Cadence入門（一）畫出漏電流和源漏電壓之間的關係

寫在前面的話：這篇講Cadence的入門。請各位牛人們不要浪費時間看這篇了哈！

作者君意識到，相當多的讀者是本科的小同學們。因此，作者君覺得不能只是一直講具體的電路設計，還應該照顧到入門的同學們。

這一篇來自於作者君做TA時候的所用課件。（這是master的一個上機lab課程的課件，作者君做了三年TA。從Cadence的使用開始，一直到設計出一個完整的wide-band amplifier，包括biasing電路和最終的layout。這門課還是很comprehensive的哈！話說兩個星期的lab課程之後，大家紛紛表示以後要做analog designer……）

這位師兄的英文還挺好懂的，作者君就不一一翻譯了，大家就當做四六級閱讀了哈！不管怎麼說，所有的IC design的EDA tools都是英文的，早些多接觸一下英文並沒有壞處。再說了，那些很經典的paper，基本上都是英文的。大家還是別抵觸英文了哈！

學習模擬電路設計，作者君非常非常建議大家裝個基本版的virtuso，不要什麼6XXX那些高級版本，古老的5141就可以了。然後工藝庫用多古老的都行。下面這個例子就是用的0.5um的工藝……老到……可能還有些做DCDC的公司在用？反正只要device的model都還齊全就行了！

具體到不同的process，大家看到的有些界面可能會略微有些不同。但是別擔心，基本上的流程就是這樣的，只要能跑一個模擬，想必大家就會放心很多啦！

除此之外，大家還應該了解一些基本的Linux命令，因為基本上所有的EDA都是運行在Linux下面的。

Welcometo Analog Design Lab! I am pleased that you have chosen thiscourse. I will be accompanying you for the next ten days. Let"s embark on a fun& enriching journey ahead.

Exercise1A: Plot of Drain Current with Drain-to-Source Voltage

1. Enter your User Name and Passwordand you will get the screen below:

2. Rightclick on the Mouse and Click Open Terminal. You will get the screenbelow:

4. Type source cshrc.amis05, pressEnter and your screen will look like:

（這個source文件的功能是導入一些配置文件，比如環境變數之類的。其實如果IT的人給力的話，這一步其實是不用的）

5. Type icfb&, press Enterand your screen will look like:（icfb是較老版本的Cadence下面啟動virtuoso的命令，如果版本是6XX，就應該敲virtuoso &）

6. Click on Tools, and then LibraryManager and your screen will look like:

7. Click on File, New and Library. Your screen will look like:

8. Under Name, type Analog_Is_Fun_Lab_Exercises, press Ok and your screen will look like:

9. Click Attach to an existing techfile, press OK. Make sure that the Technology Library is amis500cxakxx and the screenwill look like shown below. Press OK.（鏈接工藝庫。你的可能叫「smicXXX」，前面的字母一般就是foundry名）

10. You will get to see that you hadcreated a new library - Analog_Is_Fun_Lab_Exercises:

11. Click on File, New and then Cell View. Your screen is shown:

12. Under Cell Name, type Lab_1a_NMOS. Your screen is shown:

13. Press OK. Your screen should show:

14. Now you are in the schematic windowand ready to draw your schematic. Press iand an Add Instance window will pop uplike shown below.

15. Click Browse. Select as shown below and a NMOS symbol will be attached toyour mouse. Take note: enm is the name of a NMOS transistor.

16. Click on your left mouse once to place the NMOS symbol in the schematic window. Press Esc to remove the symbol from your mouse after placing it once inthe window.

17. Press i again, click on Browse and choose as shown below. A DCvoltage source will be attached to your mouse.

18. Clickon your left mouse to place it inyour schematic window. Move your mouse and left click again to place the second symbol. The final screen is shownbelow. Press Esc.

19. Press i again, click on Browse. In the AnalogLib, look for gndsymbol and place it in your schematic. It is a HAPPY test. Do try it yourself. I amsure you can do it. Your final screen should look like this below. Press [ to zoom out and ] tozoom in.

（鍵盤上的中括弧鍵，就是字幕P旁邊的兩個，是放大和縮小的快捷鍵）

20. Excellent!You had finished the whole schematic. Now, let"s continue with the wiring connections. Press wand left click once on the redsquare of the gnd symbol. Move the mouse towards the red square of thesource of the NMOS symbol. Left clickagain. You can see that a wire connection isformed. Try the other wiring yourself. Do not be upset if you cannot do it. Ask your teachingassistant. He will be happy to assist you! Your finalized schematic will look like this. PressShift and x together to save the schematic.

21.Now, we need to edit the properties (W/L ratio) of the NMOS. Press the Esc Button. Click on the NMOS symbol and it would be highlighted. Press q and then a window will pop up asshown below. Change the Finger width to3 and the Length to 1.

Take note: 3 and 1 will be treatedas 3um and 1um by the system respectively.

（一般的工藝下，後面都是帶了單位的，比如um之類的。這個古老的工藝有些骨骼精奇……）

22. Now, we need to edit the properties (DC Value) of the voltagesource(V0). Click on the V0 voltage source symbol and it would be highlighted. Press q and then a window will pop up as shown below. Change the DCvoltage to 1.2. （設置bias的Vgs電壓大小，必須保證比Vth大，否則下面的圖可能看不到）

23. Do the same for V1 voltage sourceand change the value to 3. The finalschematic should look like this. Press Shiftand x together to save this schematic.

24. Now, we are ready for the simulation. Are you ready? Click on Tools,then Analog Environment.A new window will pop-up as shown below.

25. Click Setup, then Model Libraries. Under Model LibraryFile, type this: /net/wildar/software2/local/library/AMIS/AMIS05_CDS/MSD_PDK/lib/amis500cx/tech/ spectre/amis500cxakxx/Rev2.20/res-Default.scs. Type typ under Section. Afterwhich, press Add. Your screen shouldlook like this:（設置model的process corner，一般有typ，也就是typical，還有slow，fast，fs，就是fast-slow，和sf，一共五種。基於不同的process，可能還會有別的corner，名字也有可能不一樣。如果你夠幸運的話，這一步其實是不用手動加library的，可能已經被embedded進去了）

26. Repeatthe same for the other 5 model files:cap, bip, dio, var and mos. It is a simple enjoyable test. Do try it yourself.Ask for help if you encounter any problems. Do not be shy. You will get thescreen as shown below. Press OK. （你也有可能不用這樣做，很多process默認加入了所有的device models）

27. In the AnalogDesign Environment window, press Setup,then Simulator, change the Project Directory to /tmp. It is shown below. Press OK.（告訴tool，你想把模擬結果保存在哪裡。tmp是Linux下的臨時文件夾，你也可以放在自己想放的任何地方，比如: /home/johnyy/simulation_results/nmos_test/）

28.In the Analog Design Environmentwindow, press Analyses, then Choose. We want to run a DC simulation to sweep the drain tosource voltage from 0V to 3V. Thus, it has to be filled up like the screen below. Press OK.（準備sweep那個mos的Vds值，設置了範圍，用DC，也就是直流穩態模擬）

29.In the Analog Design Environmentwindow, you should get the screen as shown:

30.In the Analog Design Environmentwindow, press Outputs, To be plotted and Select on Schematic.Click on the red square at the bottom of V1 voltage source. After clicking on it, agreen oval will surround the red square as shown below. This is so that the output result would be current. Overall, the graph plotted would be Id Vs Vds.（你也可以點擊Results，然後direct plot，然後選擇DC，再在schematic裡面點擊你想看的電壓線或是電流節點）

31.In the Analog Design Environmentwindow, it should be as shown below. Click on the Netlistand Run button as shown by the arrow below:（為了避免每次都要在schematic裡面選擇，你可以按Outputs，然後下面有to be plot，一次選好，下次跑simulation，結束之後，waveform就會自己彈出來）

32.After 5 seconds, a graph of Id Vs Vds would appear and will look like the graphbelow. If you get it, Congratulations! If you cannot get it, please do not despair. Youjust have to work harder at it. Look at the bright sideof life.

這張圖就是Id和Vds的關係，跟Razavi第二章裡面的那個圖是一樣的。

33.Now, we are going to get a family of curves by running a parametric simulation. It is to sweep the V0 voltage values and a family ofcurves will emerge. Click on V0 voltage source and press q. Change the DC voltage to parameter. Press OK. In the schematic window, press Shift and x together to save it. （說實話，parameter這種名字其實不直接，作者君建議叫Vds_set之類的名字，簡單直接。注意：名字里別用空格）

34.In the Analog Design Environmentwindow, click Variables, then Edit. Key in the information shown below. The maximum valueof V0 is 2V. Press Add and OK.

35.In the Analog Design Environmentwindow, it should be as shown below.

36.In the Analog Design Environmentwindow, click Tools, then Parametric Analyses. The pop-up window is shown below. Fill inthe information as shown below. It sweeps V0 from 1V to 2V in a total of 6 steps.

37.In the Parametric Analyses window,click Analysis, then Start. The family of curves are shown below.

這一系列的圖，每個代表了不同的Vgs下，Id和Vds之間的關係。很顯然，Vgs越大，這個mos能夠運輸的電流也更大，符合大家的估計哈！

Congratulations!I am so proud of you. You had obtained the family of curves for drain current plottedwith drain-to-source voltage. Look at the curves. They are GREAT!

Do remember that parametric simulation is a very important step in circuitsimulation as it saves a lot of time and effort as compared to simulating eachcomponent parameter separately. Check with your teaching assistant if you stillhave any doubts or queries with regard to any of the simulation steps above. He is a very nice and helpful person.No worries.

———————————————————————————————————————

原創聲明：本文為原創，未經許可，嚴禁轉載。如需轉載，請聯繫作者。

微信公眾號：analogIC_gossip