(Help):timestep too small error and how to do changes in the simulation

[雪域]

HI ALL,

I have a constant current  source circuit.When i tried to simulate,  it gives me a message that time step too small.I changed in the simulation as the way in the forum,but the error still exit.

i saw the presentation on the SPICE simulation options in http://zone.ni.com/devzone/cda/tut/p/id/5418#toc4, and changed correlation parameter, but it's no help.  

How to change the simulation options in the MULTISIM?

How do i can avoid some very generic error?

Everybody can give some advices and experiences about the MULTISIM setting for new personality.  You can discuss the familiar problems and resolvents.

here is the three circuits I've tried in Multisim 10. Thanks for your help. Thanks!

[lacy]

Here's what I have found.

1) You can use the convergence assistant when it pops up to help you in solving problems such as this and it automatically set the simulator settings.. Granted that not all the time will it be able to help, but in a majority of the times it does. If you have this option in your version, it is the quickest way correct these situations. If you don't then goto #2.

2) As far as the first circuit goes, everything looks correct (connections, etc.) as far as I can tell. To get it simulating go into SIMULATE>INTERACTIVE SIMULATION SETTINGS>ANALYSIS. While there check the circle whare it says USE CUSTOM SETTINGS then click the CUSTOMIZE button. From there goto the TRANSIENT Tab and click it. At the very bottom of the list that comes up it says Integration Method (METHOD). Click the box to activate it and then in the drop down box select GEAR.

If you don't have the convergence assistant then you just have to experiment with different settings until you find the right combination.

Message Edited by lacy on 10-10-2007 08:53 AM

[lacy]

As far as the second circuit is concerned it simulates just fine on mine with the default settings. One thing I will bring to your attention is the fact that the O-scope is not grounded.

I am going to make an additional comment for NI. I have run into on more than one occasion where some of the simplest circuits would not work with the default settings and I would have to either run the convergence assistant or manually set up the simulator. This convergence issue is really bothersome.How I am I to trust the results of a simulation if there isn't some consistancy in the simulator settings. I have had times when each circuit I tried had to have different settings in order to get them simulating and then at other times I would have different resutls from the same circuit with different settings. In my opinion, this type of inconsistancy should not happen. I really think that this needs to be looked into and some sort of standard come up with that works across all circuts as much as is possible.

[lacy]

Your post said you had three circuts, but only 2 managed to get posted. You might want to try and re-post the 3rd one for us to look at.

[lacy]

I found something else here that the convergence assistant never told me about when it went through its paces. It not only changed the method to Gear but it also changed Upper Transient Iteration Limit (ITL4) from 100 to 10000. So you have to change that.That is in the Transient Tab where you changed to the METHOD to Gear.

After finding this, you don't have to change the METHOD only ITL4 from 100 to 10,000. If the Convergence Assistant had notified me of this change at first then I would have told you that also, but it just told me that it switched the Method only. I came to question this only after loading simulation setting that I had saved previously that were already set to GEAR. It wouldn't simulate and the Assistant couldn't fix it. I then compared what it did the first time with my settings and the only difference was IT4 had been increased.

I am sorry if this caused any problems, but I blame the assitant for not giving me full info on changes made.

That setting just by itself has seemed to make things more stable on my end as far as the circut problems I desctibed in a previous post where sometimes circuits would simulate and sometime they wouldn't. I will continue trying this setting across all my circuits and see it this is what I have been looking for also.

Message Edited by lacy on 10-10-2007 02:52 PM

[Maxish]

Hello,

I tried the first circuit. It fails in transient analysis because it fails to find the DC operating point using the default settings. You can push the simulator to try harder by adjusting the simulation settings by going to simulate->interactive simulations settins->analysis options tab->select custom radio button-> customize button

Go to DC analysis tab and increase ITL1 from 100 to 1000. Worked for me!

[lacy]

Hi Max,

I was just wondering about having to re-adjust the simulator like this. Is there any standard setting that a person can use that would be universal for most circuits because the defaults don't always seem to work?

On aniother note, I will try what you said about IT1, but IT4 seemed like it done the trick. It doesn't really matter as long as we get people's circuits up and running for them.

Thanks a bunch for this information and response.

Edit: Thanks Max for that info in IT1. I tried that and it worked great too. So now he has 2 options to choose from to help him.

Message Edited by lacy on 10-10-2007 04:39 PM

[雪域]

Hello,Maxish

First, Thanks for your response and help. In the first circuit, I increased ITL1 to 1000. The circuit simulation didn't give me  error messages about DC. But it still clue on Timestep too small. I tried what lacy said about IT4. Increasec ITL4 to 1000, the circuit worked well. Thanks lacy for your help too.

By the simulation, i knowed the convergence assistant can give some important informations. We must using well.

Thanks!

Thanks!

[雪域]

Hi lacy,

Here is third  circuit. I only changed ITL1. the circuit simulation didn't give me error info. Thanks!

[lacy]

Your welcome. We are here to try to help. It doesn't make any difference as to which method you chose to use as long as you get your circuit working the way you want it to. I would like to thank Max again for his input on this and it is greatly appreciated.

Just as an added comment on this subject. You can save these simulation setting for future use once you get them adjusted. To do this just go to SIMULATE>SAVE SIMULATION SETTINGS. I would recommend keeping IT1 at 1000 and ITL4 at 10000 and saving this. From my investigation it seems these settings work well with all my circuts that I had problems with and had various different settings set up for each circuit. Now I only have one setting that seems to work pretty well across all of them and this was something I have been trying to accomplish for a while. So we both gained something from this discussion and that is always a good thing.

I thought I would just let you know this inforamtion and you can do with it what you want.