在线咨询
eetop公众号 创芯大讲堂 创芯人才网
切换到宽版

EETOP 创芯网论坛 (原名:电子顶级开发网)

手机号码,快捷登录

手机号码,快捷登录

找回密码

  登录   注册  

快捷导航
搜帖子
查看: 2692|回复: 4

[转贴] [转]Cadence to Matlab Tutorial

[复制链接]
发表于 2012-9-23 20:03:08 | 显示全部楼层 |阅读模式

马上注册,结交更多好友,享用更多功能,让你轻松玩转社区。

您需要 登录 才可以下载或查看,没有账号?注册

x
【经常需要转数据的朋友可以借鉴一下,写成脚本非常方便】

This file describes the process of outputting data from Cadence to Matlab.  First, the data from Cadence must be written to a file.  Then, Matlab can import the data from the written file.  This tutorial assumes the user is comfortable with Cadence and Matlab.



Step 1:

Set up your Cadence schematic and simulation.  Prepare the analyses as you normally would.



Step 2:

In the Cadence Analog Design Environment Window, select Sessions -> Save Script

Save and name the script to what ever name you desire.



Step 3:

The script will now open in a text editor.  Here is an example of what you might see:



simulator( 'spectre )

design(   "/auto/fsc/apg7/cadence/simulation/exp3/spectre/schematic/netlist/netlist")

resultsDir( "/auto/fsc/apg7/cadence/simulation/exp3/spectre/schematic" )

modelFile(

    '("/ee2/Cadence/NCSU/local/models/spectre/standalone/tsmc25N.m" "")

)

analysis('tran ?stop "60m"  )

desVar(    "RI" 10K         )

desVar(    "RF" 40K         )



temp( 27 )

run()



The file contains all of the information required to run your simulation.  It lists the simulator, design directory, required model files, analyses (can have more than 1), design variables, etc.  The 'run()' command is the command that actually runs the simulation.



In order to write data to a file, one has to create the file first. After the simulation is complete, some commands must be included in the script to retrieve the results before they can be printed to the file.  Then, they can be printed to the file.  The example below is the same example as above, but with the added commands to print the data to the output file 'paramResults.out':



simulator( 'spectre )

design(   "/auto/fsc/apg7/cadence/simulation/exp3/spectre/schematic/netlist/netlist")

resultsDir( "/auto/fsc/apg7/cadence/simulation/exp3/spectre/schematic" )

modelFile(

    '("/ee2/Cadence/NCSU/local/models/spectre/standalone/tsmc25N.m" "")

)

analysis('tran ?stop "60m"  )

desVar(    "RI" 10K         )

desVar(    "RF" 40K         )



temp( 27 )

out = outfile("./paramResults.out" "w")  ; name the output file and open it for write access

run()                                                        ; run the file

results()                                                 ; open up the results

selectResults(`tran)                                            ; Select the transient results

outputs()                                                               ; View the outputs

;Below, voltage measurements of VOUT_tran node are found at time points 0 to

;50 msec by increments of 1 msec.

for(tt 1 51

    time = tt*0.001 - 1*0.001

    fprintf(out "%5.3f    " time)    ; Print the time stamp

    fprintf(out "%1.6e \n" value(VT("/VOUT_tran"),time))                ; Print the voltage associate with the time

  stamp

)



close(out)



Step 4:

Once your script is ready, save it.  Then, from the Command Interpreter Window (CIW - the main window), type:



load("filename")



If your script has been saved in another directory, make sure you list the whole path between the quotes in the load command.  The script listed in the example above was named 'oceanScript.ocn' and saved in the cadence root directory.  In that case, you would type:



load("oceanScript.ocn")



This command runs your script.  Now your output data file has been created.



Step 5:

Start Matlab, and copy your output data file to your work directory in Matlab.  To retrieve the data from the output file, a Matlab script was written:



%Example for retrieval of paramResults.out data.



clear



filename = 'paramResults.out';

fid = fopen(filename,'r');



Z = fscanf(fid,'%g %g',[2 inf])';

t = Z(:,1);

y = Z(:,2);



fclose(fid);





The above script will have to be modified for different cases, such as having more data.  In this case though, we need to retrieve the time and voltage and put them in time vector 't' and the voltage vector 'y', respectively.  Any Matlab post-processing can be executed on the retrieved data once it has been imported, using the above script, into Matlab.
发表于 2012-11-17 16:25:47 | 显示全部楼层
HAHA,已看
发表于 2012-12-13 21:14:38 | 显示全部楼层
看看了额
发表于 2012-12-13 21:19:34 | 显示全部楼层
I thinks it is pretty good!
发表于 2013-1-13 11:56:28 | 显示全部楼层
好东西   看看
您需要登录后才可以回帖 登录 | 注册

本版积分规则

关闭

站长推荐 上一条 /2 下一条


小黑屋| 手机版| 关于我们| 联系我们| 在线咨询| 隐私声明| EETOP 创芯网
( 京ICP备:10050787号 京公网安备:11010502037710 )

GMT+8, 2024-11-24 17:51 , Processed in 0.024791 second(s), 8 queries , Gzip On, Redis On.

eetop公众号 创芯大讲堂 创芯人才网
快速回复 返回顶部 返回列表