[Top][All Lists]

[Date Prev][Date Next][Thread Prev][Thread Next][Date Index][Thread Index]
## [Help-gnucap] Re: NTC and PTC

**From**: |
nbs |

**Subject**: |
[Help-gnucap] Re: NTC and PTC |

**Date**: |
Thu, 08 Jun 2006 21:27:11 +0900 |

**User-agent**: |
Thunderbird 1.5 (X11/20060317) |

Hello Markus,
There are two ways for simulating thermal effects:
1. Native (and somewhat limited) Spice method. Use a resistor model and
define tc1, tc2 parameters.
That might be something like this (not checked):
.model NTCRES R res=1k tc1=-1 tc2=0.01
Rntc1 n1 n2 NTCRES
Rntc2 n3 n4 NTCRES temp='temp_param'
Temperature of Rntc1 is set in simulation options. Temperature of Rntc2
is equal to the 'temp_param' parameter value.
Refer to this page for details:
http://www.gnu.org/software/gnucap/man/node77.html
(BTW. in the description of tc1, tc2 should be [Ohm/degree C], I guess)
2. Above method cannot be used for simulating dynamic thermal effects
(this is a limitation of Spice) as temperature is constant within a
simulation sweep. You may want to design your own resistor model where
temperature will be represented as a signal (for example a node voltage).
Here is an example of what could be possibly used in hspice:
i_ntc1 n1 n2 cur='v(n1,n2)/(resistance_value+tc1_param*v(temp_val)'
v_temperature temp_val 0 pwl (0 0, 1s 10, 3s -10, 4s 0)
Andrzej
>* Hi,*
>* *
>* I founded the fit command.*
>* *
>* Ihis possible, that i can use the fit command to get an NTC or PTC?*
>* For example,*
>* R1 2 0 fit 2k,22°C 1k,30°C 500,40°c 250,50°c order=1*
>* *
>* Maybe the Temperatur will not be increased, and therefore the Value of*
>* the Resistor will not be sweeped?*
>* Are there any Ideas?*
>* *
>* mfg Markus*

**[Help-gnucap] Re: NTC and PTC**,
*nbs* **<=**