simulation difference between multisim 10.1 and 14.0

[blanne]

I have been using Multisim 10.1 to verify and create examples for students and want to switch Multisim 14. Simulating a small ac-circuit I got different results using multisim 10.1 and 14.

The result of multisim 10.1 is identical with the manual solution.

Any idea, what the problem could be?

regards

blanne

[nestor-sg · Accepted solution]

Hi Blanne:

The default simulation setting in Multisim is to let its engine automatically determine TMAX, the maximum allowed timestep. In version 13, we modified this code in a way that it will let slower frequency circuits simulate faster in real time, we did this in order to speed up simulations as requested by users. For the most part this change has worked as expected, however your circuit is a clear example of a negative effect of this change. Its accuracy was affected by using larger time steps.

In your evaluation of Multisim 14, you can quickly change this. Click the Interactive analysis button in the toolbar to open up the analysis properties, and in the Interactive Simulation analysis > Analysis parameters tab look for the checkbox labelled Maximum time step (TMAX), place a check and let it set at 1e-005. Run your simulation again and you'll now see the 1.155 A result in the multimeter.

(Version 14 was automatically calculating TMAX as 1.25e-003)

I'll file a defect report so we review how we automatically determine TMAX so it won't get to a state like this example. I hope that my explanation helps you to move forward on your evaluation of the software.

Regards,

[blanne]

Thanks, now it´s working fine.

But I found another topic:

Why is the circuit being simulated in multisim 14  without an explicit ground?

Why multimeter XMM2 is showing a current when the switch is open?

Regards

blanne

[nestor-sg]

Hi blanne, for new topics create a new post in the future.

The images were embedded quite small, can you instead post the exact design file you are working on, so that we can all open it and help?

[blanne]

Hi Nestor,

find attached the ms14-file.

regards

blanne

[nestor-sg · Accepted solution]

Hi blanne:

Yeah, usually Multisim should pop up an error message saying that you have not grounded the circuit. However, in your circuit, you are using a switch, if you look at the View > SPICE Netlist Viewer you can see that this switch is introducing net 0 since it uses internal voltage sources in its model. The simulator considers this good enough to move on and simulate.

I quickly chatted with our simulation engineer, we are going to file a report so that we extend the check to require a ground component or net 0 in the first-level netlist, rather than anywhere which is the current situation.

Regards,

[nestor-sg]

Hi blanne, just to let you know the two reports filed (as a result of your forum post) are now fixed internally and will be part of our upcoming maintenance update to be released in 2 months.

Regards,