Help----spectre fatal error "input.scs"

fatal error spectre



fatal error found by spectre during circuit read-in "input.scs" 2:
xSPICE Reader failure, see SPICE Reader log file:"input.spplog"


What does it mean?? What kind of problem with my circuit?

Thanks for help !!!

input.scs 2: xspice reader failure

What's in your "input.scs" line #2 ?
What's in your SPICE Reader log file: "input.spplog" ?

pspice subcircuit in spectre

Maybe the somewhere junction of your circuit is not correct, it will result in the spectre read in error !

to include spice netlist in cadence spectre

erikl said:

What's in your "input.scs" line #2 ?
What's in your SPICE Reader log file: "input.spplog" ?

Click to expand...

huojinsi said:

Maybe the somewhere junction of your circuit is not correct, it will result in the spectre read in error !

Click to expand...

It's my circuit schematic.
It's an typical example and should not has some theory mistake.

Where could I find the two files, i.e. input.scs and input.spplog?
From the two files, can i makeout the mistake?
I think it should be a common mistake, but i have too little experience to find it.[/img]

spectre save subcircuit

Hi istyle, in fact I have the same problem. SPP is responsible of this problem. First you can find the input.spplog in the directory in which you have your simulation result. It 's the directory that you have chosen by clicking:

Setup (Menu in Analog Environment) -> Simulator/Directory/Host
Project Directory.
For example, for me my directory is /users/these/baccarcadence/Sim
then in Sim Directory I have openend the folder that has the same name of my cell view. In this folder you will find a folder called "spectre" then in Spectre you find schematic folder, then netlist folder and finally you find input.spplog file. For example, my input.spplog is in this location:
/users/these/baccar/cadence/Sim/Simulation_THS4131_Cell/spectre/schematic/netlist

you find as attachement the pictures of input.spplog and the spectre.out

As you can see it's the same error when I try to type the spp command
//-- FATAL ERROR --// SPICE Reader: /.............Synatx Error caused by ""

I don't know how will be able to insert my spice block in schematic of cadence. I have tried the two follownig procedure but in the two case I have the same error. These are the two procedures:

----------------------------------------------------------------------------

*Problem:

In Composer, you would like to be able to create a symbol and
bind it directly to a text description netlist. How can you do this?

Your motivation is that you receive macro models for discrete

parts which you wish to simulate in conjunction with your on
chip devices. The macro models are in the form of text
SPICE subckt decks. Your current work around is to do a schematic
entry for the subcircuit. Unfortunately for larger subcircuits
this is not practical.


*Solution:

There are several ways to do this.

Procedure #1:


1. Convert the SPICE block using spp.

2. Open any schematic, select Design -> Create Cellview->From
pin list, and type in the destination symbol and pin list.

3. From the symbol view, choose Design->Save As, and save it as a spectre
view. Alternatively, use the Library Manager to copy the symbol view to the
spectre view.

4. Start Artist, and in the Setup -> Model Libraries form, include the path
to the converted text.

5. Set the model property on the block to be the same as the top-level
subcircuit name in the converted text. You will probably need to add the
model property. Just select the block, then choose Edit -> Properties ->
Objects. Next, Click on the Add button in the User Property section. For
"name", put "model", "type" should be "string", and you can leave the other
two fields blank. Under the Local Value on the Properties form, enter the
name of the top-level subcircuit.

What you have in the netlist is an instance statement for the block
representing the converted netlist that looks something like this:

X1 (ports) oa_rr

And a converted netlist that has a top-level subcircuit name that
corresponds to this.

Doing this with earlier versions than 4.4.3 gets complicated due to
name-mapping/subcircuit unfolding.



Procedure #2:

1. Create the schematic and add the needed pins, then create a symbol from that.
This is just to get the CDF parameters added automatically. You can also open
a schematic and then use Design->Create Cellview->From Pinlist... whichever
you want.

2. Make sure the terminal list in the CDF are correct and in the right
order. Check using (CIW) Tools->CDF->Edit... and enter the library/cellname
in the form.

3. In the CDF form change "CDF Type" from "effective" to "Base" (this is
to save the changes to disk).

4. Go to "Simulation information" and click Edit.

5. In the new form choose Spectre.

6. In the new form you will find componentName=subcircuit. Change this to
the exact name of your subcircuit netlist. Your spice netlist _must_ be a
subcircuit. Then OK both forms.

7. In the libManager, copy your symbol to a view called spectre. This is very
important.

8. Put your nice symbol in your schematic you want.

9. In Artist, find menu Setup->Environment... and "Use SPICE Netlist Reader(spp)".
Select "Y". This means your spice subcircuit will be translated to Spectre during
simulation.

10. Make sure your subcircuit file is added to the model library.
----------------------------------------------------------------------------
I hope someone help me
thanks

input.spplog

First of all , thanks a lot for the help from goldeboy huojinsi erikl.
Now I have found the origion of the problem,although i still haven't totally settle it. But at least i know the reason. That is I have loaded a wrong model for the schematic in ADE for spectre. A silly mistake!!
Again thanks all the people helped me

fatal error by spectre during circuit read-in

Thank you istyle. In fact I have contacted Cadence Support. They have said to me that the problem comrs from the fact that the file was used:edited in Windows. They have converted my netlist and sent it to me. I will post the exact answer of Cadence Suport after as soon as possible.

input.scs 16: statemen,t is not in spectre format

Well, it seams that's the problem is due to the fact that if spice netlist files are opened or edited in windows they can be no longer compatible uncer Unix. So it's better to download and open files in Linux systems and avoid to copy text files from WIndows to Unix, some problem of uncompatiblity may occur. So, to solve this problem, you can use dos2unix command.
I hope I have helped you