Designer’s Guide Community

Stefan Senior Member Offline Posts: 124	Check Simulator Settings from within module Jan 23^rd, 2008, 2:55pm Hi, does anyone know if it's possible to check the simulator options from within a module ? In the special case, I need to know the settings of fmax of transient noise in AMS (spectre solver). Kind regards, Stefan
Back to top	IP Logged

Geoffrey_Coram Senior Fellow Offline Posts: 1999 Massachusetts, USA	Re: Check Simulator Settings from within module Reply #1 - Jan 28^th, 2008, 6:54am Verilog-AMS LRM 2.2 added the $simparam() system function to get values from the simulator; GMIN, for example, is explicitly mentioned. FMAX is not, so you'd have to check with your simulator vendor and probably request an enhancement.
Back to top	If at first you do succeed, STOP, raise your standards, and stop wasting your time. IP Logged

Marq Kole Senior Member Offline Hmmm. That's weird... Posts: 122 Eindhoven, The Netherlands	Re: Check Simulator Settings from within module Reply #2 - Mar 19^th, 2008, 2:44pm An approach that works in Spectre is to define a parameter with the fmax value and pass it to the model and to the relevant option of the transient analysis instance. Cheers, Marq
Back to top	IP Logged

Geoffrey_Coram

Senior Fellow

Offline

Posts: 1999
Massachusetts, USA

Re: Check Simulator Settings from within module
Reply #3 - Mar 20^th, 2008, 6:11am

Marq -
That approach might work OK if you are writing the netlist. But if you're developing a Verilog-A model for use in other people's simulations, and they use ADE to generate the netlist for Spectre (where ADE is responsible for taking the FMAX value from a box on the GUI form and putting it in the netlist), then I don't think your approach is viable.

-Geoffrey

Back to top

If at first you do succeed, STOP, raise your standards, and stop wasting your time.

IP Logged

jbdavid

Community Fellow

Offline

Posts: 378
Silicon Valley

Re: Check Simulator Settings from within module
Reply #4 - Apr 13^th, 2008, 11:42pm

I was hoping that the $simparam would let me access ANY variable in the Model files used by the underlying spice simulator..
for the LAST project where I needed to get the values of modelfile parameters into the models, I created special subcircuits
in the model files with voltage sources set to the parameter value..
then instantiated those in my model.. and used the voltage connection read the parameter value.
-- in a large design where I might have many models needing this value it would be quite inefficient.
but it was something that I could do that day with things under my control.

-- now maybe the LRM couldn't tell me about these variables because it relates to a specific simulator function..
but I hopefully simulators will provide more such values..
--
Alternately, I might do something with a netlist pre-processor.. but that might limit the use of something in a corners tool situation.
jbd

Back to top

jbdavid
Mixed Signal Design Verification

IP Logged