Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

How does one do .MEASURE in Spectre ?

Status
Not open for further replies.

analogTechie

Junior Member level 1
Joined
Nov 2, 2004
Messages
15
Helped
3
Reputation
6
Reaction score
0
Trophy points
1,281
Location
USA
Activity points
170
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

Member level 4
Joined
Jan 10, 2005
Messages
73
Helped
6
Reputation
12
Reaction score
5
Trophy points
1,288
Activity points
717
spectre mdl

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

analogTechie

Junior Member level 1
Joined
Nov 2, 2004
Messages
15
Helped
3
Reputation
6
Reaction score
0
Trophy points
1,281
Location
USA
Activity points
170
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

Full Member level 3
Joined
Mar 25, 2004
Messages
174
Helped
4
Reputation
8
Reaction score
1
Trophy points
1,298
Activity points
1,852
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
 

Attachments

  • spectre_tut_149.pdf
    179.4 KB · Views: 142

paladinzlp

Full Member level 2
Joined
Feb 2, 2005
Messages
134
Helped
4
Reputation
8
Reaction score
0
Trophy points
1,296
Activity points
916
spectre measurement

You can use the tool :Spice Exp
 

morecode1234567890

Junior Member level 1
Joined
Oct 4, 2003
Messages
15
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
174
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

Junior Member level 1
Joined
May 20, 2005
Messages
18
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,485
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

Advanced Member level 4
Joined
Jun 26, 2001
Messages
107
Helped
3
Reputation
6
Reaction score
0
Trophy points
1,296
Activity points
970
run spectre command line

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

Hughes

Advanced Member level 3
Joined
Jun 10, 2003
Messages
717
Helped
113
Reputation
226
Reaction score
25
Trophy points
1,298
Activity points
5,984
.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

Full Member level 4
Joined
Dec 3, 2004
Messages
230
Helped
10
Reputation
20
Reaction score
6
Trophy points
1,298
Activity points
1,410
spectre measure to file

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

uncle_urfi

Full Member level 2
Joined
Mar 15, 2004
Messages
146
Helped
10
Reputation
20
Reaction score
6
Trophy points
1,298
Activity points
2,004
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

Full Member level 3
Joined
Apr 9, 2007
Messages
167
Helped
5
Reputation
10
Reaction score
5
Trophy points
1,298
Activity points
2,389
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

Member level 3
Joined
Sep 5, 2006
Messages
57
Helped
9
Reputation
18
Reaction score
6
Trophy points
1,288
Activity points
1,639
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

Junior Member level 2
Joined
Mar 31, 2009
Messages
22
Helped
2
Reputation
4
Reaction score
0
Trophy points
1,281
Activity points
1,366
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

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

Newbie level 4
Joined
Mar 14, 2006
Messages
7
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,315
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:

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
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top