[SOLVED] How to use rand_bit_stream for trasimpedance amplifier ?

[ultrasonic.1991]

hi i saw this thread https://www.edaboard.com/showthread.php?354967-How-to-used-VPRBS-for-trasimpedance-amplifier and i have a same problem but i use cadence 6.14 i know i should use rand_bit_stream from ahdllib for generating random bits but its a voltage source and i need current source i saw that someone said Use VCCS but i dont know how to use rand_bit_stream with vccs because rand steam has 1 output but vccs has 2 inputs . another thing that i saw in a thread here but it didn't help me is how to make 2^31-1 bits i thought it means that we should fo a transient simulation for 32767*period is that it?
thanks in advance .

 

[pancho_hideboo]

but i dont know how to use rand_bit_stream with vccs because rand steam has 1 output but vccs has 2 inputs .

The other input is connected to ground.

another thing that i saw in a thread here but it didn't help me is how to make 2^31-1 bits i thought it means that we should fo a transient simulation for 32767*period is that it?

Right.

I don't know what simulator you use.
However, if you use Cadence Spectre, Spectre Primitive, "isource with type=prbs" is available.

See "spectre -h isource".

 

[ultrasonic.1991]

i'm sorry i forgot to say i'm using cadence 6.14 . i used isource as you said it doesn't have a prbs type it has a bit type and i filled its parameters as in the picture that i attached . when i want to plot the input it says " expression evaluation failed: Expression evaluates to nil" **broken link removed** my speed is 10Gbps

 

[pancho_hideboo]

i'm sorry i forgot to say i'm using cadence 6.14 .

You can not understand tools you use at all.
This is a version of Design Framework.

i used isource as you said it doesn't have a prbs type

Simply GUI does not support this type for isource.
What version of Cadence Spectre do you use ?
Surely see "spectre -h isource".

it has a bit type
and i filled its parameters as in the picture that i attached .
when i want to plot the input
it says " expression evaluation failed:
Expression evaluates to nil"

I can not undesrstand what you want to mean at all.
Describe correctly.

Anyway what you want to do is no more than very easy thing for everyone.

 

[ultrasonic.1991]

You can not understand tools you use at all.
This is a version of Design Framework.
.

i don't get what you mean by version if its not 6.14 maybe you mean what technology i use its tsmc 0.13 um
what do you mean by spectre -h isource can you describe more please ?
i want to simulate eye diagram for my transimpedance amplifier . i saw in the papers that the input current they use for eye diagram in 10 Gbps is about 20um . i need a current supply that generates bits .what part you don't understand exactly ?

Anyway what you want to do is no more than very easy thing for everyone.

no its not very easy how can you think its easy when you don't even understand what i'm saying ? i appreciate your time and your help dear pancho but you seem a little condescending . people who ask their questions here are not all professionals like you. .

 

[pancho_hideboo]

maybe you mean what technology i use its tsmc 0.13 um

No.
You are same as https://www.edaboard.com/showthread.php?378988#6

what do you mean by spectre -h isource can you describe more please ?

Enter it as unix command.

what part you don't understand exactly ?

There is no attached file in your previous post.

no its not very easy how can you think its easy

Too easy thing.

when you don't even understand what i'm saying ?

Simply you can not understand tools you use at all.
Design Framework and Simulator are different.
Can you understand ?

 

[ultrasonic.1991]

ok now i get it my version is 7.1.1.187.isr11 32bit -- 18 Aug 2009 it was in spectre.out file . i checked the attachment its ok i upload it again

- - - Updated - - -

ps : i searched spectre h isource and spectre h i found nothing then i entered specter h isource and then spectre h in terminal it says command not found can you help with that too ?

 

[pancho_hideboo]

Simply you can not understand type=bit.
First it is a fixed data stream not pseudo number.
Second your setting generates constant zero pattern.

I don't need hardcopy of GUI.
Show me
Netlist
Version of Simulator
Version of Design Framework
Ocean Script if you plot some data from Cadence ADE

 

[pancho_hideboo]

ok now i get it my version is 7.1.1.187.isr11 32bit -- 18 Aug 2009

Your Spectre is relative old.
I don't remember whether your Spectre supports "type=prbs" or not.

i entered specter h isource
and then spectre h in terminal
it says command not found

Simply you don't include Spectre path in your command search path.

Confirm "echo $path".

If you can do "spectre -h isource", you can know whether your Spectre supports "type=prbs" or not.

If not, you have to use "type=bit with setting data pattern" or "ahdlLib/rand_bit_stream".

See attached figures.
Don't you think it is too easy ?

"guide_for_ultrasonic1991.scs"

// Generated for: spectre
// Generated on: Jul 31 12:15:01 2018
// Design library name: My_RFDE_Test
// Design cell name: guide_for_ultrasonic1991
// Design view name: schematic
simulator lang=spectre
global 0
parameters _EXPR_2=1.024e-07 Bit_Rate=10G

// Library name: My_RFDE_Test
// Cell name: guide_for_ultrasonic1991
// View name: schematic
I0 (net5) rand_bit_stream tperiod=1/Bit_Rate vlogic_high=20u vlogic_low=0 \
        trise=(1/Bit_Rate)/20 tfall=(1/Bit_Rate)/20
G0 (net3 0 net5 0) vccs gm=-1
IPRB0 (net3 0) iprobe
simulatorOptions options psfversion="1.1.0" reltol=1e-3 vabstol=1e-6 \
    iabstol=1e-12 temp=25.0 tnom=25.0 scalem=1.0 scale=1.0 gmin=1e-12 \
    rforce=1 maxnotes=5 maxwarns=5 digits=5 cols=80 pivrel=1e-3 \
    sensfile="../psf/sens.output" checklimitdest=psf 
tran tran stop=_EXPR_2 errpreset=moderate annotate=status maxiters=5 
designParamVals info what=parameters where=rawfile
save IPRB0:in 
saveOptions options save=selected
ahdl_include "/hoge/tools/dfII/samples/artist/ahdlLib/rand_bit_stream/veriloga/veriloga.va"

"guide_for_ultrasonic1991.ocn"

simulator( 'spectre )
design(	 "/hoge/simulation/guide_for_ultrasonic1991/spectre/schematic/netlist/netlist")
resultsDir( "/hoge/simulation/guide_for_ultrasonic1991/spectre/schematic" )
analysis('tran ?stop "1024/VAR(\"Bit_Rate\")"  ?write ""  ?writefinal ""  
		?finalTimeOp nil  )
desVar(	  "Bit_Rate" 10G	)
envOption(
	'analysisOrder  list("tran") 
)
saveOption( ?infoOptions list(list("modelParameter" "models" "rawfile" "" "" "" nil) list("element" "inst" "rawfile" "" "" "" nil) list("outputParameter" "output" "rawfile" "" "" "" nil) list("designParamVals" "parameters" "rawfile" "" "" "" t) list("primitives" "primitives" "rawfile" "" "" "" nil) list("subckts" "subckts" "rawfile" "" "" "" nil) list("asserts" "assert" "rawfile" "" "" "" nil) list("extremeinfo" "all" "logfile" "" "yes" "" nil) list("<Click_To_Add>" "none" "rawfile" "" "" "" nil) ) )
saveOption( ?saveahdlvars "" )
save( 'i "/IPRB0/PLUS" )
temp( 25.0 ) 
run()
Eye_Diagram = eyeDiagram(i("/IPRB0/PLUS" ?result "tran") 0 0.01 (2 / VAR("Bit_Rate")) ?autoCenter t)
plot( Eye_Diagram ?expr '( "Eye_Diagram" ) )

 

[ultrasonic.1991]

thanks i used rand_bit_stream and vccs like the way you did in the pictures and the eye diagram seems fine.however i have some questions about eye diagram of tia that i think its better to post it in a new thread.