|
I have a filter with some sharp notches and flat pass-bands. I want to be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k (transition band)
How do I do this in LTspice...?
Cheers
A. Ganesan
|
I forgot to add, I don't know how to do variable resolution for
transient analysis either...
Cheers
A. Ganesan
toggle quoted message
Show quoted text
On 9/10/2011 4:43 PM, Apparajan wrote:
I have a filter with some sharp notches and flat pass-bands. I want to
be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply
rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k (transition
band)
How do I do this in LTspice...?
Cheers
A. Ganesan
|
--- In LTspice@..., Ganesan <dg1@...> wrote:
I forgot to add, I don't know how to do variable resolution for
transient analysis either...
Cheers
A. Ganesan
On 9/10/2011 4:43 PM, Apparajan wrote:
I have a filter with some sharp notches and flat pass-bands. I want to
be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply
rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k (transition
band)
How do I do this in LTspice...?
Cheers
A. Ganesan
Hello, There is only the option of lin, dec, oct and list in the .AC-command. This means you would have to use "list", but it would be a big effort to create the 10000 or more frequency values. The AC-simulation runs so fast, that you can simulate the whole span with high resolution, even if you end with 100000 or more frequency-points. I also don't know of any simple solution for .TRAN. A possible workaround may be a dummy-source creating bursts. This may force the automatic timestep calculator in LTspice to reduce the time step. Best regards, Helmut
|
Thanks.. I didn't know "list" works with .ac.. Is this in the help
file.? My filter is of 46th order.. So could take a while..
By the way does list work with .tran too?
Cheers
A. Ganesan
toggle quoted message
Show quoted text
On 9/10/2011 6:16 PM, Helmut wrote:
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>,
Ganesan <dg1@...> wrote:
I forgot to add, I don't know how to do variable resolution for
transient analysis either...
Cheers
A. Ganesan
On 9/10/2011 4:43 PM, Apparajan wrote:
I have a filter with some sharp notches and flat pass-bands. I
want to
be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply
rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k (transition
band)
How do I do this in LTspice...?
Cheers
A. Ganesan
Hello,
There is only the option of lin, dec, oct and list in the
.AC-command. This means you would have to use "list", but it
would be a big effort to create the 10000 or more frequency
values.
The AC-simulation runs so fast, that you can simulate the
whole span with high resolution, even if you end with 100000
or more frequency-points.
I also don't know of any simple solution for .TRAN.
A possible workaround may be a dummy-source creating bursts.
This may force the automatic timestep calculator in LTspice
to reduce the time step.
Best regards,
Helmut
|
The list seems to work..But the interpolated output on the plot looks
funky... I can live with it..
Cheers
A. Ganesan
toggle quoted message
Show quoted text
On 9/10/2011 6:16 PM, Helmut wrote:
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>,
Ganesan <dg1@...> wrote:
I forgot to add, I don't know how to do variable resolution for
transient analysis either...
Cheers
A. Ganesan
On 9/10/2011 4:43 PM, Apparajan wrote:
I have a filter with some sharp notches and flat pass-bands. I
want to
be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply
rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k (transition
band)
How do I do this in LTspice...?
Cheers
A. Ganesan
Hello,
There is only the option of lin, dec, oct and list in the
.AC-command. This means you would have to use "list", but it
would be a big effort to create the 10000 or more frequency
values.
The AC-simulation runs so fast, that you can simulate the
whole span with high resolution, even if you end with 100000
or more frequency-points.
I also don't know of any simple solution for .TRAN.
A possible workaround may be a dummy-source creating bursts.
This may force the automatic timestep calculator in LTspice
to reduce the time step.
Best regards,
Helmut
|
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
===================================================================================
toggle quoted message
Show quoted text
On 9/10/2011 6:41 PM, Ganesan wrote:
The list seems to work..But the interpolated output on the plot looks
funky... I can live with it..
Cheers
A. Ganesan
On 9/10/2011 6:16 PM, Helmut wrote:
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>,
Ganesan <dg1@...> wrote:
I forgot to add, I don't know how to do variable resolution for
transient analysis either...
Cheers
A. Ganesan
On 9/10/2011 4:43 PM, Apparajan wrote:
I have a filter with some sharp notches and flat pass-bands. I
want to
be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply
rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k
(transition
band)
How do I do this in LTspice...?
Cheers
A. Ganesan
Hello,
There is only the option of lin, dec, oct and list in the
.AC-command. This means you would have to use "list", but it
would be a big effort to create the 10000 or more frequency
values.
The AC-simulation runs so fast, that you can simulate the
whole span with high resolution, even if you end with 100000
or more frequency-points.
I also don't know of any simple solution for .TRAN.
A possible workaround may be a dummy-source creating bursts.
This may force the automatic timestep calculator in LTspice
to reduce the time step.
Best regards,
Helmut
No virus found in this incoming message.
Checked by AVG - www.avg.com
Version: 9.0.901 / Virus Database: 271.1.1/3889 - Release Date: 09/10/11 13:44:00
|
--- In LTspice@..., Ganesan <dg1@...> wrote:
...My filter is of 46th order..
any practical use for that? hws
|
Has been in production for a while..
toggle quoted message
Show quoted text
On 9/11/2011 9:30 AM, Heinz-W. Schockenbaum wrote:
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>,
Ganesan <dg1@...> wrote:
...My filter is of 46th order..
any practical use for that?
hws
|
In message <j4igm8+9gih@...>, dated Sun, 11 Sep 2011, Heinz-W. Schockenbaum <schockenbaum@...> writes: --- In LTspice@..., Ganesan <dg1@...> wrote:
...My filter is of 46th order..
any practical use for that? Keeping component manufacturers in business? -- OOO - Own Opinions Only. Try www.jmwa.demon.co.uk and www.isce.org.uk John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK When I point to a star, please look at the star, not my finger. The star will be more interesting.
|
I am re posting this since I didn't get aye or nay...
Cheers
AG
toggle quoted message
Show quoted text
On 9/10/2011 6:46 PM, Ganesan wrote:
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
===================================================================================
On 9/10/2011 6:41 PM, Ganesan wrote:
The list seems to work..But the interpolated output on the plot looks
funky... I can live with it..
Cheers
A. Ganesan
On 9/10/2011 6:16 PM, Helmut wrote:
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>,
Ganesan <dg1@...> wrote:
I forgot to add, I don't know how to do variable resolution for
transient analysis either...
Cheers
A. Ganesan
On 9/10/2011 4:43 PM, Apparajan wrote:
I have a filter with some sharp notches and flat pass-bands. I
want to
be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply
rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k
(transition
band)
How do I do this in LTspice...?
Cheers
A. Ganesan
Hello,
There is only the option of lin, dec, oct and list in the
.AC-command. This means you would have to use "list", but it
would be a big effort to create the 10000 or more frequency
values.
The AC-simulation runs so fast, that you can simulate the
whole span with high resolution, even if you end with 100000
or more frequency-points.
I also don't know of any simple solution for .TRAN.
A possible workaround may be a dummy-source creating bursts.
This may force the automatic timestep calculator in LTspice
to reduce the time step.
Best regards,
Helmut
|
<snip> --- In LTspice@..., Ganesan <dg1@...> wrote:
I am re posting this since I didn't get aye or nay...
Cheers
AG
On 9/10/2011 6:46 PM, Ganesan wrote:
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
===================================================================================
</snip> Hello Ganesan, There at least two ways to do this. The first one is very clunky, and you might not want to do it more than once or twice, depending on how patient you are. Export the waveform data of each plot (File>Export), and then combine the data in Excel. You can use Excel's Data>Sort feature to sort the points into order of increasing frequency. Be aware, though, that some versions of Excel only support 20,000 points in a chart series. Alternatively, you can use Helmut's ltsputils program, which can read and reformat raw files. This is a Perl command line program, but there is also a GUI front end available for this. Search the Files section for these and lots of other useful utilities and add-ons. Help that helps. Regards, Tony
|
AG,
I don't know how to do this sort of thing within LTspice However, the proprietary binary output of LTspice is SpiceExplorer compatible, so I use SpiceExplorer as the waveform viewer for anything like this.
I know SpiceExplorer is not free, but it is a very useful tool.
regards
Robert
toggle quoted message
Show quoted text
--- In LTspice@..., "Tony Casey" <tony@...> wrote:
<snip>
--- In LTspice@..., Ganesan <dg1@> wrote:
I am re posting this since I didn't get aye or nay...
Cheers
AG
On 9/10/2011 6:46 PM, Ganesan wrote:
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
===================================================================================
</snip>
Hello Ganesan,
There at least two ways to do this. The first one is very clunky, and you might not want to do it more than once or twice, depending on how patient you are. Export the waveform data of each plot (File>Export), and then combine the data in Excel. You can use Excel's Data>Sort feature to sort the points into order of increasing frequency. Be aware, though, that some versions of Excel only support 20,000 points in a chart series.
Alternatively, you can use Helmut's ltsputils program, which can read and reformat raw files. This is a Perl command line program, but there is also a GUI front end available for this.
Search the Files section for these and lots of other useful utilities and add-ons.
Help that helps.
Regards,
Tony
|
Thanks..will get back in a few days..
Cheers
AG
On 9/14/2011 3:28 AM, RobertTalty wrote:I am re posting this since I
didn't get aye or nay...
Cheers
AG
toggle quoted message
Show quoted text
On 9/10/2011 6:46 PM, Ganesan wrote:
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
===================================================================================
On 9/10/2011 6:41 PM, Ganesan wrote:
The list seems to work..But the interpolated output on the plot looks
funky... I can live with it..
Cheers
A. Ganesan
On 9/10/2011 6:16 PM, Helmut wrote:
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>,
Ganesan <dg1@...> wrote:
I forgot to add, I don't know how to do variable resolution for
transient analysis either...
Cheers
A. Ganesan
On 9/10/2011 4:43 PM, Apparajan wrote:
I have a filter with some sharp notches and flat pass-bands. I
want to
be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply
rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k
(transition
band)
How do I do this in LTspice...?
Cheers
A. Ganesan
Hello,
There is only the option of lin, dec, oct and list in the
.AC-command. This means you would have to use "list", but it
would be a big effort to create the 10000 or more frequency
values.
The AC-simulation runs so fast, that you can simulate the
whole span with high resolution, even if you end with 100000
or more frequency-points.
I also don't know of any simple solution for .TRAN.
A possible workaround may be a dummy-source creating bursts.
This may force the automatic timestep calculator in LTspice
to reduce the time step.
Best regards,
Helmut
AG,
I don't know how to do this sort of thing within LTspice However, the
proprietary binary output of LTspice is SpiceExplorer compatible, so
I use SpiceExplorer as the waveform viewer for anything like this.
I know SpiceExplorer is not free, but it is a very useful tool.
regards
Robert
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>,
"Tony Casey" <tony@...> wrote:
<snip>
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>,
Ganesan <dg1@> wrote:
I am re posting this since I didn't get aye or nay...
Cheers
AG
On 9/10/2011 6:46 PM, Ganesan wrote:
I can run different ac simulations with different frequency
resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
===================================================================================
</snip>
Hello Ganesan,
There at least two ways to do this. The first one is very clunky, and you might not want to do it more than once or twice, depending on
how patient you are. Export the waveform data of each plot
(File>Export), and then combine the data in Excel. You can use
Excel's Data>Sort feature to sort the points into order of increasing
frequency. Be aware, though, that some versions of Excel only support
20,000 points in a chart series.
Alternatively, you can use Helmut's ltsputils program, which can
read and reformat raw files. This is a Perl command line program, but
there is also a GUI front end available for this.
Search the Files section for these and lots of other useful
utilities and add-ons.
Help that helps.
Regards,
Tony
|
LTspice doesn't have any built in capability for merging data. However, you can export the data and then use a program like Octave, Scilab or Matlab to merge the data. The data would be represented as vectors in these programs and vectors can be concatenated. With either Octave or Scilab you are working with ASCII data. Whereas with NAtlab you could use LTspice2Matlab, keep the data in binary format and gain the benefit of smaller file sizes. In addition you can zoom in and out in plots in Matlab.
Howard
toggle quoted message
Show quoted text
On 9/13/2011 10:38 PM, Ganesan wrote: I am re posting this since I didn't get aye or nay...
Cheers
AG
On 9/10/2011 6:46 PM, Ganesan wrote:
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
===================================================================================
On 9/10/2011 6:41 PM, Ganesan wrote:
The list seems to work..But the interpolated output on the plot looks
funky... I can live with it..
Cheers
A. Ganesan
On 9/10/2011 6:16 PM, Helmut wrote:
--- In LTspice@...<mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>,
Ganesan<dg1@...> wrote:
I forgot to add, I don't know how to do variable resolution for
transient analysis either...
Cheers
A. Ganesan
On 9/10/2011 4:43 PM, Apparajan wrote:
I have a filter with some sharp notches and flat pass-bands. I want to
be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply
rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k
(transition
band)
How do I do this in LTspice...?
Cheers
A. Ganesan
Hello,
There is only the option of lin, dec, oct and list in the
.AC-command. This means you would have to use "list", but it
would be a big effort to create the 10000 or more frequency
values.
The AC-simulation runs so fast, that you can simulate the
whole span with high resolution, even if you end with 100000
or more frequency-points.
I also don't know of any simple solution for .TRAN.
A possible workaround may be a dummy-source creating bursts.
This may force the automatic timestep calculator in LTspice
to reduce the time step.
Best regards,
Helmut
------------------------------------
Yahoo! Groups Links
|
Thanks.. What freeware will meet my needs..? (I am a windows XP guy)
cheers
AG
toggle quoted message
Show quoted text
On 9/14/2011 9:18 AM, Howard Hansen wrote:
LTspice doesn't have any built in capability for merging data. However,
you can export the data and then use a program like Octave, Scilab or
Matlab to merge the data. The data would be represented as vectors in
these programs and vectors can be concatenated. With either Octave or
Scilab you are working with ASCII data. Whereas with NAtlab you could
use LTspice2Matlab, keep the data in binary format and gain the benefit
of smaller file sizes. In addition you can zoom in and out in plots in
Matlab.
Howard
On 9/13/2011 10:38 PM, Ganesan wrote:
I am re posting this since I didn't get aye or nay...
Cheers
AG
On 9/10/2011 6:46 PM, Ganesan wrote:
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
===================================================================================
On 9/10/2011 6:41 PM, Ganesan wrote:
The list seems to work..But the interpolated output on the plot looks
funky... I can live with it..
Cheers
A. Ganesan
On 9/10/2011 6:16 PM, Helmut wrote:
--- In LTspice@...
<mailto:LTspice%40yahoogroups.com><mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>,
Ganesan<dg1@...> wrote:
I forgot to add, I don't know how to do variable resolution for
transient analysis either...
Cheers
A. Ganesan
On 9/10/2011 4:43 PM, Apparajan wrote:
I have a filter with some sharp notches and flat pass-bands. I want to
be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply
rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k
(transition
band)
How do I do this in LTspice...?
Cheers
A. Ganesan
Hello,
There is only the option of lin, dec, oct and list in the
.AC-command. This means you would have to use "list", but it
would be a big effort to create the 10000 or more frequency
values.
The AC-simulation runs so fast, that you can simulate the
whole span with high resolution, even if you end with 100000
or more frequency-points.
I also don't know of any simple solution for .TRAN.
A possible workaround may be a dummy-source creating bursts.
This may force the automatic timestep calculator in LTspice
to reduce the time step.
Best regards,
Helmut
------------------------------------
Yahoo! Groups Links
No virus found in this incoming message.
Checked by AVG - www.avg.com
Version: 9.0.914 / Virus Database: 271.1.1/3896 - Release Date: 09/14/11 01:34:00
|
Both Octave and Scilab are freeware.
Howard
toggle quoted message
Show quoted text
On 9/14/2011 9:25 AM, Ganesan wrote: Thanks.. What freeware will meet my needs..? (I am a windows XP guy)
cheers
AG
On 9/14/2011 9:18 AM, Howard Hansen wrote:
LTspice doesn't have any built in capability for merging data. However,
you can export the data and then use a program like Octave, Scilab or
Matlab to merge the data. The data would be represented as vectors in
these programs and vectors can be concatenated. With either Octave or
Scilab you are working with ASCII data. Whereas with NAtlab you could
use LTspice2Matlab, keep the data in binary format and gain the benefit
of smaller file sizes. In addition you can zoom in and out in plots in
Matlab.
Howard
On 9/13/2011 10:38 PM, Ganesan wrote:
I am re posting this since I didn't get aye or nay...
Cheers
AG
On 9/10/2011 6:46 PM, Ganesan wrote:
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
===================================================================================
On 9/10/2011 6:41 PM, Ganesan wrote:
The list seems to work..But the interpolated output on the plot looks
funky... I can live with it..
Cheers
A. Ganesan
On 9/10/2011 6:16 PM, Helmut wrote:
--- In LTspice@...
<mailto:LTspice%40yahoogroups.com><mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>,
Ganesan<dg1@...> wrote:
I forgot to add, I don't know how to do variable resolution for
transient analysis either...
Cheers
A. Ganesan
On 9/10/2011 4:43 PM, Apparajan wrote:
I have a filter with some sharp notches and flat pass-bands. I want to
be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply
rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k
(transition
band)
How do I do this in LTspice...?
Cheers
A. Ganesan
Hello,
There is only the option of lin, dec, oct and list in the
.AC-command. This means you would have to use "list", but it
would be a big effort to create the 10000 or more frequency
values.
The AC-simulation runs so fast, that you can simulate the
whole span with high resolution, even if you end with 100000
or more frequency-points.
I also don't know of any simple solution for .TRAN.
A possible workaround may be a dummy-source creating bursts.
This may force the automatic timestep calculator in LTspice
to reduce the time step.
Best regards,
Helmut
------------------------------------
Yahoo! Groups Links
No virus found in this incoming message.
Checked by AVG - www.avg.com
Version: 9.0.914 / Virus Database: 271.1.1/3896 - Release Date: 09/14/11 01:34:00
------------------------------------
Yahoo! Groups Links
|
Thanks
A. Ganesan
toggle quoted message
Show quoted text
On 9/14/2011 12:25 PM, Howard Hansen wrote:
Both Octave and Scilab are freeware.
Howard
On 9/14/2011 9:25 AM, Ganesan wrote:
Thanks.. What freeware will meet my needs..? (I am a windows XP guy)
cheers
AG
On 9/14/2011 9:18 AM, Howard Hansen wrote:
LTspice doesn't have any built in capability for merging data. However,
you can export the data and then use a program like Octave, Scilab or
Matlab to merge the data. The data would be represented as vectors in
these programs and vectors can be concatenated. With either Octave or
Scilab you are working with ASCII data. Whereas with NAtlab you could
use LTspice2Matlab, keep the data in binary format and gain the benefit
of smaller file sizes. In addition you can zoom in and out in plots in
Matlab.
Howard
On 9/13/2011 10:38 PM, Ganesan wrote:
I am re posting this since I didn't get aye or nay...
Cheers
AG
On 9/10/2011 6:46 PM, Ganesan wrote:
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
===================================================================================
On 9/10/2011 6:41 PM, Ganesan wrote:
The list seems to work..But the interpolated output on the plot
looks
funky... I can live with it..
Cheers
A. Ganesan
On 9/10/2011 6:16 PM, Helmut wrote:
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com><mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>
<mailto:LTspice%40yahoogroups.com>,
Ganesan<dg1@...> wrote:
I forgot to add, I don't know how to do variable resolution for
transient analysis either...
Cheers
A. Ganesan
On 9/10/2011 4:43 PM, Apparajan wrote:
I have a filter with some sharp notches and flat pass-bands. I want to
be able to simulate it with variable resolution.
For example
.ac lin 10 20 50 lin 1000 50 70 oct 20 70 3k lin 1000 3k 3.8k
(linearly sweep the frequency 10 points from 20 to 50 hz;
high resolution of 1000 points between 50 to 70 HZ ( power supply
rejection notch;
Flat region from 70 to 3 khz and
a high resolution sweep of 1000points between 3k and 3.8k
(transition
band)
How do I do this in LTspice...?
Cheers
A. Ganesan
Hello,
There is only the option of lin, dec, oct and list in the
.AC-command. This means you would have to use "list", but it
would be a big effort to create the 10000 or more frequency
values.
The AC-simulation runs so fast, that you can simulate the
whole span with high resolution, even if you end with 100000
or more frequency-points.
I also don't know of any simple solution for .TRAN.
A possible workaround may be a dummy-source creating bursts.
This may force the automatic timestep calculator in LTspice
to reduce the time step.
Best regards,
Helmut
------------------------------------
Yahoo! Groups Links
No virus found in this incoming message.
Checked by AVG - www.avg.com
Version: 9.0.914 / Virus Database: 271.1.1/3896 - Release Date:
09/14/11 01:34:00
|
<snip> --- In LTspice@..., Ganesan <dg1@...> wrote:
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
</snip> Hello Ganesan, I just thought of another, more direct way for you to do exactly what you want without messing with raw files. You need to use the .ac list... syntax; but why not put your (unequally-spaced or indeed random) frequencies in an external file? 1. Calculate, or determine your list of frequencies in Excel and export as a space delimited text file. Open the file in a text editor and prepend ".ac list ". (Don't forget the space) 2. Save file as Frequency_list.txt 3. Add a SPICE directive .inc Frequency_list.txt 4. Add .op analysis directive (this will be ignored when the text file is read). Job done. I have uploaded a working example to Files>Temp. I even surprised myself with this one. :-) I guess this would work with a .dc list analysis too, but I don't see any point in this. Regards, Tony
|
Thanks Nice idea...
This will work for transient analysis too, if LIST is supported in .tran....
Is list supported in .TRAN ?? This would allow you to have lot of data
points during fast edges and few during flat portions of the clock.
Cheers
AG
================================================================================================================
toggle quoted message
Show quoted text
On 9/14/2011 2:48 PM, Tony Casey wrote:
<snip>
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>,
Ganesan <dg1@...> wrote:
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
</snip>
Hello Ganesan,
I just thought of another, more direct way for you to do exactly what
you want without messing with raw files.
You need to use the .ac list... syntax; but why not put your
(unequally-spaced or indeed random) frequencies in an external file?
1. Calculate, or determine your list of frequencies in Excel and
export as a space delimited text file. Open the file in a text editor
and prepend ".ac list ". (Don't forget the space)
2. Save file as Frequency_list.txt
3. Add a SPICE directive .inc Frequency_list.txt
4. Add .op analysis directive (this will be ignored when the text file
is read).
Job done. I have uploaded a working example to Files>Temp.
I even surprised myself with this one. :-)
I guess this would work with a .dc list analysis too, but I don't see
any point in this.
Regards,
Tony
No virus found in this incoming message.
Checked by AVG - www.avg.com
Version: 9.0.914 / Virus Database: 271.1.1/3896 - Release Date: 09/14/11 01:34:00
|
--- In LTspice@..., Ganesan <dg1@...> wrote:
Thanks Nice idea...
This will work for transient analysis too, if LIST is supported in .tran....
Is list supported in .TRAN ?? This would allow you to have lot of data
points during fast edges and few during flat portions of the clock.
Cheers
AG
================================================================================================================
On 9/14/2011 2:48 PM, Tony Casey wrote:
<snip>
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>,
Ganesan <dg1@> wrote:
I can run different ac simulations with different frequency resolutions
and range..
Is there a way to merge the plot files.?
Cheers
A. Ganesan
</snip>
Hello Ganesan,
I just thought of another, more direct way for you to do exactly what
you want without messing with raw files.
You need to use the .ac list... syntax; but why not put your
(unequally-spaced or indeed random) frequencies in an external file?
1. Calculate, or determine your list of frequencies in Excel and
export as a space delimited text file. Open the file in a text editor
and prepend ".ac list ". (Don't forget the space)
2. Save file as Frequency_list.txt
3. Add a SPICE directive .inc Frequency_list.txt
4. Add .op analysis directive (this will be ignored when the text file
is read).
Job done. I have uploaded a working example to Files>Temp.
I even surprised myself with this one. :-)
I guess this would work with a .dc list analysis too, but I don't see
any point in this.
Regards,
Tony
No virus found in this incoming message.
Checked by AVG - www.avg.com
Version: 9.0.914 / Virus Database: 271.1.1/3896 - Release Date: 09/14/11 01:34:00
[Non-text portions of this message have been removed]
Hello Ganesan, This kind of interference is not needed or even desirable in .tran analyses because SPICE itself determines the step size depending on circuit activity. Sometimes it needs some help, though, in deciding what's really important. For this we can set the minimum step size; or the cunning designer might put tripdt/tripdv limits into a bogus B source to force the step size reduction just in the areas in most interest. Another means of doing this is to have a high(er) frequency source that drives the variable step size algorithm. This could be gated to run only when it's necessary to increase the resolution. Regards, Tony
|
