Use of DC operating point parameters in plots

Hi group,

I run a DC sweep simulation on ADE (using spectre) and I would like to
plot some of the DC operating point parameter of my schematic(such as
gm, gds,vdsat of the transistor which I can not see soem of these
parameter in the Result Browser )
Does any one have any idea ?


Regards
Leyla

 

[Svenn Are Bjerkem]

On Jul 9, 8:44 am, leylakooshae...@gmail.com wrote:

Hi group,

I run a DC sweep simulation on ADE (using spectre) and I would like to
plot some of the DC operating point parameter of my schematic(such as
gm, gds,vdsat of the transistor which I can not see soem of these
parameter in the Result Browser )
Does any one have any idea ?

Regards
Leyla

Is the option "Save DC operating point" active in the setup analysis
form for the DC simulation?
Check your "Save All..." settings in the Outputs menu of ADE.
Which waveform viewer are you using?

--
Svenn

 

On Jul 10, 12:29 am, Svenn Are Bjerkem <svenn.bjer...@googlemail.com>
wrote:

On Jul 9, 8:44 am, leylakooshae...@gmail.com wrote:

Hi group,

I run a DC sweep simulation on ADE (using spectre) and I would like to
plot some of the DC operating point parameter of my schematic(such as
gm, gds,vdsat of the transistor which I can not see soem of these
parameter in the Result Browser )
Does any one have any idea ?

Regards
Leyla

Is the option "Save DC operating point" active in the setup analysis
form for the DC simulation?
Check your "Save All..." settings in the Outputs menu of ADE.
Which waveform viewer are you using?

--
Svenn

Even with activation of Save Dc operating point we can not see gm in
the Result Browser!!!
I found that the answer is to go to ADE and then print > Dc
operating point > I can see the gm
But how can I plot the gm vs VGS ?? any idea ......

 

[Andrew Beckett]

On Mon, 09 Jul 2007 14:29:08 -0000, Svenn Are Bjerkem
<svenn.bjerkem@googlemail.com> wrote:

On Jul 9, 8:44 am, leylakooshae...@gmail.com wrote:
Hi group,

I run a DC sweep simulation on ADE (using spectre) and I would like to
plot some of the DC operating point parameter of my schematic(such as
gm, gds,vdsat of the transistor which I can not see soem of these
parameter in the Result Browser )
Does any one have any idea ?

Regards
Leyla

Is the option "Save DC operating point" active in the setup analysis
form for the DC simulation?
Check your "Save All..." settings in the Outputs menu of ADE.
Which waveform viewer are you using?

Actually this has come up many times before in this forum (and over on
the Designer's Guide forum). When you do a DC sweep, it does not save the
operating point for each point in the sweep by default.

You can do this by creating an ASCII file somewhere, with:

save M1

or:

save M1ppoint

or

save M1:gm M1:gds M1:vdsat

in the file, and then adding this as a model library in ADE (effectively as
an include file). You'll then be able to get to the operating point data via the
results browser after the simulation. Normally this isn't saved for space
reasons.

Note that "M1" is the name of the instance you want to save. Watch out if
it's a subckt model - you may need to find out the hierarchical name of the
internal device to save (use "." as the hierarchy delimiter).

If you have access to the newly released MMSIM62, you can use wildcards in
the save statement. For example:

save * sigtype=all

will save absolutely everything for every device (as well as all terminal
currents and so on).

Regards,

Andrew.
--
Andrew Beckett
Senior Solution Architect
Cadence Design Systems, UK.

 

Thanks Andrew,

I am so new working with cadence so excuse of my ignorance.

I got a warning in psf/spectre.out

There is a warning from spectre during initial setup:
M0 does not have a terminal named gm
Ignoring invalid item named M0: gm in save statement

I did these procedures for creating the text file and include it to
the model library:

I create a text file in the UNIX terminal with dtpad and put the save
M0: gm inside the text file.
For running the ADE simulation for 90n CMOS technology I save the
model library from the Tools > set up corner not from set up library
(I don't know the reason)
After opening the set up corner I activate the include file and put
the tt.txt in the "include file editor "
Also I tried with tt.scs file to see any difference but it didn't
work.
Please guide me?

 

[Andrew Beckett]

On Tue, 10 Jul 2007 21:28:05 -0700, leylakooshaeian@gmail.com wrote:

Thanks Andrew,

I am so new working with cadence so excuse of my ignorance.

I got a warning in psf/spectre.out

There is a warning from spectre during initial setup:
M0 does not have a terminal named gm
Ignoring invalid item named M0: gm in save statement

I did these procedures for creating the text file and include it to
the model library:

I create a text file in the UNIX terminal with dtpad and put the save
M0: gm inside the text file.
For running the ADE simulation for 90n CMOS technology I save the
model library from the Tools > set up corner not from set up library
(I don't know the reason)
After opening the set up corner I activate the include file and put
the tt.txt in the "include file editor "
Also I tried with tt.scs file to see any difference but it didn't
work.
Please guide me?

Most likely this is because M0 is an instance of a subckt model, not a direct
instantiation of a primitive device. Check to see if your models are subckts -
if so, you'll need to save the gm of the actual device inside that subckt, as I
described in my previous post (e.g. M0.Minternal:gm or whatever it is called).
Alternatively use MMSIM62 which means you can use the wildcard!

The corner stuff must be some customisation for the technology you're using -
but that probably doesn't matter - this is just a means of including a file
somehow.

Regards,

Andrew.
--
Andrew Beckett
Senior Solution Architect
Cadence Design Systems, UK.

 

Andrew,
I search and I found the similar disscusion in 2004 you recomended:

The problem is that because the filename did not end in .scs, it
assumed that
the include file was in SPICE syntax (for compatibility reasons), and
so it
then becomes case insensitive - actually all are mapped to lowercase.
This is why the M0 you specified got mapped to m0, and there is no m0
in
the netlist.

You have two choices:

1. Call the include file "settings.scs"
2. or, at the top of the included file, add a line:

simulator lang=spectre

I tried with include" tt.scs "and also with and without adding
simulator lang=spectre in teh first line of "tt.scs " again same
warning

Please guide ?

Best reagrds/ leyla

 

On Jul 11, 3:16 pm, Andrew Beckett <andr...@DcEaLdEeTnEcTe.HcIoSm>
wrote:

On Tue, 10 Jul 2007 21:28:05 -0700, leylakooshae...@gmail.com wrote:
Thanks Andrew,

I am so new working with cadence so excuse of my ignorance.

I got a warning in psf/spectre.out

There is a warning from spectre during initial setup:
M0 does not have a terminal named gm
Ignoring invalid item named M0: gm in save statement

I did these procedures for creating the text file and include it to
the model library:

I create a text file in the UNIX terminal with dtpad and put the save
M0: gm inside the text file.
For running the ADE simulation for 90n CMOS technology I save the
model library from the Tools > set up corner not from set up library
(I don't know the reason)
After opening the set up corner I activate the include file and put
the tt.txt in the "include file editor "
Also I tried with tt.scs file to see any difference but it didn't
work.
Please guide me?

Most likely this is because M0 is an instance of a subckt model, not a direct
instantiation of a primitive device. Check to see if your models are subckts -
if so, you'll need to save the gm of the actual device inside that subckt, as I
described in my previous post (e.g. M0.Minternal:gm or whatever it is called).
Alternatively use MMSIM62 which means you can use the wildcard!

The corner stuff must be some customisation for the technology you're using -
but that probably doesn't matter - this is just a means of including a file
somehow.

Regards,

Andrew.
--
Andrew Beckett
Senior Solution Architect
Cadence Design Systems, UK.

Thanks Andrew,
Sorry I didn't recognise you replied, the schematic taht I am testing
very simple circuit with only one transisitor with instance's name of
M0.
Regards

 

[Andrew Beckett]

On Tue, 10 Jul 2007 22:38:13 -0700, leylakooshaeian@gmail.com wrote:

Andrew,
I search and I found the similar disscusion in 2004 you recomended:

The problem is that because the filename did not end in .scs, it
assumed that
the include file was in SPICE syntax (for compatibility reasons), and
so it
then becomes case insensitive - actually all are mapped to lowercase.
This is why the M0 you specified got mapped to m0, and there is no m0
in
the netlist.

You have two choices:

1. Call the include file "settings.scs"
2. or, at the top of the included file, add a line:

simulator lang=spectre

I tried with include" tt.scs "and also with and without adding
simulator lang=spectre in teh first line of "tt.scs " again same
warning

Please guide ?

Best reagrds/ leyla

As I said before (twice), is the model a subckt? There may only be a single
instance, but if that instance is an instance of a subckt model, you will need
to include the additional hierarchy in the instance name to be saved.

Easiest way to find this out is to do a DC operating point (don't sweep), and
then look in the results browser to see if there is any hierarchy there, and
to see what the names are.

You do also need to give the file the right suffix, or use simulator
lang=spectre, but I don't think that's your problem here?

Regards,

Andrew.
--
Andrew Beckett
Senior Solution Architect
Cadence Design Systems, UK.

 

Thanks Andrew,
the circuit that I use,is not an instance of a subckt model. I tried
with another circuit as well now it gives me a warning that "M0:does
not have a terminal name gm"
I make a file named tt.scs and put the save M0:gm in the first line .
This is nontrivial question for you but I don't now how to solve it,
please guide....
Regards
Leyla

 

[Andrew Beckett]

On Wed, 11 Jul 2007 23:17:43 -0700, leylakooshaeian@gmail.com wrote:

Thanks Andrew,
the circuit that I use,is not an instance of a subckt model. I tried
with another circuit as well now it gives me a warning that "M0:does
not have a terminal name gm"
I make a file named tt.scs and put the save M0:gm in the first line .
This is nontrivial question for you but I don't now how to solve it,
please guide....
Regards
Leyla

Well, it won't give that message unless M0 is an instance of a subckt.
For example:

//
// Noddy analysis to generate id vs vds and vgs curves for a simple
// level 1 transistor.
//

subckt nch (d g s b)
parameters w=1u l=1u
nch (d g s b) nch w=w l=l
model nch mos1 type=n vto=1 kp=16u gamma=1.3 lambda=0.01 \
phi=0.7 pb=0.80 mj=0.5 mjsw=0.3 cgbo=200p cgso=350p cgdo=350p \
cj=300u cjsw=500p ld=0.1u tox=80n \
af=1 kf=3.1e-24
ends nch

parameters channel=0.8u
m1 (drain gate 0 0) nch w=20u l=channel
vgs (gate 0) vsource dc=3
vds (drain 0) vsource dc=1

simulator lang=spectre

save m1:gm
// end of netlist

gives:

Warning from spectre during initial setup.
`m1': Does not have a terminal named `gm'.
Ignoring invalid item `m1:gm' in save statement.

If I change the save statement to:

save m1.nch:gm

it works OK - since that's the name of the actual instance.

I suggest you put something like this in your netlist:

components info what=inst where=logfile

and then run with a single transistor. In my case I get:

Instance: m1.nch of nch
Model: m1.nch
Primitive: mos1
w = 20 um
l = 800 nm
ld = 0 m
m = 1
region = off
degradation = no

so you can see what the instance name of the primitive device is called.

Regards,

Andrew.
--
Andrew Beckett
Senior Solution Architect
Cadence Design Systems, UK.

 

Thanks Andrew,
I run the components info what=inst where=logfile
and in the logfile I got this:

Instance: M0.m1 of nsvt
Model: M0.nsvt
Primitive: bsim4
w = 1.2 um
l = 100 nm
as=number
ad=number
ps=number
pd=number
m = 1
region = off

Also I have the M0.Dd and M0.Ds for just a single transistor,

Then I try with

Save M0.nsvt: gm

Another try was with
Save M0.m1: gm

Both of them give me the same warning that I mentioned in the previous
post.
By the way, if finally after your guide I succeed to get the gm can I
plot it Vs VGS, I sweep the VGS in my dc analysis because I think I
can see only the last sweep parameter for gm.
I desperately need your advice.

Best Regards
Leila

 

Thanks Andrew,
I run the components info what=inst where=logfile
and in the logfile I got this:

Instance: M0.m1 of nsvt
Model: M0.nsvt
Primitive: bsim4
w = 1.2 um
l = 100 nm
as=number
ad=number
ps=number
pd=number
m = 1
region = off

Also I have the M0.Dd and M0.Ds for just a single transistor,

Then I try with

Save M0.nsvt: gm

Another try was with
Save M0.m1: gm

Both of them give me the same warning that I mentioned in the previous
post.
By the way, if finally after your guide I succeed to get the gm can I
plot it Vs VGS, I sweep the VGS in my dc analysis because I think I
can see only the last sweep parameter for gm.
I desperately need your advice.

 

On Jul 17, 6:47 pm, Andrew Beckett <andr...@DcEaLdEeTnEcTe.HcIoSm>
wrote:

On Wed, 11 Jul 2007 23:17:43 -0700, leylakooshae...@gmail.com wrote:

Thanks Andrew,
the circuit that I use,is not an instance of a subckt model. I tried
with another circuit as well now it gives me a warning that "M0:does
not have a terminal name gm"
I make a file named tt.scs and put the save M0:gm in the first line .
This is nontrivial question for you but I don't now how to solve it,
please guide....
Regards
Leyla

Well, it won't give that message unless M0 is an instance of a subckt.
For example:

//
// Noddy analysis to generate id vs vds and vgs curves for a simple
// level 1 transistor.
//

subckt nch (d g s b)
parameters w=1u l=1u
nch (d g s b) nch w=w l=l
model nch mos1 type=n vto=1 kp=16u gamma=1.3 lambda=0.01 \
phi=0.7 pb=0.80 mj=0.5 mjsw=0.3 cgbo=200p cgso=350p cgdo=350p \
cj=300u cjsw=500p ld=0.1u tox=80n \
af=1 kf=3.1e-24
ends nch

parameters channel=0.8u
m1 (drain gate 0 0) nch w=20u l=channel
vgs (gate 0) vsource dc=3
vds (drain 0) vsource dc=1

simulator lang=spectre

save m1:gm
// end of netlist

gives:

Warning from spectre during initial setup.
`m1': Does not have a terminal named `gm'.
Ignoring invalid item `m1:gm' in save statement.

If I change the save statement to:

save m1.nch:gm

it works OK - since that's the name of the actual instance.

I suggest you put something like this in your netlist:

components info what=inst where=logfile

and then run with a single transistor. In my case I get:

Instance: m1.nch of nch
Model: m1.nch
Primitive: mos1
w = 20 um
l = 800 nm
ld = 0 m
m = 1
region = off
degradation = no

so you can see what the instance name of the primitive device is called.

Regards,

Andrew.
--
Andrew Beckett
Senior Solution Architect
Cadence Design Systems, UK.

Thanks Andrew,
I run the components info what=inst where=logfile
and in the logfile I got this:

Instance: M0.m1 of nsvt
Model: M0.nsvt
Primitive: bsim4
w = 1.2 um
l = 100 nm
as=number
ad=number
ps=number
pd=number
m = 1
region = off

Also I have the M0.Dd and M0.Ds for just a single transistor,

Then I try with

Save M0.nsvt: gm

Another try was with
Save M0.m1: gm

Both of them give me the same warning that I mentioned in the previous
post.
By the way, if finally after your guide I succeed to get the gm can I
plot it Vs VGS, I sweep the VGS in my dc analysis because I think I
can see only the last sweep parameter for gm.
I desperately need your advice.

 

[Andrew Beckett]

On Fri, 20 Jul 2007 00:44:17 -0700, leylakooshaeian@gmail.com wrote:

Thanks Andrew,
I run the components info what=inst where=logfile
and in the logfile I got this:

Instance: M0.m1 of nsvt
Model: M0.nsvt
Primitive: bsim4
w = 1.2 um
l = 100 nm
as=number
ad=number
ps=number
pd=number
m = 1
region = off

Also I have the M0.Dd and M0.Ds for just a single transistor,

Then I try with

Save M0.nsvt: gm

Another try was with
Save M0.m1: gm

Both of them give me the same warning that I mentioned in the previous
post.
By the way, if finally after your guide I succeed to get the gm can I
plot it Vs VGS, I sweep the VGS in my dc analysis because I think I
can see only the last sweep parameter for gm.
I desperately need your advice.

Well, it would be:

save M0.m1:gm

or just

save M0.m1

(that way it will save all op point data).

save is in lower case, and there should be no space between the colon and the
gm.

So this ought to work, provided you get the syntax correct. Without seeing the
example as a whole, it's hard to know what you've done wrong. You were saying
that you definitely didn't have subckts - but clearly you do - so I can only
imagine that you've made a simple mistake somewhere?

Note, if you do a sweep, you'll get the saved op point params versus the sweep.

Regards,

Andrew.
--
Andrew Beckett
Senior Solution Architect
Cadence Design Systems, UK.