How to convert hspice model file to spectre model file?

convert spice file to spectre file

How to convert hspice model file to spectre model file? Is there some soft can do it?

hspice model file to spectre

Specter can itself do that

how to convert spice file to spectre file

Can you tell me how to do by spectre in detail? I really appreciate your help.

level 49 bsim

in the console use
spp -convert -hspcompatible <hspice file> <specterfile>
look also into online help

spectre case insensitive

You have helped me . I have done it accorrding to your direction. And I delete "level=49" in the spectre model file that produed, because when I simulate netlist by spectre, there are some error .I want to know whether this will impact simulation percision.

Can you firstly tell me what error you are getting? I mean, it is better not to delete the level. It is always a risk, in the sense that there could be some other level models which might not model some second order effects as model 49.

"Spectre provides the SPICE Reader to let you simulate existing SPICE netlists with Spectre"
I think that this feature exists only in version 5.0 and above
Read the documentation

Error found by spectre during circuit read-in.
"/home/wzhao/model/t025model/hspice/mix0255_2.scs" 1868: Syntax error in
model statement.


This is the 1868 line:
model nch5 bsim3v3 level=49 {

If I delete the "level=49" , there is no error.

hi
spectre can simulate with bsim levels rather than hspice levels.

hspice level 49 = bsim level 13
...


tnx

You may need to inform spectre about it by some sort of command line options

I convert modle like this,why it not work??
spp -convert -hspcompatible wujl.l wujl.scs

please help me.

Hi friends,

The problem is as simple as this. Spectre defines level 49 model as 'bism3v3'. You follow the following procedure.

1.First spice file contains all the letters in uppercase letters. Write a simple C program to convert all the upper case letters into lower case letters.

2.Delete the '.' before the model

3.Add the statement in the beginning of the file as

simulator lang= spectre

4. Remove any brackets in the model file.

4. After model include your given transistor name in lower case letters for example 'pfet', 'nfet' or what ever the name you gave for the transistor.

6. After that you include bsim3v3 in lower case letters

7. After that you specify its type

type=p for PMOS
type=n for nmos


7.If your version of specre supports recent version in bsim3v3 you can include now

version=3.24.

version numbers 3.21,3.22,3.23,3.24 are all supported on ic5.0. All are same with improved curve fitting for capacitance models for recent versions like 3.24.

8. Remove '.m' extension to the model file and give '.scs' extension



leave the rest of the things as it is. It should work now. Other wise write to me with your problem. You can completely remove the level=49 if you specify version. No harm. Remeber that spectre is case sensitive where as SPICE is case insensitive.