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.
|