How to run simulation with spice netlist coming from dracula

[tech11]

After run lpe drawing with dracula, I get one spice netlist which including
parasitical cap and res. But when I run simulation with spectre and get
errors such as 'spectre section definition not found' and many syntax
errors. I remember spcetre can read spice netlist well, why does it output
such errors? Need I deal with the drawing spice netlist? How should I do it?
Since I have not done such one flow and would you please help me or give me
some advice? Thanks for your help!

Have a good day!

Best Regards,

Joffre

 

[Andrew Beckett]

On Sun, 11 Dec 2005 22:58:51 +0800, "tech11" <tech11@sohu.com> wrote:

After run lpe drawing with dracula, I get one spice netlist which including
parasitical cap and res. But when I run simulation with spectre and get
errors such as 'spectre section definition not found' and many syntax
errors. I remember spcetre can read spice netlist well, why does it output
such errors? Need I deal with the drawing spice netlist? How should I do it?
Since I have not done such one flow and would you please help me or give me
some advice? Thanks for your help!

Have a good day!

Best Regards,

Joffre

Well, without seeing an example netlist, I don't know. You must be doing
something to the netlist, since it wouldn't have analysis statements within it,
nor would it have model references. It sounds as if you're trying to include a
section of a model file, but are specifying it incorrectly.

Note that files with the .scs suffix are interpreted as spectre syntax;
everything else is SPICE. You might also want to use IC5141 and
the +csfe command line option to spectre, or MMSIM60 where +csfe is on by
default (this is the new front end which parses SPICE more completely).

Regards,

Andrew.

 

[tech11]

Well, without seeing an example netlist, I don't know. You must be doing
something to the netlist, since it wouldn't have analysis statements
within it,
nor would it have model references. It sounds as if you're trying to
include a
section of a model file, but are specifying it incorrectly.

Note that files with the .scs suffix are interpreted as spectre syntax;
everything else is SPICE. You might also want to use IC5141 and
the +csfe command line option to spectre, or MMSIM60 where +csfe is on by
default (this is the new front end which parses SPICE more completely).

Regards,

Andrew.

Dear Andrew,

Below is my spectre running spice netlist and run file:
1) lpe extract file 'LPENET.sp':
* CADENCE/LPE SPICE FILE : LPENET
* DATE : 6-DEC-2005
*
******
****** MOS XTOR PARAMETERS FROM : 7MOSXREF
******
*
*
*.GLOBAL GND VDD
*
*
..SUBCKT .......
****** RESISTORS PARAMETERS FROM : 7RESXREF
******
*
*
RI18 ZT<4> GND RH 1.40000E05K
........
****** BJT XTOR PARAMETERS FROM : 7BJTXREF
******
*
*
QQ2 GND ZT<2> ZT<3> PN $EA=195.84P $EP=81.60U
........
****** CAPACITORS PARAMETERS FROM : 7CAPXREF
******
******
****** CAPACITORS PARAMETERS FROM : 7CAPXMER
******
*
*
C1 XI0-XI2-NET265 GND 1.19480E-12PF
.......
*
..ENDS


The spice netlist 'input.sp':
// Generated for: spectre
// Generated on: Dec 6 18:00:12 2005
// Design library name: xxxxxx
// Design cell name: xxxxxx
// Design view name: schematic
simulator lang=spectre
global 0
include $CDS_INST/tools.lnx86/dfII/samples/artist/ahdlLib/quantity.spectre"
include "./LPENET.sp"

parameters esr=20m iout=30m
include "....model/.../xxx.scs" section=tt_bt_rt

// Library name: xxxxxx
// Cell name: xxxxxx
// View name: schematic
......................

The run file 'runs':
spectre +spp +escchars +log ../psf/spectre.out
+mpssession=spectre1_25233_40 -format psfbin -raw ../psf input.sp

Then I run 'runs' directly
$> ./runs
//--INFORMATION--// SPICE Reader : MDL @version 1.2.2 01/31/2003

//--FATAL ERROR--// SPICE Reader : Spectre section definition not found.
//--FATAL ERROR--// SPICE Reader : Spectre section definition not found.
//--FATAL ERROR--// SPICE Reader : Spectre section definition not found.
//--WARNING--// SPICE Reader : ./LPENET.sp", Line 12 : zt<2> contained
misused > operator!
.........................................

I don't know what's the reason and how to continue to finish the simulation.
Would you please help me or give me some advice? Thanks for your help!

BTW, do you know how to do the flow with hspice?

Have a good day!

 

[Andrew Beckett]

On Tue, 13 Dec 2005 00:23:41 +0800, "tech11" <tech11@sohu.com> wrote:

Well, without seeing an example netlist, I don't know. You must be doing
something to the netlist, since it wouldn't have analysis statements
within it,
nor would it have model references. It sounds as if you're trying to
include a
section of a model file, but are specifying it incorrectly.

Note that files with the .scs suffix are interpreted as spectre syntax;
everything else is SPICE. You might also want to use IC5141 and
the +csfe command line option to spectre, or MMSIM60 where +csfe is on by
default (this is the new front end which parses SPICE more completely).

Regards,

Andrew.

Dear Andrew,

Below is my spectre running spice netlist and run file:
1) lpe extract file 'LPENET.sp':
* CADENCE/LPE SPICE FILE : LPENET
* DATE : 6-DEC-2005
*
******
****** MOS XTOR PARAMETERS FROM : 7MOSXREF
******
*
*
*.GLOBAL GND VDD
*
*
.SUBCKT .......
****** RESISTORS PARAMETERS FROM : 7RESXREF
******
*
*
RI18 ZT<4> GND RH 1.40000E05K
.......
****** BJT XTOR PARAMETERS FROM : 7BJTXREF
******
*
*
QQ2 GND ZT<2> ZT<3> PN $EA=195.84P $EP=81.60U
.......
****** CAPACITORS PARAMETERS FROM : 7CAPXREF
******
******
****** CAPACITORS PARAMETERS FROM : 7CAPXMER
******
*
*
C1 XI0-XI2-NET265 GND 1.19480E-12PF
......
*
.ENDS


The spice netlist 'input.sp':
// Generated for: spectre
// Generated on: Dec 6 18:00:12 2005
// Design library name: xxxxxx
// Design cell name: xxxxxx
// Design view name: schematic
simulator lang=spectre
global 0
include $CDS_INST/tools.lnx86/dfII/samples/artist/ahdlLib/quantity.spectre"
include "./LPENET.sp"

parameters esr=20m iout=30m
include "....model/.../xxx.scs" section=tt_bt_rt

// Library name: xxxxxx
// Cell name: xxxxxx
// View name: schematic
.....................

The run file 'runs':
spectre +spp +escchars +log ../psf/spectre.out
+mpssession=spectre1_25233_40 -format psfbin -raw ../psf input.sp

Then I run 'runs' directly
$> ./runs
//--INFORMATION--// SPICE Reader : MDL @version 1.2.2 01/31/2003

//--FATAL ERROR--// SPICE Reader : Spectre section definition not found.
//--FATAL ERROR--// SPICE Reader : Spectre section definition not found.
//--FATAL ERROR--// SPICE Reader : Spectre section definition not found.
//--WARNING--// SPICE Reader : ./LPENET.sp", Line 12 : zt<2> contained
misused > operator!
........................................

I don't know what's the reason and how to continue to finish the simulation.
Would you please help me or give me some advice? Thanks for your help!

BTW, do you know how to do the flow with hspice?

Have a good day!

Unfortunately you've cut so much out of the netlist, that I can't really see
what's wrong. I tried taking what you'd done and hacking it together. I get some
warnings about the "misused > operator", but the main problem is the same as one
I get when I try to run with the (better) spectre +csfe:

spectre +csfe test.scs

Error found by spectre during circuit read-in.
"./LPENET.sp" 17: An exponential format number was found with an alphabetic
suffix (1.40000E05K).
"./LPENET.sp" 30: An exponential format number was found with an alphabetic
suffix (1.19480E-12PF).


I essentially get the same error with spectre +spp too:

Error found by spectre in `blah', during circuit read-in.
"./LPENET.sp" 17: An exponential format number was found with an alphabetic
suffix (1.40000e05K).
"./LPENET.sp" 30: An exponential format number was found with an alphabetic
suffix (1.19480e-12p).

It's not surprising - the values have an exponent _and_ a suffix. I don't think
that makes sense... sounds as if something is wrong in your Dracula LPE setup.

I don't get any errors due to sections - so there must be something else wrong
in your netlist - or perhaps it's because you're using some older version with a
bug (you don't say what version you're using).

Can you try using +csfe like I suggested? (obviously you'll need to fix the
values, otherwise you'll hit the problem I did).

Andrew.

 

[tech11]

Unfortunately you've cut so much out of the netlist, that I can't really
see
what's wrong. I tried taking what you'd done and hacking it together. I
get some
warnings about the "misused > operator", but the main problem is the same
as one
I get when I try to run with the (better) spectre +csfe:

spectre +csfe test.scs

Error found by spectre during circuit read-in.
"./LPENET.sp" 17: An exponential format number was found with an
alphabetic
suffix (1.40000E05K).
"./LPENET.sp" 30: An exponential format number was found with an
alphabetic
suffix (1.19480E-12PF).


I essentially get the same error with spectre +spp too:

Error found by spectre in `blah', during circuit read-in.
"./LPENET.sp" 17: An exponential format number was found with an
alphabetic
suffix (1.40000e05K).
"./LPENET.sp" 30: An exponential format number was found with an
alphabetic
suffix (1.19480e-12p).

It's not surprising - the values have an exponent _and_ a suffix. I don't
think
that makes sense... sounds as if something is wrong in your Dracula LPE
setup.

I don't get any errors due to sections - so there must be something else
wrong
in your netlist - or perhaps it's because you're using some older version
with a
bug (you don't say what version you're using).

Can you try using +csfe like I suggested? (obviously you'll need to fix
the
values, otherwise you'll hit the problem I did).

Andrew.

Dear Andrew,

Sorry for the cutting netlist! Since I'm not a designer and just try to help
to test this flow, so it's inconvenient to post the full netlist and lpe
result.

Our tools is IC5033, I have no way to try the latest version. Would you
please share your post-simulation steps with spectre? I have not do such one
flow and don't know how to deal with the lpe results. Need I deal with the
lpe-after spice netlist before reading in by spectre? May the spectre models
be used by hspice?
Is my run file right?

When I run simulation with spectre? Does I need the schematic netlist?

Sorry to trouble you so much!

Have a good day!

Best Regards,

Joffre

 

[fogh]

Joffre,

include $CDS_INST/tools.lnx86/dfII/samples/artist/ahdlLib/quantity.spectre"
^^^ ^^^

this part looks wrong, you did not open the quote.
Use a proper text editor (it smells a bit like flame bait here ...) to help you
catch this kind of typos.

 

[tech11]

"fogh" <cad_support@skipthisandunderscores.catena.nl>
??????:11q3a5j9efkrk45@news.supernews.com...

Joffre,

include
$CDS_INST/tools.lnx86/dfII/samples/artist/ahdlLib/quantity.spectre"
^^^
^^^
this part looks wrong, you did not open the quote.
Use a proper text editor (it smells a bit like flame bait here ...) to
help you catch this kind of typos.

Dear Fogh,

Thanks for your reply! I lose to input the left quota, but there's it in my
running file, so it's not the real reason. Have you go this flow and help
me? Thanks a lot!

Have a good day!

Best Regards,

Joffre

 

[fogh]

tech11 wrote:

"fogh" <cad_support@skipthisandunderscores.catena.nl
??????:11q3a5j9efkrk45@news.supernews.com...

Joffre,


include
$CDS_INST/tools.lnx86/dfII/samples/artist/ahdlLib/quantity.spectre"

^^^
^^^
this part looks wrong, you did not open the quote.
Use a proper text editor (it smells a bit like flame bait here ...) to
help you catch this kind of typos.



Dear Fogh,

Thanks for your reply! I lose to input the left quota, but there's it in my
running file, so it's not the real reason. Have you go this flow and help
me? Thanks a lot!

Joffre ,

I can t make tests for you. As Andrew pointed out, the main problem
seems to be that numbers have both scientific notation and a suffix.
This is to be adressed by LPE deck author. If he is not available, you
ll have to get the LPE file, the dracula manual on the side, and start
hacking ...
If you are not up to delving in dracula, and find those numbers'
format to be rather uniform, you can also try some regexp fix, stg like
s/([ =][0-9][.][0-9]+E[+-]?[0-9]+)[aAfFpPnNuUmMkKgGtT][^ \t]*/\1/

 

[Andrew Beckett]

On Thu, 15 Dec 2005 17:37:04 +0800, "tech11" <tech11@sohu.com> wrote:

Dear Andrew,

Sorry for the cutting netlist! Since I'm not a designer and just try to help
to test this flow, so it's inconvenient to post the full netlist and lpe
result.

Our tools is IC5033, I have no way to try the latest version. Would you
please share your post-simulation steps with spectre? I have not do such one
flow and don't know how to deal with the lpe results. Need I deal with the
lpe-after spice netlist before reading in by spectre? May the spectre models
be used by hspice?
Is my run file right?

When I run simulation with spectre? Does I need the schematic netlist?

Sorry to trouble you so much!

Have a good day!

Best Regards,

Joffre

Just doing a bit of catching up, and I just noticed that I didn't answer this -
probably because I didn't understand the question...

Andrew.