simulation software

hacknet · 13th December 2005, 11:54 AM

hey guys!

is there a downloadable simulation software i can use to get distortion figures. i've recently been working on SwCAD and I don't seem to be able to churn out distortion figures.

Thanks a million guys!

Robert McLean · 13th December 2005, 03:03 PM

I use Switcher CAD, aka LTSpice, for distortion all the time. An example of the standard SPICE op code to use is

.FOUR 1000 5 V(Out)

where 1000 is the fundamental frequency, 5 is the number of harmonics (including the fundamental) to report, and V(Out) is the name of the node. Change these to suit your own requirements, place the statement anywhere on your schematic, and after you execute a transient run view the results by clicking on View | SPICE Error Log.

Make sure your signal source frequency is the same as the fundamental specified, and also make sure your time step is small enough to give accurate results.

andrei · 13th December 2005, 07:29 PM

Well, you could try mine

...

hacknet · 14th December 2005, 01:33 PM

THANKS A MILLION ROBERT!

andrei, i'll try out your proggie.

thanks for the help guys!!!

nuvistor · 14th December 2005, 05:20 PM

For low level distortion analysis you should use the following settings:

In transient analysis set the time for 11 cycles, start saving data after 1 cycle, maximum timestep of saved data time/FFT no of data point samples in time. For instance for 1kHz, with 8192 FFT samples, maximum timestep is 10ms/8192 or 1.2us.

Tools/Control Panel/Compression, clear check boxes. The waveform compression introduces spurious distortion products, clearing the check boxes removes compression.

If this isn't good enough try Tools/Control Panel/Spice, reduce Reltol, default is 0.001, try 0.0005 or 0.0001, but convergence may be more difficult.

When using FFT Blackman window seems to give the lowest FFT noise floor.

Using these settings should give FFT dynamic range of at least 100dB or so with good frequency resolution, of course your actual circuit probably won't perform the same.

hacknet · 15th December 2005, 02:06 PM

whoa...! i just tried out the FFT functions and i realise that the voltage source is distortion ridden.

i'll try it out and report back!

thanks a million!!!

hacknet · 15th December 2005, 02:11 PM

thanks man! it works like a charm now!

13th December 2005, 11:54 AM	#1
hacknet diyAudio Member Join Date: Nov 2002 Location: sg	simulation software hey guys! is there a downloadable simulation software i can use to get distortion figures. i've recently been working on SwCAD and I don't seem to be able to churn out distortion figures. Thanks a million guys!

13th December 2005, 03:03 PM	#2
Robert McLean diyAudio Member Join Date: May 2005 Location: Stittsville, Ontario, Canada	I use Switcher CAD, aka LTSpice, for distortion all the time. An example of the standard SPICE op code to use is .FOUR 1000 5 V(Out) where 1000 is the fundamental frequency, 5 is the number of harmonics (including the fundamental) to report, and V(Out) is the name of the node. Change these to suit your own requirements, place the statement anywhere on your schematic, and after you execute a transient run view the results by clicking on View \| SPICE Error Log. Make sure your signal source frequency is the same as the fundamental specified, and also make sure your time step is small enough to give accurate results. __________________ Robert McLean

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Isn't there any 3d audio simulation software out yet??	JinMTVT	Multi-Way	26	14th March 2009 02:56 AM
Free simulation software from AD and NI	zapnspark	Everything Else	10	6th October 2007 03:37 PM
Simulation software.	beppe61	Solid State	30	28th February 2006 08:19 PM
Anyone uses simulation software ?	boxedin	Solid State	0	22nd December 2005 09:56 PM

New To Site?	Need Help?
Register to Participate Search Privacy Statement Contact Us	Frequently Asked Questions Did you forget your password? Mark Forums Read

13th December 2005, 07:29 PM	#3
andrei diyAudio Member Join Date: Dec 2002 Location: Canada	Well, you could try mine ...

14th December 2005, 01:33 PM	#4
hacknet diyAudio Member Join Date: Nov 2002 Location: sg	THANKS A MILLION ROBERT! andrei, i'll try out your proggie. thanks for the help guys!!!

14th December 2005, 05:20 PM	#5
nuvistor diyAudio Member Join Date: Jun 2004 Location: Richmond CA	For low level distortion analysis you should use the following settings: In transient analysis set the time for 11 cycles, start saving data after 1 cycle, maximum timestep of saved data time/FFT no of data point samples in time. For instance for 1kHz, with 8192 FFT samples, maximum timestep is 10ms/8192 or 1.2us. Tools/Control Panel/Compression, clear check boxes. The waveform compression introduces spurious distortion products, clearing the check boxes removes compression. If this isn't good enough try Tools/Control Panel/Spice, reduce Reltol, default is 0.001, try 0.0005 or 0.0001, but convergence may be more difficult. When using FFT Blackman window seems to give the lowest FFT noise floor. Using these settings should give FFT dynamic range of at least 100dB or so with good frequency resolution, of course your actual circuit probably won't perform the same.

15th December 2005, 02:06 PM	#6
hacknet diyAudio Member Join Date: Nov 2002 Location: sg	whoa...! i just tried out the FFT functions and i realise that the voltage source is distortion ridden. i'll try it out and report back! thanks a million!!!

15th December 2005, 02:11 PM	#7
hacknet diyAudio Member Join Date: Nov 2002 Location: sg	thanks man! it works like a charm now!

Currently Active Users Viewing This Thread: 1 (0 members and 1 guests)