Timestep Too Small Error (12ax7 circuit)

[moparman]

Hi, I've just started using multisim 8 to simulate Vacuum Tube circuits and am having trouble. Everytime I build a preamp circuit using a 12ax7 or similar tube and hit "simulate"; I get an error "timestep too small.....". Then the simulation stops. I've tried changing the timestep options in transient analysis instruments options. If I change the maximum timestep to a higher value, the simulation starts but just keeps running and I get no results with the oscilloscope I have on the outputs of the preamp tube circuit. All other analog and digital simulations I've tried work perfectly without having to change any of the default values for the transient analysis instrument options. I cannot understand what the problem is. My computer is a AMD 64 bit 3.4 ghz with 512 megs of ram, 280 gig hard drive, etc. I'm not using 64 bit windows xp, I'm using 32 bit windows xp professional. Any help would be greatly appreciated. If anyone has had any luck simulating 12ax7 or similar circuits, please send me a reply or the saved file to see if that works. I've been looking for any tube preamp circuits to download for multisim but haven't been able to find any. Thanks!

[lacy]

What would be helpful is a circuit file or picture of your circuit. That way I can look at it for errors, simulate it, and try to figure out what is causing your particular error. Without it, I can't and won't try to guess as to what is happening.

[moparman]

Okay, here is the three circuits I've tried in Multisim 8. Thanks for your help.

[lacy]

O.K. Here's what I have so far. Keep in mind I am using 2001 and I am not  a tube expert. First I did away with your power supply and ran the voltages direct to the tubes. The only thing I have found is that the two 1Mohm resistors seem to be causing a problem for some reason. I eliminated the input resitor R9 and output resistor R6 from your original file (not the revised circuit). After doing that the circuit seemed to work normally. Why these two resistors would cause a problem I don't know.

The simulator also seems to be having problems with your power supply when it is hooked to the tubes. I haven't quite figured that one out yet. I will continue working on it to see if I can find a solution.

[moparman]

Hey, thanks for helping me work on this. I've been fooling around with it for a while now. I just keep getting the same error. I tried what you said about removing the 1 meg resistors and then hooking the AC 120v and DC 12 v up to the tube directly. I STILL get the error. Maybe it's just the versions of multisim I am using. I have both version 8 (2005) and 9 (2006). I am still wondering what's wrong. Never had any problems with multisim at all until I started trying to build the tube circuits. The funny thing is; I have built the real version of this circuit and it works perfect!!! By the way, it's an electric guitar preamp "overdrive" circuit. It boost the guitar signal, gives it that sweet tube sound and will go from ultra-clean to overdriven. Great sounding... Would you mind sending the circuit back to me so I can see it? Thanks again!

[lacy]

I don't really understand why Multisim (in all forms) has trouble with circuits that work in the real world. You would think that iif it works in reality, then the simulator shouldn't have one ounce of problems with it, but that just isn't the case.

I may have jumped the gun when I said I had it working. I found out that as long as R10 was set at 100% then it did work right and the volume control spanned correctly. Anytime I tried to adjust R10 below 100%, the error would return. I am going to continue playing around with this to satisfy my curiousity and also to get more tube experience. I will let everyone know what I find if I find anything.

[I.Foldvari]

I like to give an (general) answer to the common questions regarding "Time Step to small" and convergence problems in Multisim.

SPICE takes a text netlist describing the circuit elements (transistors, resistors, capacitors, etc.) and their connections, and translate this description into equations to be solved. The general equations produced are nonlinear differential algebraic equations which are solved using implicit integration methods, Newton's method and sparse matrix techniques.

To cut a long story short: If Multisim displays a "Time Step to small" or similar message, it only means that SPICE can't find a mathematical solution to the given circuit. Even if your circuit looks real, it is possible that through ideal models (e.g. don't take 'real' parasitic effects into account), ideal sources (e.g. high rise and fall time for a clock source) it doesn't behave like in reality. "Playing" around with your circuit (e.g. changing resistor values etc.) may or may not solve the problem. But as a rule of thumb, it is always recommended to match the components to their real counterparts.

A good approach to overcome convergence problems is to understand more about the SPICE Engine Options. They define what is rated as a "good" solution and what will become a "Time Step to small" or similar error. You can find the settings for the SPICE Options in the Analysis tab (part of setup for all analysis and the Interactive Simulation Settings for instruments).

Steps to solve "Time Step to small"

• Change RELTOL to 0.01% (Relative Error Tolerance)
• Change METHOD to "trapezodial" (Integration method)
• Change ITL4 to 100 (Upper transient iteration limit)

Please consult Multisim's online help for further assistance on convergence problems and SPICE options.

A great online resource are the SPICE Simulation Fundamentals on ni.com.

[lacy]

Thanks for your explaination on this subject. I have never really fooled around too much with the default settings in Multisim other than chaning the maximum timestep setting. I am going to give this a shot and see what happens.

I am no expert when it comes to Multisims internal workings that is why I have always tried re-working circuits to make them work in the simiulator at the default settings. I knew you could change the way the simulator does it's thing, but I never told anyone to adjust these settings based on my experience level with Multisim. I just didn't feel comfortable with my level of knowledge on the matter to recommend anything like this.

Thank you so much for taking the time to help and increase our level of knowledge about Multisim.

[lacy]

Ingo, your adjustments to the simulator worked great. I have one question: How can I make them permenant or will ajustment be necessary everytime I start a new circuit?

[I.Foldvari]

The default options for new circuits can't be changed as they are set to fit most circuits you will ever simulate.

However, the settings (all analysis and interactive simulation settings) are specific to a circuit and will be saved with it.

You also have the option to save your settings (go to menu Simulate > Save Simulation Settings) and load it into a new file (go to menu Simulate > Load Simulation Settings)