The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Simulate with netlist using spectre in ADE
https://designers-guide.org/forum/YaBB.pl?num=1198763559

Message started by ywguo on Dec 27^th, 2007, 5:52am

Title: Simulate with netlist using spectre in ADE
Post by ywguo on Dec 27^th, 2007, 5:52am

Hi Guys,

I am testing a DAC. An LM7372 differential amplifier is put at the DAC output to buffer the 50 Ohm load. I have got the spice model of LM7372 at national semiconductor website. How do I simulate the DAC and LM7372 together in ADE? I have schemtic of the DAC, but the spice model of LM7372 is netlist only.

Thanks
Yawei

Title: Re: Simulate with netlist using spectre in ADE
Post by rajdeep on Dec 27^th, 2007, 9:29am

Hi,
You can create a VerilogAMS view of the diffamp.
This diffamp would have the same interface as the spice level design you have.
It is just a wrapper. Then instantiate the diffamp as a subckt. It is possible to
use a spice/spectre subcircuit from a verilogAMS model. Then create a symbol of it and use it with
the DAC.

There are some issues though which I donot know offhand..
1. If you want to use spectre as the simulator, you have to use VerilogA instead of VerilogAMS. I hope
one can instantiate a spctre/spice subckt in a verilogA module also. I have never tried the latter though/

2. How will you include the spice netlist of diffamp?? I once simulated a design, partly in spectre and VerilogAMS, but I used command line interface, i.e. ncsim -ams. I included the subckt definition in a file named hdl.var as below:

Quote:

define MODELPATH ldotest/SpectreFiles/<netlist.scs>

There must be some way to tell the simualtor from where pick up this subckt definition using some option
of ADE, or may be it can be included in the verilogA/MS file iteself using include directive!! Not sure though.

Hope that helps.
Rajdeep

Title: Re: Simulate with netlist using spectre in ADE
Post by ywguo on Jan 4^th, 2008, 4:50am

Hi Rajdeep,

I have a simpler method now, that SPICE model is included in the spectre netlist when simulate in ADE. Open ADE, click Setup -> Simulation Files ... . Fill in the Include path and Stimulus File. Then click the button netlist and run.

An example of the stimulus file is shown below.

Code:

.include 'LM7372.MOD'
XOP1 IN- IN+ V+ V- OUT_Q LM7372
R1 OUT_QN IN- 200
R2 IN- OUTQ 200
R3 OUT_QP IN+ 200
R4 IN+ 0 200
V+ V+ 0 5
V- V- 0 -5
RL OUT_Q 0 50

.PLOT V(IN+) V(IN-) V(V+) V(V-) V(OUT_Q)

Thank you, Rajdeep.

Yawei

Title: Re: Simulate with netlist using spectre in ADE
Post by Frank Wiedmann on Jan 4^th, 2008, 5:32am

Another alternative would be to convert the netlist from SPICE to Spectre with spp and then use the scasubckt component as described in http://www.designers-guide.org/Forum/YaBB.pl?num=1191334088/1#1. A slightly simplified version of this component is offered at http://sourcelink.cadence.com/docs/db/kdb/2003/Nov/11013814.html.