How does one do .MEASURE in Spectre ?

[analogTechie]

spectre measure

Hi All,

Greetings!

Can anyone help with measuring propagation delay in Spectre ?

In HSPICE, one can do the following, for instance:

.MEAS TPLH TRIG PAR('V(2)-0.5*VDD') VAL=0 FALL=1
+ TARG PAR('V(3)-0.5*VDD') VAL=0 RISE=1

How can we make the same measurement in Spectre ?
I hear there is a deltax command but I cannot find it in either the User
Guide or the Ref Manual.

Thanks,

 

[flamingo]

spectre mdl

Spectre's tools :calculator, there incude many useful mathmatical operation, just like the data post operation in Hspice

 

[analogTechie]

measure statements in spectre

Flamingo,

Thanks for the response.

I am using the command line interface to run spectre. I am not running it
within the Cadence Analog Design Environment. So to run spectre I give the
command

spectre filename.scs

Then I use the -format nutbin option to generate a .raw file which I can view
using a smartspice postprocessor. So I do not have access to spectre's
calculator.

Coming back to my original question, you can put .measure statements in your
HSPICE deck. Isn't there some equivalent command that you can put in your
spectre deck ?

thanks. all assistance is appreciated greatly.

 

[jordan76]

measureing delay in cadence spectre

Hi,

As far as I know,there are two methods to solve the measurement problem in Spectre. One is to use verilog-a model, the other is to resort to OCEAN(Open Command Environment for Analysis). Attached is a tutorial about verilog-a;you can google for OCEAN tutorial.

Hope it helps.

regards,
jordan76

 

[paladinzlp]

spectre measurement

You can use the tool :Spice Exp

 

[morecode1234567890]

cadence spectre .measure

is there any way to automatizate the measurement using calculator, i have not found any script language manual.

and please, how can i plot differential waves????

that is all thx

 

[intuition]

spectre .measure

You can using command :

spectrespp *.sp

directly, and spectre will create a file *.mdl to transform spice .measure and run, the rusult output file styled *.measure. But it seems just work for tran, ac, and dc analysis, not ready for pss and pac..(or there's newer version released?)

Added after 13 minutes:

is there any way to automatizate the measurement using calculator, i have not found any script language manual.

and please, how can i plot differential waves????

that is all thx

You can use Cadence Analog Environment to indicate output waveform by calculator, and save by Session-->Save State; just load the state while running you circuit.

 

[rambus_ddr]

run spectre command line

use ocean, you can run spectre and measure many parameters.

 

[Hughes]

.measure spectre

is there any way to automatizate the measurement using calculator, i have not found any script language manual.

and please, how can i plot differential waves????

that is all thx

You can add the expression to the "Setup Outputs" form. E.g.:
Name: VIN
Expression: VT("/VINP")-VT("/INN")

 

[layes2]

spectre measure to file

I think you can not use it in spectra but spectre is power enough in graph interface

 

[uncle_urfi]

spectre meas

The full potential of spectre is only utilized when one uses a graphical interface. There are many people preparing to respond to this opening sentence.

I say to them that a very small minority of IC designers are good at OCEAN/SKILL scripting and it is prob. not the right thing to send a newbie into this whirlpool.

In the graphical mode, one can get a lot more work done with spectre, given the same proficiency level. Sorry Hspice/Eldo users! You need a cad specialist on site to setup you geeky scripts (typos anyone)

Learning SKILL/OCEAN as you go along is a worthwhile endeavor though, for it allows the same benefits as scripting does.

I think i am going in circles.

 

[Julian18]

mdl spectre programing

hi, I just need one piece of lines using OCEAN to get a Y value from a waveform giving the X value.

Thanks

 

[kumar123]

measure in spectre

Hi All,

Greetings!

Can anyone help with measuring propagation delay in Spectre ?

In HSPICE, one can do the following, for instance:

.MEAS TPLH TRIG PAR('V(2)-0.5*VDD') VAL=0 FALL=1
+ TARG PAR('V(3)-0.5*VDD') VAL=0 RISE=1

How can we make the same measurement in Spectre ?
I hear there is a deltax command but I cannot find it in either the User
Guide or the Ref Manual.


Hi
You can't perform directly the .measurement in spectre how you declare in Hpice and SPICE within deck(signle file) the reason here the measurement is done seperately as below
1) from the simulation ersults using waveform viewer u can select the calculator
( there you will see many functions)
2) else to direct dumping of the value in a file using MDL approach
if you are using command line spectre run you can give spectre mdl run to compute that value as below
spectremdl -b file1.mdl -d file2.scs

where file2.scs ----> is your deck
file1.mdl ----> is your mdl file ( sample is pasted below to use your purpose just change the simulation name "run ANA_tran_TT" ANA_tran_TT with your transient analysis name )

the results will be displayed in "file1.measure" always it is better to give same name file1 = file2

Hope this helps your need
//***********************************************
alias measurement Tr_Tf_Delay {
//Variable declaration of real type
export real Fall_Time , Rise_Time ,Delay_R ,Delay_F

//Calling Analysis name declared in deck
run ANA_tran_TT

// Fall, Rise , Rise Delay, Fall Delay measurement
Fall_Time = falltime(V(OUT),1,0,theta1=90,theta2=10)
Rise_Time = risetime(V(OUT),0,1,theta1=10,theta2=90)
Delay_R = deltax( sig1=V(IN), dir1='rise, thresh1=0.5*VDD,\
sig2=V(OUT), dir2='rise, thresh2=0.5*VDD )

Delay_F = deltax( sig1=V(IN), dir1='fall, thresh1=0.5*VDD,\
sig2=V(OUT), dir2='fall, thresh2=0.5*VDD )

}

// Running the Function declared in MDL file
run Tr_Tf_Delay

 

[mmic1978]

Re: measure in spectre

Hi All,

Greetings!

Can anyone help with measuring propagation delay in Spectre ?

In HSPICE, one can do the following, for instance:

.MEAS TPLH TRIG PAR('V(2)-0.5*VDD') VAL=0 FALL=1
+ TARG PAR('V(3)-0.5*VDD') VAL=0 RISE=1

How can we make the same measurement in Spectre ?
I hear there is a deltax command but I cannot find it in either the User
Guide or the Ref Manual.


Hi
You can't perform directly the .measurement in spectre how you declare in Hpice and SPICE within deck(signle file) the reason here the measurement is done seperately as below
1) from the simulation ersults using waveform viewer u can select the calculator
( there you will see many functions)
2) else to direct dumping of the value in a file using MDL approach
if you are using command line spectre run you can give spectre mdl run to compute that value as below
spectremdl -b file1.mdl -d file2.scs

where file2.scs ----> is your deck
file1.mdl ----> is your mdl file ( sample is pasted below to use your purpose just change the simulation name "run ANA_tran_TT" ANA_tran_TT with your transient analysis name )

the results will be displayed in "file1.measure" always it is better to give same name file1 = file2

Hope this helps your need
//***********************************************
alias measurement Tr_Tf_Delay {
//Variable declaration of real type
export real Fall_Time , Rise_Time ,Delay_R ,Delay_F

//Calling Analysis name declared in deck
run ANA_tran_TT

// Fall, Rise , Rise Delay, Fall Delay measurement
Fall_Time = falltime(V(OUT),1,0,theta1=90,theta2=10)
Rise_Time = risetime(V(OUT),0,1,theta1=10,theta2=90)
Delay_R = deltax( sig1=V(IN), dir1='rise, thresh1=0.5*VDD,\
sig2=V(OUT), dir2='rise, thresh2=0.5*VDD )

Delay_F = deltax( sig1=V(IN), dir1='fall, thresh1=0.5*VDD,\
sig2=V(OUT), dir2='fall, thresh2=0.5*VDD )

}

// Running the Function declared in MDL file
run Tr_Tf_Delay

I use the new MDL like this:

spectre =mdl *.mdl #.scs

if *=#, then auto produce one *(#).measure file

But, if it can not produce, how to reslove?

 

[hansbe]

Re: spectre measure

Hi All,

Greetings!

Can anyone help with measuring propagation delay in Spectre ?

In HSPICE, one can do the following, for instance:

.MEAS TPLH TRIG PAR('V(2)-0.5*VDD') VAL=0 FALL=1
+ TARG PAR('V(3)-0.5*VDD') VAL=0 RISE=1

How can we make the same measurement in Spectre ?
I hear there is a deltax command but I cannot find it in either the User
Guide or the Ref Manual.

Thanks,

In my spectre (version 6.2 from 2007) I can just put in spice .measure commands enclosed by simulator lang directives in the spectre netlist:

simulator lang=spice
.MEAS  TPLH  TRIG   PAR('V(2)-0.5*VDD')  VAL=0  FALL=1  TARG  PAR('V(3)-0.5*VDD')  VAL=0  RISE=1
simulator lang=spectre