PSpice's limit function places a lower and upper limit on a value but we haven’t implemented this in our program yet. However, you CAN use B2 Spice's nonlinear 'B' source's IF-THEN-ELSE function in place of the limit.

The LIMT function’s format is LIMIT(x, lower, upper), so the equivalent ITE expression is

if(x < lower, lower, if(x > upper, upper, x))

That’s just nesting two IF statements to mean

"if x < lower, then the value is lower. If x > upper, then the value is upper. Otherwise the value is x."

IF-THEN-ELSE functions can ONLY be used in the 'B' nonlinear source.

When the tutorial and manual were written, we had not actually implemented a timing diagram yet and there was an assumption that we would eventually. However that has not yet happened but it is still on the list of things to do. But to get a timing diagram, you can use a 'cheat'. Just set up a Transient test for a start time of 0 and a stop time of -1. When the Transient Test is run, the simulation will proceed indefinitely until you stop and reset it using the simulation toolbar. The circuit will still be interactive if you have digital inputs and outputs in it and digital traces will be displayed in the resulting graph.

This is usually due to the fact that Windows' screen fonts have been changed from the default "Small Fonts" to "Large Fonts". We're trying to find a solution to this problem because the font size is handled automatically and is out of our control. Until we get a fix for this, the workaround is to change Windows' screen font size back to "Small Fonts". To do so, go to the Control Panels->Display Properties->Settings->Advanced Button->General tab. In that dialog, there should be a Font Size box with a drop-down box. If it currently lists 'Large Fonts', change it to 'Small Fonts' and OK all the dialogs.

For some reason, an invalid or non-working version of this DLL exists in your system or was installed incorrectly. Follow the these instructions to fix this:

Go to your C:\Windows\System32 directory and locate BDSP.DLL. Rename it to BDSP.BCK.

Download the following zip file: bdsp.zip and extract the BDSP.DLL in that zip file to the C:\Windows\System32 directory

Try starting up v5 and let us know if this does not solve the problem.

A specific PSPICE specific conversion to look for is how PSPICE denotes resistors, capacitors, and inductors in the .model line. PSPICE uses RES, CAP, and IND where Berkeley SPICE uses R, C, and L respectively. For instance, a resistor model in PSPICE will be something like

.model rmod RES ...
whereas Berkeley SPICE will look like
.model rmod R ...

Also, PSPICE's dependent sources can use a VALUE= syntax and then an equation for the voltage or current. SPICE doesn't have this syntax but the conversion for this is to replace the device with a non-linear source, depending on the original PSPICE device type. For instance:

PSPICE:
EFB 12 OUT VALUE={8.822-.4024*V(13,5)+5.250E-3*V(13,5)*V(13,5) -.6667*V(13,5)*V(6,5)}

SPICE:
BEFB 12 OUT V = 8.822-.4024*V(13,5)+5.250E-3*V(13,5)*V(13,5) -.6667*V(13,5)*V(6,5)

The "VALUE =" with a "V=" to denote a voltage source because the original device was an "E" voltage controlled voltage source and the "V =" means "voltage equals". If the original device were a current source F or G type device, the instead of "V=", you would use "I ="

Also there are simply some model parameters that just have no SPICE equivalent and must be left out. I don't have a complete list of the non-SPICE syntax but our program will let you know if it doesn't recognize a parameter and then ignore it so really nothing has to be done. But it's worth keeping in mind that the effects of the omission are unknown and must be considered.

The hardest thing to convert is PSPICE's ability to use If-Then equations. There is a convoluted way to use logical syntax in SPICE and one of our users was kind enough to write up a guide on doing so: http://www.beigebag.com/case_logical_1.htm.

These are the most common problems when trying to convert PSpice to Berkeley SPICE and there will probably be more specific problems that are not covered here. PSPICE to Berkeley SPICE conversion is as much art as science and there's no set way to convert all cases of PSPICE to Berkeley SPICE. If you have problems, you can always submit it to us for help.

There are a couple of things to try if you believe that the simulation that you're running is going slower than it should.

The first thing to try is to make sure that circuit state animation is turned off. One of the features of version 5 is the ability to show animated circuits, i.e., showing voltages and current flow with dynamic symbols and colors.  To see an example of this click here.  This feature, while very useful, does take up a significant amount of computing power as it redraws the circuit wires with each simulation interval.  If you value speed over visuals, make sure that all these options are turned off in the ANIMATIONS tab.

Also, if you have any virtual instruments showing, try collapsing the instrument window so the program does not need to update the instrument displays.

Another thing you can do is to try to change your simulation parameters. If you're running a Transient simulation, you can try increasing the step size if you don't mind losing a bit of resolution. Or if you have "use initial conditions" checked when you really don't need to, turn that off. Also in Transient simulation, you can try going to the Miscellaneous Options in the Simulation menu and playing with the minbreak parameter. One of our users reported good results using a value of 1n and increasing from there. Too large a value might result in convergence problems.

Finally, you can try altering the convergence options found under the "Simulations->Simulation Options" menu. By default, we have pre-set some parameters to avoid the most common convergence problems. However, you can try increasing the "reltol" parameter since we've set it to something finer than it needs to be. Try 1e-3 instead of the given 1e-4. But keep in mind that this might affect the accuracy of your simulation. You might need to change your step size to compensate.

This message means that the simulation engine encountered a model parameter that isn't recognized by Berkeley Spice. For instance, the following line will produce an error:
.MODEL Dbody D Is=125f N=1.023 Rs=1.281 Ikf=18.01 Cjo=46.3p M=.3423
+ Vj=.4519 Bv=60 Ibv=10u Tt=161.6n
>ERROR: unrecognized parameter (ikf) - ignored
This is because the IKF parameter is a PSPICE parameter and isn't a valid Berkeley SPICE parameter. B2 Spice will then ignore the parameter and proceed with the simulation. However, the effects of the ignored parameter is unknown and should be kept in mind. You can elect to remove these parameters permanently from the model by using the Database Editor to remove these parameters.

Another PSPICE notation that can cause problems is PSPICE's way of denoting resistors, capacitors, and inductors in the .MODEL line. PSPICE uses RES, CAP, and IND, respectively while Berkeley SPICE uses R, C, and L, respectively. Just make these changes and the model should import correctly. An example is below:
.model rt RES tc1=-0.006 (PSPICE)
.model rt R tc1=-0.006 (Berkeley SPICE)
However, the Database Editor can automatically fix these error automatically in the process of importing the model.

More often than not, the problem is that the model you've imported is not Berkeley Spice compatible.  The Database Editor can convert older Berkeley Spice format but it can't convert from PSpice, IBIS, and some other formats to Berkeley Spice.  So if you're having this kind of error, then email us about it and include the model text.   We'll see if we can't get something working for you.

It could also be that within the controlled-source line is a scientific notation type for a number, such as 1e3 or 1K. If this is the case, these numbers need to be replaced with decimal equivalents, e.g., 1000 for 1e3 or .001 for 1m.

If this does not get the circuit to work, then follow the advice in the item above on getting the circuit with switches to simulate.

The same principals apply when performing parameterized transient and ac sweeps with temperature as the parameter.

Use the device name whose temperature is to be swept for the source name and the parameter named "temp" if it is available for the property name. If you are sweeping a resistor’s temperature, then make sure that it is a temperature dependent resistor and give it TC1 (and possibly TC2) values.