开云体育

I have to simulate a complex circuit that have zeners, magnetics, MOSFET, resistors, capacitors and different diodes. the simulation shall be performed at three different temperatures (+25C, -34C, +71C). I already have all the components model at each temperatures, but there is a model of a SCHOTTKY DIODE, that is only at +25C, which is the following:

.MODEL 15ljq100 D(IS=6.15446e-05 RS=0.0153982 N=1.88088 EG=1.3 XTI=3.60437 BV=100 IBV=0.0001 CJO=1.08848e-09 VJ=0.4 M=0.371667 FC=0.5 TT=1e-09 KF=0 AF=1)

These are the questions: In order to have the model behavior on other temperatures (-34C and +71C), which parameters from the model above I have to change? How the parameter are change?(there is a tutorial or formulas that take the temperature as a function of the parameters)?
Thanks

... which parameters from the model above I have to change?

Perhaps none. Semiconductor models in LTspice already have
temperature dependencies built-in. For example, the ideal diode law
has temperature in the denominator of the exponential function.

That's not to say that the diode's characteristics could not be
enhanced by additional tweaking to account for temperature
dependencies that deviate from the norm, or from SPICE's equations.
But at least to some degree of accuracy, it is already there.

I think you may need to ask the manufacturer for better models if you
need them. I don't think anyone else can predict how this diode
differs from the SPICE model.

Do you have different models to account for part-to-part differences
too? That is probably a much bigger variation (than the difference
between the real diode and how SPICE already handles its tempco).

Andy

--- In LTspice@..., "j_asoto" <jasoto32@...> wrote:

I have to simulate a complex circuit that have zeners, magnetics, MOSFET, resistors, capacitors and different diodes. the simulation shall be performed at three different temperatures (+25C, -34C, +71C). I already have all the components model at each temperatures, but there is a model of a SCHOTTKY DIODE, that is only at +25C, which is the following:

.MODEL 15ljq100 D(IS=6.15446e-05 RS=0.0153982 N=1.88088 EG=1.3 XTI=3.60437 BV=100 IBV=0.0001 CJO=1.08848e-09 VJ=0.4 M=0.371667 FC=0.5 TT=1e-09 KF=0 AF=1)

These are the questions: In order to have the model behavior on other temperatures (-34C and +71C), which parameters from the model above I have to change? How the parameter are change?(there is a tutorial or formulas that take the temperature as a function of the parameters)?
Thanks

Hello,

The SPICE diode model handles various temperatures without any changes. If you want to simulate you circuit at different temperatures you need to put a .TEMP directive on your schematic. See .TEMP in the help file under Dot Commands.

Rick

The problem is that I have to indicate the worst case escenario even if this escenario never be possible in the real world. That's why I wrote Worst case analysis on the subject. I have to do many tests (simulations) to this circuit. Could happen that a worst case escenario of a test, shall have passive components in high temperature but active components at low temperature. What advice could any one give me for this case?
On 04/09/2013, at 9:30 p.m., "sawreyrw" <sawreyrw@...> wrote:

--- In LTspice@..., "j_asoto" <jasoto32@...> wrote:

I have to simulate a complex circuit that have zeners, magnetics, MOSFET, resistors, capacitors and different diodes. the simulation shall be performed at three different temperatures (+25C, -34C, +71C). I already have all the components model at each temperatures, but there is a model of a SCHOTTKY DIODE, that is only at +25C, which is the following:

.MODEL 15ljq100 D(IS=6.15446e-05 RS=0.0153982 N=1.88088 EG=1.3 XTI=3.60437 BV=100 IBV=0.0001 CJO=1.08848e-09 VJ=0.4 M=0.371667 FC=0.5 TT=1e-09 KF=0 AF=1)

These are the questions: In order to have the model behavior on other temperatures (-34C and +71C), which parameters from the model above I have to change? How the parameter are change?(there is a tutorial or formulas that take the temperature as a function of the parameters)?
Thanks

Hello,

The SPICE diode model handles various temperatures without any changes. If you want to simulate you circuit at different temperatures you need to put a .TEMP directive on your schematic. See .TEMP in the help file under Dot Commands.

Rick

[Non-text portions of this message have been removed]

... Could happen that a worst case escenario of a test, shall have passive
components in high temperature but active components at low temperature.
What advice could any one give me for this case?

LTspice lets you assign different temperatures to each component. See
the optional "temp=<value>" qualifier, which can be added to any
component that has a temperature dependency. It acts as an override
to the global temperature set by the .TEMP statement.

Andy

--- In LTspice@..., "j_asoto" <jasoto32@...> wrote:

I have to simulate a complex circuit that have zeners, magnetics, MOSFET, resistors, capacitors and different diodes. the simulation shall be performed at three different temperatures (+25C, -34C, +71C). I already have all the components model at each temperatures, but there is a model of a SCHOTTKY DIODE, that is only at +25C, which is the following:

.MODEL 15ljq100 D(IS=6.15446e-05 RS=0.0153982 N=1.88088 EG=1.3 XTI=3.60437 BV=100 IBV=0.0001 CJO=1.08848e-09 VJ=0.4 M=0.371667 FC=0.5 TT=1e-09 KF=0 AF=1)

These are the questions: In order to have the model behavior on other temperatures (-34C and +71C), which parameters from the model above I have to change? How the parameter are change?(there is a tutorial or formulas that take the temperature as a function of the parameters)?
Thanks

Hello,

The change of the forward voltage versus temperature can be set
with the parameter Eg. This allows you to adjust the -x.xmV/°C.

What also depend on temperature is leakage current in reverse
operation and series resistance Rs in forward operation.

Best regards,
Helmut

Helmut, are there formulas or equations to change those parameters?
On 04/10/2013, at 1:02 a.m., "Helmut" <helmutsennewald@...> wrote:

--- In LTspice@..., "j_asoto" <jasoto32@...> wrote:

I have to simulate a complex circuit that have zeners, magnetics, MOSFET, resistors, capacitors and different diodes. the simulation shall be performed at three different temperatures (+25C, -34C, +71C). I already have all the components model at each temperatures, but there is a model of a SCHOTTKY DIODE, that is only at +25C, which is the following:

.MODEL 15ljq100 D(IS=6.15446e-05 RS=0.0153982 N=1.88088 EG=1.3 XTI=3.60437 BV=100 IBV=0.0001 CJO=1.08848e-09 VJ=0.4 M=0.371667 FC=0.5 TT=1e-09 KF=0 AF=1)

These are the questions: In order to have the model behavior on other temperatures (-34C and +71C), which parameters from the model above I have to change? How the parameter are change?(there is a tutorial or formulas that take the temperature as a function of the parameters)?
Thanks

Hello,

The change of the forward voltage versus temperature can be set
with the parameter Eg. This allows you to adjust the -x.xmV/°C.

What also depend on temperature is leakage current in reverse
operation and series resistance Rs in forward operation.

Best regards,
Helmut

[Non-text portions of this message have been removed]

--- In LTspice@..., George <jasoto32@...> wrote:

Helmut, are there formulas or equations to change those parameters?

Sent from my iPad

Hello,
You could change the parameter Eg and then rerun a temperature
simulation while watching the forward voltage. You should get
something like -1.5mV/°C to -2mV/°C.

Best regards,
Helmut

On 04/10/2013, at 1:02 a.m., "Helmut" <helmutsennewald@...> wrote:

--- In LTspice@..., "j_asoto" <jasoto32@> wrote:

I have to simulate a complex circuit that have zeners, magnetics, MOSFET, resistors, capacitors and different diodes. the simulation shall be performed at three different temperatures (+25C, -34C, +71C). I already have all the components model at each temperatures, but there is a model of a SCHOTTKY DIODE, that is only at +25C, which is the following:

.MODEL 15ljq100 D(IS=6.15446e-05 RS=0.0153982 N=1.88088 EG=1.3 XTI=3.60437 BV=100 IBV=0.0001 CJO=1.08848e-09 VJ=0.4 M=0.371667 FC=0.5 TT=1e-09 KF=0 AF=1)

These are the questions: In order to have the model behavior on other temperatures (-34C and +71C), which parameters from the model above I have to change? How the parameter are change?(there is a tutorial or formulas that take the temperature as a function of the parameters)?
Thanks

Hello,

The change of the forward voltage versus temperature can be set
with the parameter Eg. This allows you to adjust the -x.xmV/?°C.

What also depend on temperature is leakage current in reverse
operation and series resistance Rs in forward operation.

Best regards,
Helmut

.MODEL 15ljq100 D(IS=6.15446e-05 RS=0.0153982 N=1.88088 EG=1.3 ...

I don't know much about the details ... but EG=1.3 might be a bit high
for a Schottky diode. The LTspice help docs imply a value of 0.69
would be more typical for a Schottky. But I would be very reluctant
to change any of the parameters and have something depend on the
results.

You could try searching the Internet for "SPICE diode model" and see
what pops out. For example, this document looks interesting:



Also there is the PSPICE reference manual, easily found by searching
the net for "PSPCREF.pdf".

Andy