[請益] HSPICE問題..

[pinns (努力向上中...)]

小弟有兩個問題想請教各位高手...

1.以下是小地跑SPICE的時候 所出現的錯誤訊息..
  能否請高手指教一下,到底是什麼問題呢?
  是不是收斂的問題...因為剛開始跑沒多久  跑到一半 會當掉..
  lis檔如下..
_____________________________________
 **error**:  internal timestep too small in transient analysis

          time =  0.00000D+00;  delta =  3.72529E-19;  numnit =   112

 **warning** no convergence, invoking autoconvergence


          ***** job aborted

 **warning** autoconvergence is invoked!  trying method=gear from time=0
 ***autoconvergence sets default value of the options:
         method= gear           lvltim=  2
        mbypass=    1.00        bypass=    0.
          bytol=   50.00u     slopetol=  500.00m
           rmax=    2.00


 **diagnostic** dc convergence failure,
 resetting dcon option to 1 and retrying


 **diagnostic** dc convergence failure,
 resetting dcon option to 2 and retrying.

 no convergence with standard algorithm,  trying damped pseudo-transient

 **diagnostic** number of iteration exceeds min(7000, 20*itl1)=  4000 in pseudo
 tran process (converge=1 process). Usually this happens when the
 models are discontinous, or there are uninitialized bi-stable cells
 (flip-flop) in the circuit. By setting options dcon=-1 and converge=-1
 you can disable auto convergence process. Retry the run, non-convergence
 diagnostics will provide useful information about the nodes and devices
 which can be used to work around the non-convergence problems.

 no convergence in damped pseudo-transient,  trying gmath ramping method


 **diagnostic** op convergence successful with gmath ramping method


 **warning** This was a difficult operating point.
             You can speed up your simulation by specifying:
             .OPTION CONVERGE=4

  Opening plot unit= 79
 file=c:\flexlm\comp(dc).tr1
_________________________________________


問題2.
      小弟在跑比較器的電路 請問高手 怎麼跑出出 遲滯曲線呢??
      要使用.dc 還是.tran跑呢??
      怎麼跑呢 能否請高手指教 ...
 拜託了 請指教...

--
※ 發信站: 批踢踢實業坊(ptt.cc)
◆ From: 203.68.223.110
※ 編輯: pinns           來自: 203.68.223.110       (02/22 18:31)
推 akiottm:問題1:H-spice用它預設的init值去跑結果發散,請檢查電路,
→ akiottm:或照他說的去修改.opt設定或修改.tran的scale
→ akiottm:問題2:用.dc先掃最負到最正電位再.alter掃最正到最負,
→ akiottm:開avanwave把X-axis設定成V(in)就有hysteresis curve
※ pinns:轉錄至看板 comm_and_RF                                    02/22 20:04
→ pinns:多謝A大啦..我試試看..以後有問題還請你多提攜一點嚕
推 cpt:要不要試試看用 .ic 設定各端點的初始電壓, 會比較容易
→ cpt:converge
推 pinns:你是說用，.IC設定初始電壓比較不容易不收斂嗎?
→ akiottm:某些元件你已經大約可估計他工作在哪個電壓就可用.ic設定,
→ akiottm:例如將BJT的VBE初始值設定成0.7V(DC),讓元件直接active,
→ akiottm:若不知.ic如何下其實可將電源初始設定為0比較容易收斂,
→ akiottm:例如Vdd VDD gnd! pwl(0 0V 100us 'vdd')
→ pinns:恩 謝各位高手..我會試看看的..