How does one do .MEASURE in Spectre ?

analogTechie · Mar 9, 2005

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 · Mar 10, 2005

spectre mdl

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

analogTechie · Mar 10, 2005

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 · Mar 10, 2005

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 · Mar 10, 2005

spectre measurement

You can use the tool :Spice Exp

morecode1234567890 · Mar 15, 2005

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 · Jul 14, 2005

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:

morecode1234567890 said:
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 · Jul 16, 2005

run spectre command line

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

Hughes · Jul 17, 2005

.measure spectre

morecode1234567890 said:
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 · Jul 20, 2005

spectre measure to file

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

uncle_urfi · Jul 24, 2005

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 · Nov 29, 2007

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 · Nov 30, 2007

measure in spectre

analogTechie said:
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 · Nov 10, 2009

Re: measure in spectre

kumar123 said:
analogTechie said:

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

Click to expand...

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 · Sep 7, 2010

Re: spectre measure

analogTechie said:
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:

Code:

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

How does one do .MEASURE in Spectre ?

analogTechie

Junior Member level 1

flamingo

Member level 4

analogTechie

Junior Member level 1

jordan76

Full Member level 3

Attachments

paladinzlp

Full Member level 2

morecode1234567890

Junior Member level 1

intuition

Junior Member level 1

rambus_ddr

Advanced Member level 4

Hughes

Advanced Member level 3

layes2

Full Member level 4

uncle_urfi

Full Member level 2

Julian18

Full Member level 3

kumar123

Member level 3

tangqin55

mmic1978

Junior Member level 2

hansbe

Newbie level 4

Similar threads

How does one do .MEASURE in Spectre ?

Junior Member level 1

Member level 4

Junior Member level 1

Full Member level 3

Attachments

Full Member level 2

Junior Member level 1

Junior Member level 1

Advanced Member level 4

Advanced Member level 3

Full Member level 4

Full Member level 2

Full Member level 3

Member level 3

Junior Member level 2

Newbie level 4

Similar threads

Privacy & Transparency

Privacy & Transparency