| Author |
Message |
epp
Joined: 04 Mar 2004
Posts: 264
Helped: 8
|
 06 Feb 2005 12:47 Large PSpice output file ??? Help. |
|
|
|
Hi!
When I simulate power electronic circuits in Pspice I got large *.dat file as a result (<=2GB). Circuit is very big with ABM, digital and analog parts and with large values of voltage, current and requency.
Is there any way how can I change deafult max value for this in Pspice which is 2GB (I need bigger) or how can I change some parameters in Pspice to get this dat file smaller so my simulation would reach its end without interrupting?
I mustn't change timestep or duration of simulation.
Thanks.
|
|
| Back to top |
|
 |
Vamsi Mocherla
Joined: 06 Sep 2004
Posts: 478
Helped: 61
|
| 12 Feb 2005 15:27 Re: Large PSpice output file ??? Help. |
|
|
|
| Hey, there are two things which determine the output file size. One the length of the simulation(of course depends on the time step accuracy). The other thing is the number of nodes you want to probe or save. When you want to reduce the size of your dat file, you can select only certain nodes to be probed and the file size will reduce considerably. Look into the .OPTIONS PROBE command or any other equivalent command
|
|
| Back to top |
|
|
mazelk
Joined: 23 Apr 2004
Posts: 107
Helped: 2
Location: COLOMBIA
|
| 13 Feb 2005 6:13 Re: Large PSpice output file ??? Help. |
|
|
|
When PSpice performs a simulation, it creates a waveform data file. The size of this file for a transient analysis is roughly equal to:
(# transistors)·(# simulation time points)·24 bytes
The size for other analysis types is about 2.5 times smaller. For long runs, especially transient runs, this can generate waveform data files that are several megabytes in size. Even if this does not cause a problem with disk space, large waveform data files take longer to read in and take longer to display traces on the screen. You can limit waveform data file size by:
· placing markers on your schematic before simulation and having PSpice restrict the saved data to these markers only
· excluding data for internal subcircuits
· suppressing simulation output
(cite: OrCAD PSpice User Guide)
Also, I can recommend you the follow commands for .OPTION statement:
.OPTION CPUTIME
CPU time allowed for thi run
.OPTION LIMPTS
maximun points allowed for any print table or plot
.OPTION NUMDGT
number of digits output in print tables (maximun of 8 useful digits)
Finally:
.PROBE V(node1) V(node2) ... V(node n) ...
writes only those output variables specified to the data file, to restrict the size of the data file.
|
|
| Back to top |
|
|
Vamsi Mocherla
Joined: 06 Sep 2004
Posts: 478
Helped: 61
|
| 15 Feb 2005 9:16 Re: Large PSpice output file ??? Help. |
|
|
|
| Well, the equation seems pretty logical. We more or less have a similar equation for the calculating the size of each out file
|
|
| Back to top |
|
|
dumbfrog
Joined: 17 Jul 2004
Posts: 191
Helped: 4
|
| 16 Feb 2005 1:46 Re: Large PSpice output file ??? Help. |
|
|
|
just probe the node you want to see
for example, just probe the node of the output and the input, not all the internal nodes.
|
|
| Back to top |
|
|
