求助：Hy8.0如何導出HSPICE MODEL

如題，小弟是Hy8.0的初學者，目前正學習如何使用hyperlynx仿真傳輸線模型，如附圖所示：

想請教高手們可否教教在下如何將我的模型導出成W-elemnet的netlist呢?
如果有詳解教學更是感激不盡阿
順便附上錯誤通知

已解決，不過只有一半，導出的W-element是lossless，為何在下的export spice netlist沒有其他選項?
附圖說明

為何要導出 SPICE net list 呢? HL8 不是可以調用 SPICE，直接跑就有結果了。

回樓上大大，因為在下主要使用的模擬軟體還是HSPICE，所以目前正在找尋生成W-element的方法。
小弟初學還不太熟悉軟體，不過定義了節點名稱以後就可以導出Netlist，但是如何生成有Loss的W-element還有請高手指教
----------------------------------------------------------------------------------------------------------------------------------------------------
附上Hyperlynx的說明書
Two Types of Netlist Output - Uncoupled and Coupled
The files generated by the HyperLynx SPICE writer come in two "flavors", depending on whether or not crosstalk is enabled in BoardSim/LineSim when you generate the netlist:
    Uncoupled, in which no coupling is modeled, and all transmission lines are modeled with the standard SPICE lossless "T" element
    Coupled, in which coupling is included and all coupled transmission lines are modeled with the HSPICE coupled, lossy "W" element
Specifically, the choice between uncoupled and coupled output is made automatically by the SPICE Writer, as follows:
    If you are running BoardSim, and you have crosstalk enabled, coupled output is generated; if crosstalk is disabled, uncoupled output is generated
    If you are running LineSim, and you have coupling anywhere in your schematic, coupled output is generated; if there is no coupling in your schematic, uncoupled output is generated
但是小弟目前找不到如何選擇coupled netlist output的方法
懇請大俠相救

1. ) 在建 LineSim sechematic 時，要點選 [ Enable Lossy Simulation] icon，就可以生成 W-Element。
例如：
****  Transmission line models ***********************
*********************************
* RLGC model created by HyperLynx SPICE generator
*
.MODEL Cond_000 W MODELTYPE=RLGC N=2
* Lo  (H/m)
+ Lo =
+ 4.86549e-007  
+ 1.22574e-007  4.86549e-007  
* Co  (F/m)
+ Co =
+ 7.31628e-011  
+ -1.29843e-011  7.31628e-011  
* Ro (Ohm/m)
+ Ro =
+ 6.59804  
+ 0  6.59804  
* Go (S/m)
+ Go =
+ 0  
+ 0  0  
* Rs (Ohm/m-sqrt(Hz))
+ Rs =
+ 0.0014215  
+ 8.16043e-005  0.0014215  
* Gd (S/m-Hz)
+ Gd =
+ 7.93923e-012  
+ -1.13036e-012  7.93923e-012  
*********************************
2.) 只要你在 LineSim 有設定 Couple pair, 那導出來的應該就是 Couple output netlist.
例：
* Output from HyperLynx SPICE Writer
* Created by K on Date: Sunday Sep. 4,2011   Time: 19:59:31
* Created with HyperLynx v8.1 build 509 (509, 0)
* Design file: UNNAMED0.TLN
* Special Settings: Coupled
3. ) 可以直接設定你的 HSPICE 的執行檔連結，在Interactive simulation 時選HSPICE，就可以直接調用
       HSPICE 來解題，不需要再管 Netlist 怎麼寫。

感謝這位大俠相助，小弟成功提取SPICE netlist了！
有您熱心助人真是我們的福音阿

各位神啊····怎样添加节点?

你那个导出来的SPICE  netlist在hspice中可以仿真吗、?可否给我教程下！