Music to Ppice

R

reaman4ever

Guest
How do I convert a music file into something pspice can use? I figured
out that I can use the VPWL_FILE if I have a .txt with a time and
voltage column, but how do I create that .txt file?
Thanks
 
"reaman4ever" <agielchinsky@gmail-dot-com.no-spam.invalid> wrote in message
news:449b2ce2$0$14810$892e7fe2@authen.yellow.readfreenews.net...
How do I convert a music file into something pspice can use? I figured
out that I can use the VPWL_FILE if I have a .txt with a time and
voltage column, but how do I create that .txt file?
Click to expand...
Do you have access to Matlab? It'll happily read in .WAV files and write out
the type of text file you're after.
 
reaman4ever,

How do I convert a music file into something
pspice can use? I figured out that I can use
the VPWL_FILE if I have a .txt with a time and
voltage column, but how do I create that .txt file?

How do I convert a music file into something pspice
can use? I figured out that I can use the VPWL_FILE
if I have a .txt with a time and voltage column, but
how do I create that .txt file?
Click to expand...
FYI, LTspice can directly play .wav files into your
simulation. The syntax is

V1 X 0 wavefile=.\ring.wav chan=0

Example using the technique are installed as
C:/Programme/LTC/SwCADIII/examples/Educational/{wavein.asc,waveout.asc}

--Mike
 
[/quote]
Do you have access to Matlab? It'll happily read in .WAV files and
write out
the type of text file you're after.[/quote]

Yes I do, How do I do that?
Thank you
 
On Fri, 23 Jun 2006 01:57:17 GMT, "Mike Engelhardt" <nospam@spam.org>
wrote:

reaman4ever,

How do I convert a music file into something
pspice can use? I figured out that I can use
the VPWL_FILE if I have a .txt with a time and
voltage column, but how do I create that .txt file?

How do I convert a music file into something pspice
can use? I figured out that I can use the VPWL_FILE
if I have a .txt with a time and voltage column, but
how do I create that .txt file?

FYI, LTspice can directly play .wav files into your
simulation. The syntax is

V1 X 0 wavefile=.\ring.wav chan=0

Example using the technique are installed as
C:/Programme/LTC/SwCADIII/examples/Educational/{wavein.asc,waveout.asc}

--Mike
Click to expand...
Mike,

Will it create a PWL file, or is it internal use only?

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Jim,

FYI, LTspice can directly play .wav files into
your simulation. The syntax is

V1 X 0 wavefile=.\ring.wav chan=0

Example using the technique are installed as
C:/Programme/LTC/SwCADIII/examples/Educational
/{wavein.asc,waveout.asc}

Will it create a PWL file, or is it internal
use only?
Click to expand...
LTspice can read/write .wav files. This is so
you can play a track of music from a .wav into a
simulated HiFi amp while writing the amp's output
to another .wav file. (Then you can replace the
tubes with transistors and see if you like that
sound better -- all without getting near any
hardware.)

LTspice can also do the PSpice "PWL FILE=..."
syntax. But to create that file you'd have to
export the simulation data to a file and delete
the header with data labels to get the format you
need for the "PWL FILE=..." syntax.

--Mike
 
On Fri, 23 Jun 2006 20:13:36 GMT, "Mike Engelhardt" <nospam@spam.org>
wrote:

Jim,

FYI, LTspice can directly play .wav files into
your simulation. The syntax is

V1 X 0 wavefile=.\ring.wav chan=0

Example using the technique are installed as
C:/Programme/LTC/SwCADIII/examples/Educational
/{wavein.asc,waveout.asc}

Will it create a PWL file, or is it internal
use only?

LTspice can read/write .wav files. This is so
you can play a track of music from a .wav into a
simulated HiFi amp while writing the amp's output
to another .wav file. (Then you can replace the
tubes with transistors and see if you like that
sound better -- all without getting near any
hardware.)

LTspice can also do the PSpice "PWL FILE=..."
syntax. But to create that file you'd have to
export the simulation data to a file and delete
the header with data labels to get the format you
need for the "PWL FILE=..." syntax.

--Mike
Click to expand...
Mike,

How do you get the simulation data into ASCII format? (PSpice has a
block to check for CSDF, but I couldn't find a similar setting in
LTSpice.)

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Jim,

FYI, LTspice can directly play .wav files
into your simulation. The syntax is

V1 X 0 wavefile=.\ring.wav chan=0

Example using the technique are installed as
C:/Programme/LTC/SwCADIII/examples/Educational
/{wavein.asc,waveout.asc}

Will it create a PWL file, or is it internal
use only?

LTspice can read/write .wav files. This is so
you can play a track of music from a .wav into a
simulated HiFi amp while writing the amp's output
to another .wav file. (Then you can replace the
tubes with transistors and see if you like that
sound better -- all without getting near any
hardware.)

LTspice can also do the PSpice "PWL FILE=..."
syntax. But to create that file you'd have to
export the simulation data to a file and delete
the header with data labels to get the format you
need for the "PWL FILE=..." syntax.

How do you get the simulation data into ASCII format?
(PSpice has a block to check for CSDF, but I couldn't
find a similar setting in LTSpice.)
Click to expand...
You export the data from the waveform viewer:
(Active waveform window)=>File Export. You get
a file of time, value pairs that can be used as
the input for a source using the "PWL FILE=..."
syntax. Except you have to remove the first line
of this file which will look something like
time V(n001)
0.000000e+000 1.000000e+000
1.012000e-006 1.200000e-002
2.012000e-006 9.880000e-001
3.012000e-006 1.200000e-002

--Mike
 
On Sat, 24 Jun 2006 04:07:56 GMT, "Mike Engelhardt" <nospam@spam.org>
wrote:

Jim,

FYI, LTspice can directly play .wav files
into your simulation. The syntax is

V1 X 0 wavefile=.\ring.wav chan=0

Example using the technique are installed as
C:/Programme/LTC/SwCADIII/examples/Educational
/{wavein.asc,waveout.asc}

Will it create a PWL file, or is it internal
use only?

[snip]

You export the data from the waveform viewer:
(Active waveform window)=>File Export. You get
a file of time, value pairs that can be used as
the input for a source using the "PWL FILE=..."
syntax. Except you have to remove the first line
of this file which will look something like
time V(n001)
0.000000e+000 1.000000e+000
1.012000e-006 1.200000e-002
2.012000e-006 9.880000e-001
3.012000e-006 1.200000e-002

--Mike
Click to expand...
OK. Found it. Thanks!

Turns out that PSpice can export like that as well to a *.txt file.
I'd just never used it... my usual way was to simply ctrl-C a waveform
and paste into Excel.

The reading-in of *.wav files is a super idea!

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
"Jim Thompson" <To-Email-Use-The-Envelope-Icon@My-Web-Site.com> a écrit dans
le message de news:c0nq921n9248s9nudk95pb8uil1tgc8k9a@4ax.com...
On Sat, 24 Jun 2006 04:07:56 GMT, "Mike Engelhardt" <nospam@spam.org
wrote:

Jim,

FYI, LTspice can directly play .wav files
into your simulation. The syntax is

V1 X 0 wavefile=.\ring.wav chan=0

Example using the technique are installed as
C:/Programme/LTC/SwCADIII/examples/Educational
/{wavein.asc,waveout.asc}

Will it create a PWL file, or is it internal
use only?

[snip]

You export the data from the waveform viewer:
(Active waveform window)=>File Export. You get
a file of time, value pairs that can be used as
the input for a source using the "PWL FILE=..."
syntax. Except you have to remove the first line
of this file which will look something like
time V(n001)
0.000000e+000 1.000000e+000
1.012000e-006 1.200000e-002
2.012000e-006 9.880000e-001
3.012000e-006 1.200000e-002

--Mike


OK. Found it. Thanks!

Turns out that PSpice can export like that as well to a *.txt file.
I'd just never used it... my usual way was to simply ctrl-C a waveform
and paste into Excel.

The reading-in of *.wav files is a super idea!
Click to expand...
Intusoft can do that too.

Maybe it's time to do a simulator's sound contest: same amplifier design,
different simulator. Which simulator sounds best?


--
Thanks,
Fred.
 
On Mon, 26 Jun 2006 21:07:54 +0200, "Fred Bartoli"
<fred._canxxxel_this_bartoli@RemoveThatAlso_free.fr_AndThisToo> wrote:

[snippage]
Maybe it's time to do a simulator's sound contest: same amplifier design,
different simulator. Which simulator sounds best?
Click to expand...
Obviously, a computer using an Intel processor will sound better due
to the thermal emission characteristics of the CPU!
 
Thanks
Does anyone know how to get pspice to take sample points at exactly a
certain sample rate?
 
On 29 Jun 2006 17:15:42 GMT,
agielchinsky@gmail-dot-com.no-spam.invalid (reaman4ever) wrote:

Thanks
Does anyone know how to get pspice to take sample points at exactly a
certain sample rate?
Click to expand...
Depends on what you mean by "sample".

If you use a .PRINT statement, you can specify the timestep for which
data is recorded.

This data will appear in the .OUT file

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top