now. so the mystery is just rename the file to lib.

  • Former Member
    0 Former Member in reply to Gregg Granville

    Hi Gregg,

    Happy to hear the root cause has been determined, although it seems like you're still having issues.  I know our models are composed of sub-circuits to cover as many op amp parameters as possible.  But, I had not heard of someone having this issue before.

    If you'd like to try our software, I'd encourage you to do so.  One of the benefits of the software is that you don't have to mess with libraries and all that when working with new models.  Makes things more straightforward.

    Feel free to post again if you've got any questions.

    Regards,

    Daniel

  • one other question can i adda spice model for an LED fairly easily in your tool?

  • Former Member
    0 Former Member in reply to Gregg Granville

    Hello Gregg,

    Yes.  You should be able to do so without much issue.

    Download the file to your hard drive.  Then, open your TINA-TI software and go to Tools -> New Macro Wizard.  Then follow the prompts on the screen.  Let me know if you have any further questions.

    Regards,

    Daniel

  • Hi Daniel 

    trying TINA

    Getting an error when trying to use this diode 

    Syntax element: CAP|C|IND|RES|R|D|NPN|PNP|LPNP|NJF|PJF|NMOS|PMOS|VSWITCH|ISWITCH|SW|CSW|CORE|UGATE|UTGATE|UEFF|UGFF|TRN|VCO|SINE_VCO|TRI_VCO|SQUARE_VCO|AMPLI|AMPLI_GR|CNTN_UDSR|COMP|COMP_GR|COMP_GR_2INP|COMP_GR_3INP|COMP_GR_4INP|COMP_GR_NINP expected. Li

    tried attaching the file no go its a 

    https://my.centralsemi.com/product/partpage2.php?part=CMSH2-100M

  • Former Member
    0 Former Member in reply to Gregg Granville

    Hi Gregg,

    I used this method to attempt to import the file into TINA.

    I ran into the same problem as you did.  Then I tried importing a different diode model from the same site and it worked just fine.  The next idea was to compare the syntax of the two LIB files...and then I noticed there is a hyphen in the naming of the diode model.  I swapped this for an underscore and now everything seems to work fine.

    So, try going into the diode LIB file and changing the model name's hyphen to an underscore as shown below in line 25.

    Regards,

    Daniel