EDSpice Simulator

Q1.Where can I change the limits of the simulation if the error 'Iteration limit reached' appears?

You can change the Iteration limit by selecting Setup Simulation Variables (Options). This pops a list of simulator variables that maybe set. Click on the option 'Reset DC Iteration Limit' and enter the new value.

Q2. A problem I have encountered is that when I use the spice netlist generator, from inside the EDSpice simulator, in order to run the simulation with another Spice engine or just to check it, all nodes have different numbers than that of the schematic and the original Spice circuit.

EDSpice uses node numbers (EDSpice Node Id) for internal manipulation. The program for internal use creates this. However, net names that you have given in Schematic are retained in EDSpice. You can view this using the tool Display Net Info (second last tool in the toolbar).

Q3. What is Gmin Stepping error? I am lack of information, examples and about the errors that occurs in EDSpice.

GMIN stepping Error

GMIN stepping is EDSpice's default DC convergence algorithm. "GMIN stepping failed" error message means that due to some reason, the Simulator is unable to solve the given circuit. Some probable reasons are following:

1) The elements in the circuit might have not set up properly. Check all symbols in the circuit and ensure that all of them are properly set up, and appropriate models are defined wherever needed.

2) Another common reason is the absence of DC path to ground at some analog node. This may happen while cascading capacitors, inductors or code models. For such situations select "RSHUNT" option (Setup -  Simulator Variables (Options)-  Shunt Resistance from analog nodes to ground RSHUNT =) and enter 1T. This automatically introduces 1 tera ohm resistance to ground at all analog nodes in the circuit to help it to converge.

3) Another reason is a loop of voltage sources and/or inductors or a series connection of current sources and/or capacitors. To get around in such situations, use a very small resistance in series with inductors, or a very large resistance in parallel with capacitors.
In the Help pull down menu in the EDSpice Simulator module, you have a topic How to use EDSpice. Selecting this, you will get the EDSpice Interactive Module Help file. This Help file should give you all the information you require on EDSpice. Click on the last topic EDSpice Example databases and go through the examples.

About Errors in EDSpice
The documentation of errors that occur in EDSpice is available. After invoking EDSpice Simulator, select EDSpice Reference under the Help menu item. In the Contents of EDSpice Reference Help, you have a topic 'Error Messages'. Go through this for explanation of errors that may be encountered while attempting to run a simulation.

Q4. Does EDSpice accept a SPICE Library in ASCII format?

EDSpice does accept model parameters and subcircuits in ASCII format. As EDSpice provides a graphical environment, slight modifications are to be made to these library files. To do this, library files may be adapted to the form accepted by Spice. Inorder to adapt to EDSpice Libraries, they should be compatible with the SPICE 3F5/XSPICE format. The adaptation of the ASCII libraries may be done in EDSpice module itself.

To adapt model parameters:
Select FileModel Library Editor from EDSpice Simulator and click Extract from the window that pops up. This allows extracting details from the file. The parameter may be saved in a .sml file.

To adapt subcircuits:
Select File Subcircuits Adapter from EDSpice Simulator. From the window that pops up click Select File. This allows extracting details from the file. The subcircuit may be saved to a .sbc file.

Q5. Is EDWin/EDSpice capable of doing audio frequency spectrum analysis a (Bode Plot of a state variable bandpass filter?

EDWin/EDSpice is capable of doing audio frequency spectrum analysis. EDWin will not generate the Bode Diagram. You can run Pole Zero Analysis in EDSpice and get a textual output.

Q6. Why and how Pole-Zero analysis ?

Pole- Zero analysis is mainly done to find the stability of a system.If a pole exits with a positive real part, this will result in a disturbance increasing exponentially with time. Hence the condition which must be satisfied,if a system is to be stable, is that the poles of the transfer function must all lie in the left-hand half of the complex-frequency plane.

Consider the case of an  amplifier with negative feed back and without feedback.  Pole-Zero analysis gives the result with lesser pole values (negative) for amplifier with feed back than the pole values for amplifiers without feedback indicating that the amplifier with feedback is more stable and thereby having more frequency response.
 
In EdSpice before Pole-Zero analysis the corresponding nodes are to be set. NODE1 and NODE2 are the two input nodes and NODE3 and NODE4 are the two out-put nodes

 CUR stands for a transfer function of the type (output voltage)/(input current) while VOL stands for a transfer function of the type (output voltage)/(input voltage). POL stands for pole analysis only, ZER for zero analysis only and PZ for both. This feature is provided mainly because if there is a non convergence in finding poles or zeros, then, at least the other can be found. Thus, there is complete freedom regarding the output and input ports and the type of transfer function.

Q7. Can you advise me on the correct use of the EDSpice adder and multiplier blocks.

The adder (Summer) is a block with 2-to N input ports. Individual gains and offsets can be applied to each inputs and outputs. Each inputs is added to its respective offset and then multiplied by its gain. The results are then summed, multiplied by the output gain and added to the output offset. This model will operate in DC, AC, and Transient analysis modes.

The multiplier is a block with 2- to N input ports. Individual gains and offsets can be applied to each inputs and outputs. Each inputs is added to its respective offset and then multiplied by its gain. The results are multiplied along with the output gain and are added to the output offset. This model will operate in DC, AC and Transient analysis modes. However, in ac analysis it is important to remember that results are invalid unless only ONE INPUT of the multiplier is connected to a node, which bears an AC signal.

Q8: What extra features does EDSpice simulator offer?

It provides different types of analysis according to your circuit design.

In addition to its analog simulation capabilities, EDSpice also allows efficient simulation of mixed-signal (analog/digital) circuits and systems. It completely buffers the user from the SPICE netlist through easy-to-use dialog windows. A unique feature allows the extraction of SPICE.MODEL lines and Subcircuits, from existing netlists, to be saved in special libraries. They can then be reloaded or edited later on. Hierarchical schematic diagrams are directly translated into SPICE netlist syntax. This means the hierarchy structure is maintained by using Subcircuits. Simulation results can be viewed in standard SPICE2 format or plotted as graphs in EDWin's Waveform Viewer.

Q9: In EDSpice, is it possible to force in the inputs any type of multishape signal defined by the user, similar function to VPWL_FILE of MICROSIM?

Yes, in EDSpice we can attach PWL files to the source. For this you have to select the tool "Set Parameters Models" and click on the source symbol to get the Instance parameter window. Click on the row for instance parameter named "Source function
"(last one) to get the "Source function" select window. This parameter will be available only for components, which act as source. Select PWL from the list and this will display the function parameters in the list provided. Either you can edit the parameters there itself or you can load already created PWL file using the button "LOAD VALUES FROM FILE". "Repeat items" edit box allows to enter the number of times you want to repeat the function parameters for the file.

Q10: Can we load from Internet, a Spice model of component from any manufacturer (Texas...etc..) then use it in EDSPICE?

Yes, you can do this using Subcircuit adapter.

To adapt subcircuits: -


1) Select EDWin Project Explorer. Right click on the task EDWin XP/2000 and select Subcircuits Adapter
. From the window that pops up select File/ Open. This allows extracting details from the file.

2) The display window will list the selected SPICE netlist.

3) The subcircuit should start with a .SUBCKT line and should end with .ENDS line. Before using a subcircuit for simulating with EDSpice, you should adapt it using Subcircuit Adapter and attach it the symbol.

4) The subcircuit adapter receives information about the nodes and stores it in the beginning of the subcircuit file as SPICE comments (lines starting with *). This information is used to graphically attach the subcircuit to the part. It is must to supply a description for the subcircuit including one for each of the available nodes. The description for each node is typed into the edit box called "Description" and is accepted by pressing the ENTER key on your keyboard. The column "Node Type" allows to select the node type of the subcircuit.

5) The adapted subcircuit is saved into a proper sub-directory under EDWIN\EDS_SBK. Before adapting the subcircuit, make sure that the Subcircuit file name and the name of the subcircuit mentioned in the .SUBCKT line are the same. This will avoid unnecessary warnings while pre-processing. Subcircuit name can have eight characters.