AMS Designer Setup

Hi Riad and all,

Can you please help me to setup AMS Designer through HED oir ADE?
Currently, I am not able to access Sourcelink due to some unknown
reason. We have complained it to Cadence. Please help.

Thanks in advance.

Cheerssss!!!

Debjit.

 

Hi Debjit,

Sourcelink is not likely to be of that much help for this.
You better look at the AMS docs in your Cadence installation, i.e.
IUSHOME/doc/ams*

In recent versions of IC, (I'm assuming C 5.10.41.500.6.139) there is
a very good AMS workshop that is very good to start with. You have
both the database and the PDF file which are available in:

The AMS Virtuoso use model (AVUM) workshop is in
$CDSHOME/tools/dfII/samples/tutorials/AMS

the AVUM workshop is based on ADE with OSS based netlisting. That's
Cadence's recommendation and I would advise it too.
Anyway, don't waste your time, go to workshop and go through chapters
1-3. It is going to take 2 hours of your time and it's of a great
value.

In summury, running AMS in ADE is very simple, I would summrize in the
following steps:

I. The Pre-requisites
----------------------

1. the Cadence tools, i.e. IC stream and the IUS stream. the MMSIM
stream is not required to run AMS Designer. You can use following
versions of IC5141 and IUS82:
- IC 5.10.41.500.6.139
- IUS 08.20-s018
2. The Licenses
3. The cds.lib file: In addition to the design libraries, the Foundry
libraries and the Cadence's analogLib/basic libraries, user must
ensure they include:
- The Cadences's Sample library. This library contains all the
digital primitives. This library can be added as following: DEFINE
sample ${CDSHOME}/tools/dfII/samples/cdslib/sample
- The Cadences's built-in Connect Rules and Connect Modules library.
This library can be added as following: SOFTINCLUDE $AMSHOME/tools/
affirma_ams/etc/connect_lib/cds.lib
4. The Design: The Design in 5.X library structure, well your DFII
schematics ... etc.

II. The Steps
-------------

The main steps to run AMS Designer is:
1. Start a new UNIX terminal, browse to the working dir and acquire
the required tools and environment (maybe via sourcing a a setup file)
2. Launch Cadence (icms, icfb, or any of your inhouse scripts).
3. Open or create a config view for your design. Bear in mind to use
the AMS template when creating the config view. This is not mandatory
but is very handy to get the stop/switch view list suitable for AMS
Designer. Update the design hierarchy using the HED GUI at your
convenience and then save the config view. Please make sure that all
the cells and instances are well resolved in the HED. You are likely
to hit compilation and elaboration issues otherwise.
4. Open the schematic Top cell from the saved config view.
5. From the schematic, open the ADE GUI using Tools -> Analog
Environment
All the following steps are run from the Analog Environment Window,
ADE
- Setup the simulator to ams using ADE-> Setup -> Simulator -> ams
- Setup The analog Solver, if needed, using ADE -> Simulation ->
Solver. Spectre comes as default. AMS in ADE offers three analog
solvers: Spectre, Ultrasim and Aps
- Setup Netlister and run option using ADE -> Netlister and run
option. Cadence advises OSS. I would go for OSS too although I am
using Cell Based netlisting more often.
- run options = Either All (for small designs) or Incremental for big
databases
- simulation mode = Either Batch or Interactive. I’d rather use
Interactive to take benefit of controlling and debugging the
simulation using simvision
- Setup connects Rules if needed using ADE -> Setup -> Connect Rules.
By default, ADE comes with the 1v8 full fast. The following line
should be included in the cds.lib for this to happen: SOFTINCLUDE
$AMSHOME/tools/affirma_ams/etc/connect_lib/cds.lib Feel free to
customize the connect rules at you convenience.
Then
- Continue the simulation steps with setting up the usual
requirements, i.e. variables, Models, analyses and outputs.
- Run netlist and simulation.
- If netlisting, compile and elaboration steps all go fine, then
Simvision (if interactive option was chosen) would popup. Setup your
outputs and any other debug opton and then run the simulation.

Please do not hesitate to get in touch should you need any further
information.

One more thing. When you have errors, please (as advised by Andrew and
me in other posts) post
1. your tool versions, i.e.
icfb -W
nchelp -v
spectre -W (not really needed in here)
2. The exact error message
3. The source code when it applies.

This would really save our time is we are busy sorting our daily work
as you would have imagined.

That's it, I need to go for lunch now !
Cheers,
Riad.

 

Hi Riad,

Many many thanks!!!! It worked.. I have set up the AMS designer and
simulated some of the designs. It worked fine... I preffered the ADE
based AMS Designer. I will look into the tutorial as soon as possible.
Many many thanks.!!!!

Regards,

Cheers!!!
Debjit