LTSpice Issue...

mikeks · 2004-08-31 9:28 pm

How does one overlap traces from different simulations, and different circuits in LTSpice????

Andy_C? :scratch2:

mikeks · 2004-09-01 7:41 pm

Hello?

I need to run AC analysis on a circuit....modify values, and run AC analysis again to examine the effect of changes.....

How can i overlap both traces from these runs on the same plot in LTSpice..?

mikeks · 2004-09-02 12:50 am

Andy_C, specifically, do you have a solution to this problem ?

hjelm · 2004-09-02 6:46 am

This is not LTSpice but maybe the functionality is the same.
I use winspice and there is a command destroy_all that deletes previous simulation results if not then you can view them by naming them in incremental order. plot AC1.v(5) AC2.v(5). Plots v(5) from AC simulations 1 and 2.

jan.didden · 2004-09-02 7:38 am

mikeks said:
Andy_C, specifically, do you have a solution to this problem ?

Mike,

I dont now specifically LTSpice, but in most sims there is an option where you can sweep a value of a component or a source and automatically plot curves for each value. That I think is what you need. Is there anything in the help file on sweeping values or related terms?

Jan Didden

classd4sure · 2004-09-02 7:52 am

Hi,

From what I've read.. you can't?

Perhaps you can export data to a spreadsheet and do it yourself but that's rather laborious indeed.

Might I suggest you go to sci.electronics.cad newsgroup and address your question to Mike Engelardt who codes LtSpice, if people don't tell him what they don't like about it, or of its failings, then it can't ever improve.

Let us know about any response you get please, it's a good question, it might even be enough to start a war there.

Regards

mikeks · 2004-09-02 7:33 pm

janneman said:
Mike,

I dont now specifically LTSpice, but in most sims there is an option where you can sweep a value of a component or a source and automatically plot curves for each value. That I think is what you need. Is there anything in the help file on sweeping values or related terms?

Jan Didden

Hi,

No, i don't want to return a parameter sweep......

I need to run AC analysis, disconnect a component, re-connect it to another part of the circuit...and then run another AC analysis.

The results (traces) before and after the change must appear on the same graph.....viz: overlapped.

A sim. that does not posses a simple, transparent procedure for this is just so much junk as far as i am concerned.... :smash:

jan.didden · 2004-09-02 8:07 pm

mikeks said:
Hi,

No, i don't want to return a parameter sweep......

I need to run AC analysis, disconnect a component, re-connect it to another part of the circuit...and then run another AC analysis.

The results (traces) before and after the change must appear on the same graph.....viz: overlapped.

A sim. that does not posses a simple, transparent procedure for this is just so much junk as far as i am concerned....

Be creative. Put in both parts, sweep them from the nominal value to 'infinity' effectively removing them from the circuit. Do it in opposite direction for the two parts.

Jan Didden

sam9 · 2004-09-02 8:27 pm

I'm not sure about this but check it out. LT spice creates a .raw file when you run an analysis. Maybe this is only fro .TRAN. However, if it creates one when you run .AC then you couyld make your fisr run - rename the .eaw file then rub the second .AC and renamr that .raw file as well. Folowwing this you would have to take both files and uses them to plot the two curves in an external grapging program.

This sounds to me like a PITA and I'm not sure the .raw files that are generated are usable that way -- so this is just suggesing something to pursue.

BETTER IDEA. There is a Yahoo LT Spice users group where you might get a better answer. http://groups.yahoo.com/group/LTspice/

analogspiceman · 2004-09-02 9:01 pm

mikeks said:
Hello?

I need to run AC analysis on a circuit....modify values, and run AC analysis again to examine the effect of changes.....

How can i overlap both traces from these runs on the same plot in LTSpice..?

There is a very active Yahoo Group dedicated to LTspice. It's at http://groups.yahoo.com/group/LTspice. Your particular question has been discussed there several times. All posts are archived and are searchable. Also, the files section contains much useful reference material, models, and example circuits.

You can make the values of the components you wish to vary a table function of a stepped parameter. Use the ".step" command to step the controlling parameter (e.g. .step param n list 1 2 3...) to get several runs to appear in one plot. Then edit the value field of the target components to depend on this parameter (e.g. {tbl(n,1,1k,2,1p,3,1T} ). Be sure to enclose the parametrized expression in curly braces. Use extremely large values to "disconnect" the component and extremely small values to short it out.

To display only a particular step in the plot window suffix the trace expression with the step selection operator "@n", where n is the desired step number.

Most of this information is contained in the help file and is accessible via the help search function.

Graham Maynard · 2004-09-02 9:22 pm

Hi mikeks,

I don't know your simulator, but can you not construct the circuit two or more time on the same screen ? Then common your input connection and apply sensing meters as appropriate.

On some simulators it might be possible to copy and paste the first circuit on to the same page many times.

Hope you find a way.

Cheers ........... Graham.

andy_c · 2004-09-02 9:46 pm

Hi Mike,

Sorry I missed the thread yesterday. LTSpice doesn't have a way to save old simulation results to a file for later display as far as I know. Only Helmut's utility does that. The only way I can think of to do this would be to make a subcircuit of the common part of the two configurations, then replicate the subcircuit, adding in the unique portion outside the subcircuits. That's what I used to do for the Middlebrook stuff before I stumbled on the loop gain component. Maybe the loop gain component will reveal some secrets of how this might be done?

jan.didden · 2004-09-02 9:50 pm

Andy,

Post #8 shows a realistic option, that I've used with no problems.

Jan Didden

andy_c · 2004-09-02 9:59 pm

Jan,

When I first read your post I couldn't figure it out. But it seems like what you're saying is to connect with resistors and do a parameterized sweep of the resistors between two values - "very small" and "very large". That sounds like it would work and be simpler than what I suggested.

jan.didden · 2004-09-02 10:01 pm

In fact you can also do it with caps - just sweep from nominal to zero instead of infinity - that's why I had 'infinity' in quotes.

Jan

PS Nice Pelican - or is it?

andy_c · 2004-09-02 10:14 pm

janneman said:
PS Nice Pelican - or is it?

Yes, I'm part of the Spanish pelican inquisition. Our chief element is surprise!

mikeks · 2004-09-03 1:55 am

Thanks folks...although LTspice's postprocessor is probably the best around, i reckon i'll stick with Multisim 7, and Symetrix... :smash:

mikeks · 2004-09-03 8:42 am

P.s:

Graham Maynard said:
Hi mikeks,

I don't know your simulator, but can you not construct the circuit two or more time on the same screen ? Then common your input connection and apply sensing meters as appropriate.

On some simulators it might be possible to copy and paste the first circuit on to the same page many times.

Hope you find a way.

Cheers ........... Graham.

Your idea was the easiest to implement...but slowed the sim. down somewhat.....for obvious reasons...

Cheers.

LTSpice Issue...

Disabled Account

Disabled Account

Disabled Account

Member

AX tech editor

Disabled Account

Disabled Account

AX tech editor

Member

Member

R.I.P.

Banned

AX tech editor

Banned

AX tech editor

Banned

Disabled Account

Disabled Account