spectre auto model selector syntax

Guest
Hi, All
I got a error when running spectre . The related part of
spectre.out is following:
Error found by spectre during circuit read-in.
"/export/home/mos_isolation_nmos.scs" 58: Syntax error in
model statement.
"/export/home/mos_isolation_nmos.scs" 120: Syntax error.
Statement ignored.
"/export/home/mos_isolation_nmos.scs" 175: Syntax error.
Statement ignored.
........
The following is related part of model file:
library mymos
section lv_mos
model nch n{
1: lmin=2e-6-dxl lmax=2e-5 wmin=2e-6-dxw wmax=2e-5 version=3.2
+tnom=25
+mobmod=1 binunit=1 capmod=3
.........
+pvoff=-0.203624442 letab=0.16201096 wetab=0.16201096 petab=-3.24021921
(the 58th line)
2: <version=3.2 lmin=1e-006 lmax='2e-006-dxl'
.......
+ppvag=-1.47135484> (the
120th line)
..........
+wpscbe1=48706018.2 wpscbe2=-4.97722034e-009 wpvag=-1.16053045(the
175th line)

I wish anyone tell me where are errors come from and how to correct
them?

thanks .
 
Hi,

Which Spectre version are you using? The last time I got an error like
this was for a new 90nm PDK. I was using Spectre 5.x (which comes with
IC 5.1.41). After updating to Spectre 6.x (MMSIM6.0) the simulation ran
without problems. Seems that model syntax changed or new features have
been added.
If you have any documentation of your model files check for software
version requirements.

Achim


jerk_kwork@yahoo.com wrote:
Hi, All
I got a error when running spectre . The related part of
spectre.out is following:
Error found by spectre during circuit read-in.
"/export/home/mos_isolation_nmos.scs" 58: Syntax error in
model statement.
"/export/home/mos_isolation_nmos.scs" 120: Syntax error.
Statement ignored.
"/export/home/mos_isolation_nmos.scs" 175: Syntax error.
Statement ignored.
........
The following is related part of model file:
library mymos
section lv_mos
model nch n{
1: lmin=2e-6-dxl lmax=2e-5 wmin=2e-6-dxw wmax=2e-5 version=3.2
+tnom=25
+mobmod=1 binunit=1 capmod=3
........
+pvoff=-0.203624442 letab=0.16201096 wetab=0.16201096 petab=-3.24021921
(the 58th line)
2: <version=3.2 lmin=1e-006 lmax='2e-006-dxl'
......
+ppvag=-1.47135484> (the
120th line)
.........
+wpscbe1=48706018.2 wpscbe2=-4.97722034e-009 wpvag=-1.16053045(the
175th line)

I wish anyone tell me where are errors come from and how to correct
them?

thanks .
Click to expand...
 
My model syntax differs a bit from yours

model name bsim3v3 {
1: type=n
+ lmin=

Can you check this issue with your silicon vendor or whoever
has provided you the model files?


Bernd

jerk_kwork@yahoo.com wrote:

model nch n{
1: lmin=2e-6-dxl lmax=2e-5 wmin=2e-6-dxw wmax=2e-5 version=3.2
Click to expand...
 
In fact the model file is for hspice not for spectre.
But I have no hspice in hand and the silicon vendor can only provide
spice model.
I need to amend the model file for running spectre. I really thank
your reply, it may save me.

Bernd Fischer 写道：

My model syntax differs a bit from yours

model name bsim3v3 {
1: type=n
+ lmin
Can you check this issue with your silicon vendor or whoever
has provided you the model files?


Bernd

jerk_kwork@yahoo.com wrote:

model nch n{
1: lmin=2e-6-dxl lmax=2e-5 wmin=2e-6-dxw wmax=2e-5 version=3.2
Click to expand...
 
I also use Spectre 5 with IC5.1.41. In fact the model file is for
hspice not for spectre.
But I have no hspice in hand and the silicon vendor can only provide
spice model.
I have to amend the model file for running spectre.
Achim Keller 写道：

Hi,

Which Spectre version are you using? The last time I got an error like
this was for a new 90nm PDK. I was using Spectre 5.x (which comes with
IC 5.1.41). After updating to Spectre 6.x (MMSIM6.0) the simulation ran
without problems. Seems that model syntax changed or new features have
been added.
If you have any documentation of your model files check for software
version requirements.

Achim


jerk_kwork@yahoo.com wrote:
Hi, All
I got a error when running spectre . The related part of
spectre.out is following:
Error found by spectre during circuit read-in.
"/export/home/mos_isolation_nmos.scs" 58: Syntax error in
model statement.
"/export/home/mos_isolation_nmos.scs" 120: Syntax error.
Statement ignored.
"/export/home/mos_isolation_nmos.scs" 175: Syntax error.
Statement ignored.
........
The following is related part of model file:
library mymos
section lv_mos
model nch n{
1: lmin=2e-6-dxl lmax=2e-5 wmin=2e-6-dxw wmax=2e-5 version=3.2
+tnom=25
+mobmod=1 binunit=1 capmod=3
........
+pvoff=-0.203624442 letab=0.16201096 wetab=0.16201096 petab=-3.24021921
(the 58th line)
2: <version=3.2 lmin=1e-006 lmax='2e-006-dxl'
......
+ppvag=-1.47135484> (the
120th line)
.........
+wpscbe1=48706018.2 wpscbe2=-4.97722034e-009 wpvag=-1.16053045(the
175th line)

I wish anyone tell me where are errors come from and how to correct
them?

thanks .
Click to expand...
 
There is an option
spectre +spp
* +spp Run the Spice netlist reader on input
which may help you, without modify you model file.
It's at least worth a trial.

In the Artist GUI you can find it under
Setup -> Environment...
Environment Options Form | Use SPICE Netlist Reader(spp)

If this does not help, you can try to convert your model file automatically with
'spp'.
Type 'spp -h' in your terminal and you'll get help.

Bernd



file.jerk_kwork@yahoo.com wrote:
In fact the model file is for hspice not for spectre.
But I have no hspice in hand and the silicon vendor can only provide
spice model.
I need to amend the model file for running spectre. I really thank
your reply, it may save me.
Click to expand...
 
Can you update Spectre? After MMSIM60 or MMSIM61, Spectre can natively
support Hspice syntax.

Regards,
Yuchun

Bernd Fischer wrote:
There is an option
spectre +spp
* +spp Run the Spice netlist reader on input
which may help you, without modify you model file.
It's at least worth a trial.

In the Artist GUI you can find it under
Setup -> Environment...
Environment Options Form | Use SPICE Netlist Reader(spp)

If this does not help, you can try to convert your model file automatically with
'spp'.
Type 'spp -h' in your terminal and you'll get help.

Bernd



file.jerk_kwork@yahoo.com wrote:
In fact the model file is for hspice not for spectre.
But I have no hspice in hand and the silicon vendor can only provide
spice model.
I need to amend the model file for running spectre. I really thank
your reply, it may save me.
Click to expand...
 
Hi,

I just took a look at the model. It isn't legal syntax of Spectre, nor
Hspice. For Bsim3v3, the definition should look like:
Hspice:
..lib lv_mos
..model nch.1 nmos level=49 version=3.2 lmin=....
..model nch.2 nmos level=49 ...

Spectre:
model nch bsim3v3 {
1: type=n version=3.2 lmin=...
2: ....
}

Maybe you can change 'n' to bsim3v3, but you may run into other problem
or get wrong results.

Yuchun

leanderdeng@gmail.com wrote:
Can you update Spectre? After MMSIM60 or MMSIM61, Spectre can natively
support Hspice syntax.

Regards,
Yuchun

Bernd Fischer wrote:
There is an option
spectre +spp
* +spp Run the Spice netlist reader on input
which may help you, without modify you model file.
It's at least worth a trial.

In the Artist GUI you can find it under
Setup -> Environment...
Environment Options Form | Use SPICE Netlist Reader(spp)

If this does not help, you can try to convert your model file automatically with
'spp'.
Type 'spp -h' in your terminal and you'll get help.

Bernd



file.jerk_kwork@yahoo.com wrote:
In fact the model file is for hspice not for spectre.
But I have no hspice in hand and the silicon vendor can only provide
spice model.
I need to amend the model file for running spectre. I really thank
your reply, it may save me.
Click to expand...
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top