• State TI Thinks Resolved
  • Locked Locked
  • Replies 6 replies
  • Answers 2 answers
  • Subscribers 65 subscribers
  • Views 2769 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.

PSPICE-FOR-TI: WARNING(ORPSIM-16534): Using high values of ITL4 for Speed Level > 0 may increase total simulation job time.

Ihzany Vilia Devi
Prodigy 215 points
Part Number: PSPICE-FOR-TI
Other Parts Discussed in Thread: LMR33630, TINA-TI

Hi i would like to know how to make this running simulation time more fast? 

because i need to see the result fast, but on the contrary the load result is too slow. 

Please tell me the reason what makes the running simulation to run slow? Thank you 

lmr33630_test standard-2023-01-17T01-01.zip

  • 0
    TI__Expert 5880 points

    Hi Ihzany,

    Please allow me some time to look into your design. Is this identical to the reference design provided with LMR33630?

    Thank you,

    Jackie

  • 0 in reply to Jackie Horn
    Prodigy 215 points

    Yes! only change the value of the resistor 

    but when doing the simulation for 10ms it takes for 1 hour 

    and my senior got angry why PSpice for TI takes too long to simulate compare than TINA-TI

    Please resolve this problem as fast as possible

    And please give solution to the other issue that still not resolved, Thank you !

  • 0 in reply to Ihzany Vilia Devi
    TI__Expert 5880 points

    Hi Ihzany,

    I notice there are some custom sim profile settings that are slowing down your simulation:

    • Analysis tab: 0.4 seconds is excessively long for the simulation time. Please use something on the order of milliseconds. Longer sim times will inherently take longer.
    • Analysis tab: You have maximum step size set to 80ms, which is very large. This is unrealistic because the switching frequency appears to be about 1MHz. The original sim is set to 20ns, but that is not required. Please just leave this field blank and the simulator will set an appropriate value internally.
    • Options tab: Under Analog Simulation -> General, the ITL1, ITL2, and ITL4 have been changed from the defaults. Please reset to the default values (listed in right most column)
    • TINA-TI is a "faster" simulator because it is less accurate. You can modify the accuracy settings in PSpice for TI if desired. However, be aware that you may see slightly different results. I changed VNTOL to 100u, and ABSTOL to 100n. (See above image) Because you are working with high voltages and currents, loosening of these values should not be an issue.

    These settings should be used for the reference design, or any design based off of it.

    I will pass this thread to the product line to check your setup and provide any insight on the model. 

    Thank you,

    Jackie

  • 0 in reply to Jackie Horn
    Prodigy 215 points

    Hi Jackie, 

    I'll respond regarding your aswer :

    1. Analysis tab: 0.4 seconds is excessively long for the simulation time. Please use something on the order of milliseconds. Longer sim times will inherently take longer. (How can i change it to the miliseconds? because i do the simulation based on the ISO Standard from the automaker so it cannot be changed)

    2. Analysis tab: You have maximum step size set to 80ms, which is very large. This is unrealistic because the switching frequency appears to be about 1MHz. The original sim is set to 20ns, but that is not required. Please just leave this field blank and the simulator will set an appropriate value internally. (Ok, but this still not resolved my question)

    3. Options tab: Under Analog Simulation -> General, the ITL1, ITL2, and ITL4 have been changed from the defaults. Please reset to the default values (listed in right most column) (I changed it because it needs to resolved the problem ORPSIM) 

    4. TINA-TI is a "faster" simulator because it is less accurate. You can modify the accuracy settings in PSpice for TI if desired. However, be aware that you may see slightly different results. I changed VNTOL to 100u, and ABSTOL to 100n. (See above image) Because you are working with high voltages and currents, loosening of these values should not be an issue. (Is less accurate but we can do the test more fast and when we did a design verification, calculation, and simulation the result it's not too far but it's working more "FAST" and we can work until 50Second without running too slow! and we can use TINA-TI BASED ON THE ISO STANDARD, so please help me to answer this question why it cannot work on 0.4 second? it really takes too long. and if you said because it works more accurate we cannot accept that kind of answer, Thank you) 

  • 0 in reply to Ihzany Vilia Devi
    TI__Mastermind 22260 points

    Hello,

    Thank you for your patience. We will try to respond to your questions as soon as possible. 

    Best regards,

    Ridge

  • 0 in reply to Ihzany Vilia Devi
    TI__Mastermind 22260 points

    Hello,

    TINA-TI and PSPICE for TI have very different simulation engines that solve the circuit. TINA-TI is “fast” because it cuts corners. While many users look for a “fast” solution with no issues, the shortcuts that TINA-TI takes can sometimes lead to inaccuracies. Many of the models in the TI library are idealized, including discontinuities or sharp transitions. TINA-TI may handle these well due to its shortcuts, but will result in less accuracy. PSPICE for TI does not take as many shortcuts, but this does not mean that PSPICE for TI is not optimized. PSPICE for TI is optimized for more realistic models. For example, an ideal step function may be handled better in TINA-TI than PSPICE for TI. However, complex and continuous models are well optimized in PSPICE for TI. The request for a “fast” simulation of 0.4 seconds is not possible. The datasheet for your device shows that the minimum frequency is 400kHz. Based in the Nyquist rate, PSPICE for TI will require at least 320,000 times steps to run the simulation.

    Best regards,

    Ridge