pwlf bus

P

pdw

Guest
Hi,

I want to use data from MATLAB as an input vector for my simulations.
In the past, I created a seperate pwlf source for each bit of the bus.
This worked good, for small small bus widths :).

Now my bus is becoming quite large (+64b).

What is the easiest way to import such data?

Pieter
 
pdw wrote, on 01/19/10 10:44:
Hi,

I want to use data from MATLAB as an input vector for my simulations.
In the past, I created a seperate pwlf source for each bit of the bus.
This worked good, for small small bus widths :).

Now my bus is becoming quite large (+64b).

What is the easiest way to import such data?

Pieter
Click to expand...
Pieter,

You didn't say which simulator you're using, but in Setup->Simulation Files in
ADE for spectre, aps and ultrasim, you can specify a "vector file". There's more
information on the format in the Ultrasim documentation, but it allows digital
vectors to be given to these simulators - connecting to a bus, for example.

Also "spectre -h vector" will tell you more about it.

Regards,

Andrew.
 
Hi Andrew,

thanks for the suggestion! I am using spectre (v 5.10.41.121508).
I tried using the vector file and it works using the Ultrasim
simulator.

If I try the spectre simulator, I get the following error in the icfb
window:

"*Error* Errors encountered during simulation. The simulator run log
has not been generated.
Possible cause could be an invalid command line option for the version
of the simulator
you are running. Choose Setup->Environment and verify that the command
line options
specified in the userCmdLineOption field are supported for the
simulator."

- Should I provide some extra options to spectre?
- Is the accuracy of Ultrasim simulations comparable to the results of
spectre simulations?

Regards,
Pieter

On Jan 19, 1:41 pm, Andrew Beckett <andr...@DcEaLdEeTnEcTe.HcIoSm>
wrote:
pdw wrote, on 01/19/10 10:44:

Hi,

I want to use data from MATLAB as an input vector for my simulations.
In the past, I created a seperate pwlf source for each bit of the bus.
This worked good, for small small bus widths :).

Now my bus is becoming quite large (+64b).

What is the easiest way to import such data?

Pieter

Pieter,

You didn't say which simulator you're using, but in Setup->Simulation Files in
ADE for spectre, aps and ultrasim, you can specify a "vector file". There's more
information on the format in the Ultrasim documentation, but it allows digital
vectors to be given to these simulators - connecting to a bus, for example.

Also "spectre -h vector" will tell you  more about it.

Regards,

Andrew.
Click to expand...
 
pdw wrote, on 01/20/10 08:40:
Hi Andrew,

thanks for the suggestion! I am using spectre (v 5.10.41.121508).
I tried using the vector file and it works using the Ultrasim
simulator.

If I try the spectre simulator, I get the following error in the icfb
window:

"*Error* Errors encountered during simulation. The simulator run log
has not been generated.
Possible cause could be an invalid command line option for the version
of the simulator
you are running. Choose Setup->Environment and verify that the command
line options
specified in the userCmdLineOption field are supported for the
simulator."

- Should I provide some extra options to spectre?
- Is the accuracy of Ultrasim simulations comparable to the results of
spectre simulations?

Regards,
Pieter
Click to expand...
Hi Pieter,

That's a really old version of spectre. spectre was originally shipped in the IC
releases, but since the end of 2004, it's been shipped in a new stream called
"MMSIM". Because IC5141 was already released, we've not taken it out, but there
have been no new enhancements in the spectre in IC5141 - just the occasional
serious bug fix. IC61 doesn't contain spectre - you _have_ to use MMSIM.

Ultrasim is also in MMSIM (it was never in IC5141), so the chances are you
already have it. Most likely all you need to do is put the MMSIM path before the
IC path (in your UNIX $PATH setup), and all will be OK. What version of Ultrasim
are you using?

Ultrasim is FASTSPICE simulator - it gets speed improvements by trading off
accuracy on (typically) selected blocks. So digital blocks don't need the same
accuracy as mixed-signal blocks, which don't need the same accuracy as analog
blocks (there's a range of modes and speed settings that can be picked on a
block-by-block basis).

Regards,

Andrew.
 
Hi,

I am using Ultrasim version 7.1.1.187.isr11.
I have been looking at the simulation options (ADE > Simulation >
Options > Analog) of Ultrasim a bit. Is it correct to assume that if
the simulation mode is set to Spice (s), the result will be the same
as a regular spectre simulation?

Regards,
Pieter


On Jan 20, 10:46 am, Andrew Beckett <andr...@DcEaLdEeTnEcTe.HcIoSm>
wrote:
pdw wrote, on 01/20/10 08:40:



Hi Andrew,

thanks for the suggestion! I am using spectre (v 5.10.41.121508).
I tried using the vector file and it works using the Ultrasim
simulator.

If I try the spectre simulator, I get the following error in the icfb
window:

"*Error* Errors encountered during simulation. The simulator run log
has not been generated.
Possible cause could be an invalid command line option for the version
of the simulator
you are running. Choose Setup->Environment and verify that the command
line options
specified in the userCmdLineOption field are supported for the
simulator."

- Should I provide some  extra options to spectre?
- Is the accuracy of Ultrasim simulations comparable to the results of
spectre simulations?

Regards,
Pieter

Hi Pieter,

That's a really old version of spectre. spectre was originally shipped in the IC
releases, but since the end of 2004, it's been shipped in a new stream called
"MMSIM". Because IC5141 was already released, we've not taken it out, but there
have been no new enhancements in the spectre in IC5141 - just the occasional
serious bug fix. IC61 doesn't contain spectre - you _have_ to use MMSIM.

Ultrasim is also in MMSIM (it was never in IC5141), so the chances are  you
already have it. Most likely all you need to do is put the MMSIM path before the
IC path (in your UNIX $PATH setup), and all will be OK. What version of Ultrasim
are you using?

Ultrasim is FASTSPICE simulator - it gets speed improvements by trading off
accuracy on (typically) selected blocks. So digital blocks don't need the same
accuracy as mixed-signal blocks, which don't need the same accuracy as analog
blocks (there's a range of modes and speed settings that can be picked on a
block-by-block basis).

Regards,

Andrew.
Click to expand...
 
pdw wrote, on 01/20/10 11:26:
Hi,

I am using Ultrasim version 7.1.1.187.isr11.
I have been looking at the simulation options (ADE > Simulation
Options > Analog) of Ultrasim a bit. Is it correct to assume that if
the simulation mode is set to Spice (s), the result will be the same
as a regular spectre simulation?

Regards,
Pieter
Click to expand...
Hi Pieter,

It probably should be, although it really doesn't make sense to use UltraSim in
fully SPICE mode - it won't be as fast as spectre, and that's not really what
UltraSim is intended for. The idea is that you use SPICE mode in very small
parts of the circuit which need the highest accuracy. Much of the time you don't
use SPICE mode at all with UltraSim.

Your Ultrasim version is reasonably recent, so it should just be a matter of
fixing your UNIX path to have <MMSIMinstDir>/tools/bin before
<IC5141instDir>/tools/bin and <IC5141instDir>/tools/dfII/bin

You really should do this, because you're missing out on a lot of spectre
improvements, enhancements, bug fixes, and speedups (e.g. spectre turbo) by
using such an old version.

Regards,

Andrew.
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top