Integrated Circuit Design
Would you like to react to this message? Create an account in a few clicks or log in to continue.


Integrated Circuit Design exposes students to the design and fabrication aspects of ingrated circuits. Also provides knowledge on how digital electronic system can be produced on tiny semiconductor materials. This forum also focuses on the production of i
 
HomeLatest imagesSearchRegisterLog in

 

 Macam mana nk import .spc files ke Pspice

Go down 
2 posters
AuthorMessage
auna




Posts : 1
Join date : 2010-04-13

Macam mana nk  import .spc files ke Pspice Empty
PostSubject: Macam mana nk import .spc files ke Pspice   Macam mana nk  import .spc files ke Pspice I_icon_minitimeWed Apr 14, 2010 12:06 am

Salam,

saya tidak tahu bagaimana untuk membuat simulation bg layout yg telah dibuat di L-Edit. Tolong.... Very Happy
Back to top Go down
Admin
Admin



Posts : 2
Join date : 2010-04-13

Macam mana nk  import .spc files ke Pspice Empty
PostSubject: SPICE   Macam mana nk  import .spc files ke Pspice I_icon_minitimeWed Apr 14, 2010 12:36 am

Terima Kasih diatas pertanyaan anda

Ia adalah simple utk membina simulation file from the mask-level design yg telah anda create dalam L-Edit untuk diuji dalam PSPICE. Once bila anda dah selesai dengan design anda di L-EDIT (tiada error - design rules check). anda perlu ke tab tools dan pilih extract.

Ketika ini satu window akan muncul dan meminta extract definition file (morbn20.ext) dan destinasi. Fail yg dibina ini akan disimpan sbg .spc.

Macam mana nk  import .spc files ke Pspice 111

Macam mana nk  import .spc files ke Pspice 210
The extraction may take a few seconds depending on the size of the design. More windows may appear concerning
zero capacitance conditions, but notice that these warnings appear concerning mask materials that were not used in the design. Just click the OK button as it comes up.

When the extraction is complete, the program should tell you that the extract was successful. The next step is to open the .spc file that was created in a program such as Notepad. There will be many lines of information including transistor designations and information in addition to parasitic capacitances.

To this file it is necessary to add some items. First, a power source (for the p-MOSFETS, usually 5 volts) must be inserted. You must also ensure that ground is denoted by the number 0 rather than another name (e.g. Gnd-PSPICE will only interpret node 0 as ground). The transistors need to be characterized by a set of model statements that you can get from web (tak pun ada sesetengah pensyarah yg sediakan model statements ni...so copy paste jer...tak perlu nk taip nanti takut error plak).

Finally, supply input signals for functionality testing. You may also want to add .probe and/or .tran commands for graphing and numerical tracing abilities. Once the file has been prepared for PSPICE, save it as a .cir file. It will then be ready to test using PSPICE. As you know, PSPICE will send out warnings and halt simulation if there are problems with your file.

Ini contoh untuk satu fail yg berjaya digenerate melalui LEDIT dan berjaya di'simulate' usind SPICE.

* Circuit Extracted by Tanner Research's L-Edit V7.12 / Extract V4.00 ;
* TDB File: C:\Documents and Settings\Winda\Desktop\LAB_E5163\INVERTER, Cell: INVERTER
* Extract Definition File: C:\Documents and Settings\Winda\My Documents\L-Edit Student v7.12\mosis\morbn20.ext
* Extract Date and Time: 01/13/2010 - 10:55

* NODE NAME ALIASES
* 1 = VDD (20,47)
* 2 = VSS (23,-16)
* 3 = OUTPUT (34.5,13)
* 4 = INPUT (7.5,13)

M5 OUTPUT INPUT VDD VDD PMOS L=2u W=11u AD=66p PD=34u AS=55p PS=32u
* M5 DRAIN GATE SOURCE BULK (23 26 34 28)
M6 VSS INPUT OUTPUT VSS NMOS L=2u W=10u AD=70p PD=34u AS=60p PS=32u
* M6 DRAIN GATE SOURCE BULK (23 0 33 2)

*MENYATAKAN GELOMBANG MASUKAN
VVDD VDD 0 5
VVSS VSS 0 0

*MENYATAKAN GELOMBANG VOLTAN MASUKAN
VIN INPUT VSS pulse (5 0 0 1n 1n 0.5u 1u)

*SURUH PSPICE BUAT ANALISIS TRANSIENT SETIAP 2ns DARI 0 HINGGA 8us
.tran 2n 8u
.probe

* THESE ARE TYPICAL SCNA SPICE LEVEL 2 PARAMETERS
.MODEL NMOS NMOS LEVEL=2 LD=0.250000U TOX=417.000008E-10
+ NSUB=6.108619E+14 VTO=0.825008 KP=4.919000E-05 GAMMA=0.172
+ PHI=0.6 UO=594 UEXP=6.682275E-02 UCRIT=5000
+ DELTA=5.08308 VMAX=65547.3 XJ=0.250000U LAMBDA=6.636197E-03
+ NFS=1.98E+11 NEFF=1 NSS=1.000000E+10 TPG=1.000000
+ RSH=32.740000 CGDO=3.105345E-10 CGSO=3.105345E-10 CGBO=3.848530E-10
+ CJ=9.494900E-05 MJ=0.847099 CJSW=4.410100E-10 MJSW=0.334060 PB=0.800000
* Weff = Wdrawn - Delta_W
* The suggested Delta_W is -0.25 um
.MODEL PMOS PMOS LEVEL=2 LD=0.227236U TOX=417.000008E-10
+ NSUB=1.056124E+16 VTO=-0.937048 KP=1.731000E-05 GAMMA=0.715
+ PHI=0.6 UO=209 UEXP=0.233831 UCRIT=47509.9
+ DELTA=1.07179 VMAX=100000 XJ=0.250000U LAMBDA=4.391428E-02
+ NFS=3.27E+11 NEFF=1.001 NSS=1.000000E+10 TPG=-1.000000
+ RSH=72.960000 CGDO=2.822585E-10 CGSO=2.822585E-10 CGBO=5.292375E-10
+ CJ=3.224200E-04 MJ=0.584956 CJSW=2.979100E-10 MJSW=0.310807 PB=0.800000
* Weff = Wdrawn - Delta_W
* The suggested Delta_W is -1.14 um_

Cpar1 VDD 0 30.708f
Cpar2 VSS 0 28.035f
Cpar3 OUTPUT 0 31.582f
Cpar4 INPUT 0 9E-016

* Total Nodes: 4
* Total Elements: 8
* Extract Elapsed Time: 0 seconds
.END


Jadi buka fail ni di SPICE A/D. Klik RUN dan akan keluar satu paparan hitam. Disini anda perlu add plot to window dan add trace.
Semoga berjaya
Back to top Go down
https://icdesigne5163.forumotion.com
 
Macam mana nk import .spc files ke Pspice
Back to top 
Page 1 of 1
 Similar topics
-
» Kids jordan import more young blood as high-rise Provision

Permissions in this forum:You cannot reply to topics in this forum
Integrated Circuit Design :: L-EDIT :: L-EDIT-
Jump to: