Help with PSpice Error

J

Joe

Guest
Hi there,

I'm running a PSpice simulation of a simple one-stage common cathode
amp circuit. I have two triode models which I've downloaded from the
Internet, and model works as expected. When I use the second model,
however, Orcad displays a message box with this error:

There are no data values in section number one - Ignoring this
section.

Then the simulation terminates, and the output file includes this
error message:

INTERNAL ERROR -- Overflow, Convert


As a beginning electronics student, I'm having trouble understanding
what these messages indicate and haven't found any information on the
Internet relating to them.

Does anyone know what these errors mean? The biggest difference
between the models seems to be the use of the poly statement in the
second one.


Any suggestions are much appreciated.

Thanks,
Joe
 
Joe wrote:
Hi there,

I'm running a PSpice simulation of a simple one-stage common cathode
amp circuit. I have two triode models which I've downloaded from the
Internet, and model works as expected. When I use the second model,
however, Orcad displays a message box with this error:

There are no data values in section number one - Ignoring this
section.

Then the simulation terminates, and the output file includes this
error message:

INTERNAL ERROR -- Overflow, Convert


As a beginning electronics student, I'm having trouble understanding
what these messages indicate and haven't found any information on the
Internet relating to them.

Does anyone know what these errors mean? The biggest difference
between the models seems to be the use of the poly statement in the
second one.


Any suggestions are much appreciated.
Click to expand...
Yes:)

Have a go with SuperSpice (http://www.anasoft.co.uk) instead. Its demo
will allow much
larger circuits than the PSpice demo/student version. That is, 30
schematic blocks on a top level, each containing 25 real components in
one level of hierarchy. Email Support for even the demo is free.

The other reason is that there is a full set of tube/value symbols, and
as a
guitarist and analogue engineer as well, I know quite a bit about them
e.g.
(http://www.anasoft.co.uk/screenshot.html).


Kevin Aylward
salesEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.
 
Thanks a lot for the replies! I was able to find out that the models
were originally written for Intusoft PSpice 5.0. I'm using them with
Orcad PSpice 10, and it was suggested that perhaps the command syntax
is different.

The only real difference between this model and the one that works is
the use of the POLY statement - which I'm finding to be rather
confusing. Here are a couple of those statements:




eG0 10 0 poly(1) <2,3> -3.7694e+00 1.9947e+00 5.9432e-02
eG1 11 0 poly(1) <2,3> -3.2024e-02 -4.1443e-02 -4.8236e-03
eG2 12 0 poly(1) <2,3> 1.9127e-02 -1.2189e-02 -1.5526e-03
eG3 13 0 poly(1) <2,3> -1.1354e-02 4.9339e-03 6.1016e-04



eP0 110 0 poly(1) <2,3> -9.9158e+0 1.9145e+0 -2.8135e+0 1.8661e+0
+ 1.5643e+0 4.7240e-1 6.4276e-2 3.3101e-3

eP1 111 0 poly(1) <2,3> 9.5428e-1 3.2558e-2 -8.3349e-1 -4.8578e-2
+ 2.6213e-1 1.0492e-1 1.8921e-2 1.3632e-3

eP2 112 0 poly(1) <2,3> 9.5766e-2 2.5192e-2 2.2391e-1 -1.7040e-1
+ -2.4952e-1 -1.0960e-1 -2.0981e-2 -1.4882e-3

eP3 113 0 poly(1) <2,3> -6.6107e-2 -3.9657e-2 7.5560e-2 3.1025e-2
+ 2.4265e-2 1.7002e-2 4.2512e-3 3.4761e-4

eP4 114 0 poly(1) <2,3> 8.4148e-3 4.7989e-3 -1.3258e-2 -1.9288e-3
+ 5.2888e-4 -5.6853e-4 -2.4727e-4 -2.4359e-5



I can't tell if there are any glaring syntax problems or not, but from
the reading I've don, I think these lines are okay for use with Orcad.






On Tue, 02 Nov 2004 13:46:34 -0700, Jim Thompson
<thegreatone@example.com> wrote:

On Tue, 02 Nov 2004 08:31:41 -0800, Charles Edmondson
edmondson@ieee.org> wrote:

Joe wrote:
Hi there,

I'm running a PSpice simulation of a simple one-stage common cathode
amp circuit. I have two triode models which I've downloaded from the
Internet, and model works as expected. When I use the second model,
however, Orcad displays a message box with this error:

There are no data values in section number one - Ignoring this
section.

Then the simulation terminates, and the output file includes this
error message:

INTERNAL ERROR -- Overflow, Convert


As a beginning electronics student, I'm having trouble understanding
what these messages indicate and haven't found any information on the
Internet relating to them.

Does anyone know what these errors mean? The biggest difference
between the models seems to be the use of the poly statement in the
second one.


Any suggestions are much appreciated.

Thanks,
Joe
Joe,
The first error is the Probe window saying that the data file generated
is empty, i.e. there was no data to view. The second error of data
overflow I am not familiar with! Sounds like the model is doing
something that goes to infinity, either a super-high or current or
voltage, or something else illegal. Would need to see both to be sure.

--
Charlie

Charlie,

Experienced that myself recently, with PolarFAB BP30 NPN models that
are subcircuits that include the parasitic PNPs to substrate.

Cured it by setting SOLVER=0 ;-)

...Jim Thompson
Click to expand...
 
I took a closer look at the PSpice manual section below, and realized
it related to the VALUE statement also - which does exist once in this
model as follows:

eGIogVpc 20 0 value={log(v(1,3))}

I tried rephrasing this as

eGIogVpc 20 0 value={1}

and the simulation error disappeared! The results are entirely
inaccurate, but I think this confirms that the problem is with VALUE
and not POLY.

Now it's just a matter of figuring out why... :)


On Tue, 09 Nov 2004 00:42:37 GMT, Joe <joe@emailserver.net> wrote:

Thanks Charles. I just tried changing the <> characters to ( ), and I
see the same error. Specifically, this error occurs when calculating
the bias point for the transient analysis. In the output file is:


INTERNAL ERROR -- Overflow, Convert


I did find the following excerpt from the PSpice manual regarding the
POLY statement which seems to apply to this problem, though I'm not
quite sure:


" Caution must be exercised with the POLY form. For instance,

EWRONG 1 0 POLY(1) (1,0) .5 1.0

tries to set node 1 to .5 volts greater than node 1. In this case, any
analyses which you specify will fail to calculate a result. In
particular, PSpice A/D cannot calculate the bias point for a circuit
containing EWRONG. This also applies to the VALUE form of EWRONG:
(EWRONG 1 0 VALUE = {0.5 * V(1)}). "


On Mon, 08 Nov 2004 14:59:41 -0800, Charles Edmondson
edmondson@ieee.org> wrote:

Joe wrote:
Thanks a lot for the replies! I was able to find out that the models
were originally written for Intusoft PSpice 5.0. I'm using them with
Orcad PSpice 10, and it was suggested that perhaps the command syntax
is different.

The only real difference between this model and the one that works is
the use of the POLY statement - which I'm finding to be rather
confusing. Here are a couple of those statements:




eG0 10 0 poly(1) <2,3> -3.7694e+00 1.9947e+00 5.9432e-02
eG1 11 0 poly(1) <2,3> -3.2024e-02 -4.1443e-02 -4.8236e-03
eG2 12 0 poly(1) <2,3> 1.9127e-02 -1.2189e-02 -1.5526e-03
eG3 13 0 poly(1) <2,3> -1.1354e-02 4.9339e-03 6.1016e-04



eP0 110 0 poly(1) <2,3> -9.9158e+0 1.9145e+0 -2.8135e+0 1.8661e+0
+ 1.5643e+0 4.7240e-1 6.4276e-2 3.3101e-3

eP1 111 0 poly(1) <2,3> 9.5428e-1 3.2558e-2 -8.3349e-1 -4.8578e-2
+ 2.6213e-1 1.0492e-1 1.8921e-2 1.3632e-3

eP2 112 0 poly(1) <2,3> 9.5766e-2 2.5192e-2 2.2391e-1 -1.7040e-1
+ -2.4952e-1 -1.0960e-1 -2.0981e-2 -1.4882e-3

eP3 113 0 poly(1) <2,3> -6.6107e-2 -3.9657e-2 7.5560e-2 3.1025e-2
+ 2.4265e-2 1.7002e-2 4.2512e-3 3.4761e-4

eP4 114 0 poly(1) <2,3> 8.4148e-3 4.7989e-3 -1.3258e-2 -1.9288e-3
+ 5.2888e-4 -5.6853e-4 -2.4727e-4 -2.4359e-5



I can't tell if there are any glaring syntax problems or not, but from
the reading I've don, I think these lines are okay for use with Orcad.


Joe,
Looks like the problem is the <> instead of regular (). All the PSpice
examples I have show ().
--
Charlie
Click to expand...
 
On Tue, 02 Nov 2004 08:31:41 -0800, Charles Edmondson
<edmondson@ieee.org> wrote:

Joe wrote:
Hi there,

I'm running a PSpice simulation of a simple one-stage common cathode
amp circuit. I have two triode models which I've downloaded from the
Internet, and model works as expected. When I use the second model,
however, Orcad displays a message box with this error:

There are no data values in section number one - Ignoring this
section.

Then the simulation terminates, and the output file includes this
error message:

INTERNAL ERROR -- Overflow, Convert


As a beginning electronics student, I'm having trouble understanding
what these messages indicate and haven't found any information on the
Internet relating to them.

Does anyone know what these errors mean? The biggest difference
between the models seems to be the use of the poly statement in the
second one.


Any suggestions are much appreciated.

Thanks,
Joe
Joe,
The first error is the Probe window saying that the data file generated
is empty, i.e. there was no data to view. The second error of data
overflow I am not familiar with! Sounds like the model is doing
something that goes to infinity, either a super-high or current or
voltage, or something else illegal. Would need to see both to be sure.

--
Charlie
Click to expand...
Charlie,

Experienced that myself recently, with PolarFAB BP30 NPN models that
are subcircuits that include the parasitic PNPs to substrate.

Cured it by setting SOLVER=0 ;-)

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Jim Thompson wrote:
On Tue, 09 Nov 2004 00:52:49 GMT, Joe <joe@emailserver.net> wrote:


I took a closer look at the PSpice manual section below, and realized
it related to the VALUE statement also - which does exist once in this
model as follows:

eGIogVpc 20 0 value={log(v(1,3))}

I tried rephrasing this as

eGIogVpc 20 0 value={1}

and the simulation error disappeared! The results are entirely
inaccurate, but I think this confirms that the problem is with VALUE
and not POLY.

Now it's just a matter of figuring out why... :)



[snip]

You finally worked your own way thru the problem and made it easy for
me to appear wise ;-)

Bound v(1,3) so that it can't be ZERO (or fudge the operand so it can
never be ZERO).

...Jim Thompson
What Jim Said! :cool:
Click to expand...

--
Charlie
--
Edmondson Engineering
Unique Solutions to Unusual Problems
 
On Tue, 09 Nov 2004 00:52:49 GMT, Joe <joe@emailserver.net> wrote:

I took a closer look at the PSpice manual section below, and realized
it related to the VALUE statement also - which does exist once in this
model as follows:

eGIogVpc 20 0 value={log(v(1,3))}

I tried rephrasing this as

eGIogVpc 20 0 value={1}

and the simulation error disappeared! The results are entirely
inaccurate, but I think this confirms that the problem is with VALUE
and not POLY.

Now it's just a matter of figuring out why... :)


[snip]
Click to expand...

You finally worked your own way thru the problem and made it easy for
me to appear wise ;-)

Bound v(1,3) so that it can't be ZERO (or fudge the operand so it can
never be ZERO).

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Joe wrote:
Hi there,

I'm running a PSpice simulation of a simple one-stage common cathode
amp circuit. I have two triode models which I've downloaded from the
Internet, and model works as expected. When I use the second model,
however, Orcad displays a message box with this error:

There are no data values in section number one - Ignoring this
section.

Then the simulation terminates, and the output file includes this
error message:

INTERNAL ERROR -- Overflow, Convert


As a beginning electronics student, I'm having trouble understanding
what these messages indicate and haven't found any information on the
Internet relating to them.

Does anyone know what these errors mean? The biggest difference
between the models seems to be the use of the poly statement in the
second one.


Any suggestions are much appreciated.

Thanks,
Joe
Joe,
Click to expand...
The first error is the Probe window saying that the data file generated
is empty, i.e. there was no data to view. The second error of data
overflow I am not familiar with! Sounds like the model is doing
something that goes to infinity, either a super-high or current or
voltage, or something else illegal. Would need to see both to be sure.

--
Charlie
--
Edmondson Engineering
Unique Solutions to Unusual Problems
 
Joe wrote:
Thanks a lot for the replies! I was able to find out that the models
were originally written for Intusoft PSpice 5.0. I'm using them with
Orcad PSpice 10, and it was suggested that perhaps the command syntax
is different.

The only real difference between this model and the one that works is
the use of the POLY statement - which I'm finding to be rather
confusing. Here are a couple of those statements:




eG0 10 0 poly(1) <2,3> -3.7694e+00 1.9947e+00 5.9432e-02
eG1 11 0 poly(1) <2,3> -3.2024e-02 -4.1443e-02 -4.8236e-03
eG2 12 0 poly(1) <2,3> 1.9127e-02 -1.2189e-02 -1.5526e-03
eG3 13 0 poly(1) <2,3> -1.1354e-02 4.9339e-03 6.1016e-04



eP0 110 0 poly(1) <2,3> -9.9158e+0 1.9145e+0 -2.8135e+0 1.8661e+0
+ 1.5643e+0 4.7240e-1 6.4276e-2 3.3101e-3

eP1 111 0 poly(1) <2,3> 9.5428e-1 3.2558e-2 -8.3349e-1 -4.8578e-2
+ 2.6213e-1 1.0492e-1 1.8921e-2 1.3632e-3

eP2 112 0 poly(1) <2,3> 9.5766e-2 2.5192e-2 2.2391e-1 -1.7040e-1
+ -2.4952e-1 -1.0960e-1 -2.0981e-2 -1.4882e-3

eP3 113 0 poly(1) <2,3> -6.6107e-2 -3.9657e-2 7.5560e-2 3.1025e-2
+ 2.4265e-2 1.7002e-2 4.2512e-3 3.4761e-4

eP4 114 0 poly(1) <2,3> 8.4148e-3 4.7989e-3 -1.3258e-2 -1.9288e-3
+ 5.2888e-4 -5.6853e-4 -2.4727e-4 -2.4359e-5



I can't tell if there are any glaring syntax problems or not, but from
the reading I've don, I think these lines are okay for use with Orcad.
Click to expand...
Joe,
Looks like the problem is the <> instead of regular (). All the PSpice
examples I have show ().
--
Charlie
--
Edmondson Engineering
Unique Solutions to Unusual Problems
 
Thanks Charles. I just tried changing the <> characters to ( ), and I
see the same error. Specifically, this error occurs when calculating
the bias point for the transient analysis. In the output file is:


INTERNAL ERROR -- Overflow, Convert


I did find the following excerpt from the PSpice manual regarding the
POLY statement which seems to apply to this problem, though I'm not
quite sure:


" Caution must be exercised with the POLY form. For instance,

EWRONG 1 0 POLY(1) (1,0) .5 1.0

tries to set node 1 to .5 volts greater than node 1. In this case, any
analyses which you specify will fail to calculate a result. In
particular, PSpice A/D cannot calculate the bias point for a circuit
containing EWRONG. This also applies to the VALUE form of EWRONG:
(EWRONG 1 0 VALUE = {0.5 * V(1)}). "


On Mon, 08 Nov 2004 14:59:41 -0800, Charles Edmondson
<edmondson@ieee.org> wrote:

Joe wrote:
Thanks a lot for the replies! I was able to find out that the models
were originally written for Intusoft PSpice 5.0. I'm using them with
Orcad PSpice 10, and it was suggested that perhaps the command syntax
is different.

The only real difference between this model and the one that works is
the use of the POLY statement - which I'm finding to be rather
confusing. Here are a couple of those statements:




eG0 10 0 poly(1) <2,3> -3.7694e+00 1.9947e+00 5.9432e-02
eG1 11 0 poly(1) <2,3> -3.2024e-02 -4.1443e-02 -4.8236e-03
eG2 12 0 poly(1) <2,3> 1.9127e-02 -1.2189e-02 -1.5526e-03
eG3 13 0 poly(1) <2,3> -1.1354e-02 4.9339e-03 6.1016e-04



eP0 110 0 poly(1) <2,3> -9.9158e+0 1.9145e+0 -2.8135e+0 1.8661e+0
+ 1.5643e+0 4.7240e-1 6.4276e-2 3.3101e-3

eP1 111 0 poly(1) <2,3> 9.5428e-1 3.2558e-2 -8.3349e-1 -4.8578e-2
+ 2.6213e-1 1.0492e-1 1.8921e-2 1.3632e-3

eP2 112 0 poly(1) <2,3> 9.5766e-2 2.5192e-2 2.2391e-1 -1.7040e-1
+ -2.4952e-1 -1.0960e-1 -2.0981e-2 -1.4882e-3

eP3 113 0 poly(1) <2,3> -6.6107e-2 -3.9657e-2 7.5560e-2 3.1025e-2
+ 2.4265e-2 1.7002e-2 4.2512e-3 3.4761e-4

eP4 114 0 poly(1) <2,3> 8.4148e-3 4.7989e-3 -1.3258e-2 -1.9288e-3
+ 5.2888e-4 -5.6853e-4 -2.4727e-4 -2.4359e-5



I can't tell if there are any glaring syntax problems or not, but from
the reading I've don, I think these lines are okay for use with Orcad.


Joe,
Looks like the problem is the <> instead of regular (). All the PSpice
examples I have show ().
--
Charlie
Click to expand...
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top