旗艦軟體

線上影音

Home > ANSYS Simplorer教學  > Simplorer links Pspice

 

本文始於2018.08，以R19.1示範如何在Simplorer內使用Pspice models. 只要您可使用R19.1 HFSS\Q3D\SIwave\Maxwell，即可操作本文介紹功能，不需要額外的Twin Builder license.

  1. What SPICE model does simplorer support?

  2. Pspice Hands-on

  3. Q&A

    3.1 Is there another way to import SPICE?

    3.2 How to do troubleshooting for importing Pspice fail?

  4. Reference

  1. What SPICE model does simplorer support?  

Simplorer supports Pspice and Berkeley (3f5) Spice, NOT HSPICE, LTspice, SIMetrix...etc.  (Even some of them work with Simplorer after a bit of modification)

  1. Pspice Hands-on 

2.1 [Tools] \ [Options] \ [General options], select [Spice compiler]

[Spice Text as] select the Spice syntax for Spice Model Editor.

2.2 [Tools] \ [Project Tools] \ [Import Simplorer Models]

Simplorer supports .lib, NOT .olb library format. The .olb file is the component library containing the schematic symbols. It does not contain model text.

2.3 Drag and drop LM7805 from [Components] to schematic window

2.4 Right-button mouse on the LM7805 symbol, select [Edit Model] to view the spice model and pin definition

.SUBCKT LM7805 1 2 3
* In GND Out

2.5 LM7805 and 7812 LDO waveform

It is easy for users to find some regulators in Simplorer component library, but unfortunately there is not the most popular LDO 78xx series. That is why this article appears here.

  1. Q&A

    2. 3.1 Is there another way to import SPICE?

    Ans：[Twin Builder] \ [Add Model] , and 2021R2 has a new import icon as below

    3.2 How to do troubleshooting for importing Pspice fail? 

    Ans：

    -- Confirm the imported model is Pspice, not HSPICE, LTspice, SIMetrix or an encrypted one.

    -- It is .lib, not .olb which is the component library containing the schematic symbols.

    -- For TABLE syntax, remove "=" between TABLE and {}, then Simplorer can import it well

    -- Whether a "global" parameter (as af below) that has been claimed to pass to a sub-circuit, but not defined there.

    Simplorer import it fail

    Simplorer import it well

    .subckt Cxxx d g s Tj Tc
    .param af1=1
    xgmos d1 g1 s1 Tj Tc gmos params: af=af1

      ...

    .ends Cxxx
    *****************************************
    .subckt gmos d1 g2 s1 Tj Tc
      ...

    .ends gmos

    .subckt Cxxx d g s Tj Tc
    .param af1=1
    xgmos d1 g1 s1 Tj Tc gmos params: af=af1

      ...

    .ends Cxxx
    *****************************************
    .subckt gmos d1 g2 s1 Tj Tc params: af=1
      ...

    .ends gmos

    -- add "=" for parameters assigment of the GaN PSPICE (TPH3206), as the below show

    -- way1 : move the definition of .model into the definition of .subckt for the Wolfspeed SiC LTspice

    -- way2 : modify "-" to "_" , and then import Wolfspeed SiC LTspice well

  2. Reference

    [1] GaN PSPICE (TPH3206/3208)