how to change the time step

[wadeabes]

Hi,

I'm trying to simulate an analog switch MAX4714 in multisim, I got the pspice model and I have created a component for that switch.

But the main problem is that every time I tired to run the simulation I got that error

Output from instrument analysis  
|   |    TRAN:  Timestep too small; initial timepoint:trouble with (dx:x1:xu1) dcom1:x1:xu1  
|   |    doAnalyses: timestep too small  
|   |  
|   |  
|   |   tran simulation(s) aborted 

 I tried to change every option in the simulation parameters without any help.

please, I need help to solve this problem.

Note, It might be a problem in creating the switch component  but how I can know where is the problem.

Thanks a Lot

[lacy]

The simulator is fine. It is the component model that is causing the problem. I am going to re-post your circuit with the corrected part and you can just save it to your database.

The problem was that there were 2 .SUBCKT Statements at the beginning of the model file and I just deleted one of them and resaved the component. This cured the error that you were seeing. The circuit simulated fine at that point without your error.

[wadeabes]

Thanks for your help.
But the output isn't correct. It is an analog switch and the input is just DC, so the output should be two square waves on the NO and NC pins.
The circuit is working well in LTSpice and the output is just two square waves.

So, I think there is something else wrong.
It could be the pins configuration in the model.

Thanks

[wadeabes]

Hi,

By the way this is the whole circiut where the analog switch is used. The whole circiut is working OK in the LTSpice but is not in multisim.

Please, help me to fix it because it is very urgent for my reasearch.

Thanks

[lacy]

Yes, I thought that the output didn't look right when I was doing my tests. I tried last night to figure out what was causing this, but I couldn't come up with anything. It has to be a model incompatibility problem. Not all spice models will work with Multisim and this may be the case here. Since I am not an expert when it comes to deciphering model files it may be a good idea to let the NI Team take a crack at this and maybe they can see something in the model file that is causing problems. Also when I hook the IN pin to ground I get the convergence error like before and this shouldn't happen if the model file is compatible.

I would also say that this is also causing the problems you see in the main circuit. When I delete this part from the schematic then I don't get error.

Sorry I couldn't be of more assistance, but when it comes to figuring out model files my knowlege is limited. I will continue examining this and if I would happen to find something I will post it for you, but I have serious doubts about being able to find anything that would help. I will try my best.

[nestor-sg]

Just so you know, I'm looking into this.

The model nodes are not mapped correctly to the symbol pins. According to the model node 1 is IN, 2 is V+, 3 is GND and so forth... so we corrected that but then we get a convergence error...

We are tracking that error to a diode declaration inside the SPICE model, if we delete some parameters (N specifically) we can get it to work perfect... (analog switch), we are trying to know what exactly is that parameter doing on this model to see if by changing it we can still get it work or if we just are safe by deleting it...  give us an hour and we will post what we have...

[nestor-sg]

We can't figure out how the N parameter on the last diode statement is affecting the rest of the model in terms of convergence:
.MODEL DX D(IS=1E-18 N=0.001)

However, deleting that parameter makes the model to work as I believe, expected. I'm attaching your original file with the following modifications:

1. We changed the model mapping to symbol pin mapping to reflect exactly what the file says, originally it was all set up with no order and that is why Lacy and yourself were seeing only a straight line, instead of a switching signal.
2. We deleted the N parameter from that DX diode statement.
3. I move a little bit some components to make it easier to look and I changed the color of Ch B in the scope also to make it easier to read when you sample voltages.

Check if that improves your circuit simulation.

[nestor-sg]

Sorry, I forgot to mention to Lacy, having two .SUBCKT lines is not really a problem. The first .SUBCKT "structure" is calling the second one. If you have ever program in C for example, this would be equivalent to the main() section calling a MyFunction() later in the code. So, the first .SUBCKT is the entry point for the symbol and the model, inside it calls the other .SUBCKT statement... when that statement .ENDS, then the main entry point also .ENDS.

However, we did deleted the last comment lines marked with *, the last line in the code (for good practice) should always be .ENDS.

Message Edited by nestor on 11-15-2007 02:46 PM

[lacy]

Thanks Nestor for your assistance. I don't consider myself an expert on model files. I do know some about them, but definitely not enough. I should have caught the pin mapping error, but that slid right on by me. I also re-examine the model file where the double .Subckt statement was and I see what you are referring to. I didn't see the .ends statement at the end of the first .subckt statement and I think that is what threw me. Although, when I deleted the first .subckt/.ends statement the error that was being seen at simulation start disappeared and it did run even though the ouput waveforms didn't look right to me. I still had a square wave and a diferentiated wave, but they were both the same amplitude (I guess this is where the pin mapping came into play)

Thanks for your help on this. it is greatly appreciated as always

[Skums]

Hi

Can someonehelp me with this error? Everytime i get a message that trehe is an error with node and time stemp too small.

I've been chageing time steps from 0.000001 to 1sec and it still doesen't work.

One thing helps dough, when i delete a node, but that's not a solution.