A few months ago, I would like to try to make a class AB amplifier, but I do not know how to simulate the bias point, especially with the OPS power BJT temperature rise.
So, in the using Pspice my confusion is how to assign or sweep temperature parameter of the power BJT(maybe include the Vbe multiplier transistor), While maintaining the temperature of other devices unchanged.
Tks
So, in the using Pspice my confusion is how to assign or sweep temperature parameter of the power BJT(maybe include the Vbe multiplier transistor), While maintaining the temperature of other devices unchanged.
Tks
Global temperature (all devices are at the same temperature, leaving the internal dependence on the device models, if none it won't be considered) is simple and is included in the DC analysis. Local temperature (e.g. only for the power devices) is obscure and rather complicated to implement. This is how I'm doing it, others may have a better idea.
- Create a temperature dependent model for your devices. Example:
* MJL4281A NPN EPITAXIAL SILICON TRANSISTOR
* ONSEMI MODEL MODIFIED FOR TEMPERATURE DEPENDENCE
*-------------------------------------------------
.SUBCKT MJL4281T C B E
+ params:
+ REL_TEMP=0
Q_MJL4281 C B E MJL4281
.MODEL MJL4281 NPN (
+IS=6.5498e-11 BF=139.247 NF=1.00176 VAF=46.776
+IKF=10 ISE=7.75232e-12 NE=3.34341 BR=4.98985
+NR=1.09511 VAR=4.32026 IKR=4.37516 ISC=3.25e-13
+NC=3.96875 RB=11.988 IRB=0.111742 RBM=0.102914
+RE=0.00127227 RC=0.209833 XTB=0.115253 XTI=1.03146
+EG=1.11986 CJE=1.0531e-08 VJE=0.4 MJE=0.450375
+TF=2.6464e-9 XTF=1000 VTF=2.06045 ITF=175
+CJC=5e-10 VJC=0.4 MJC=0.85 XCJC=0.959922
+FC=0.1 CJS=0 VJS=0.75 MJS=0.5
+TR=1e-07 PTF=0 KF=0 AF=1
+ T_REL_GLOBAL={REL_TEMP})
.ENDS MJL4281T
- Create a new part with REL_TEMP as a parameter and make the parameter visible (see the attachment).
- Associate the temperature dependent spice model with the part.
- In the schematic, create a PARAM and add a new Property named "Tmpr". Don't use Temp TEMP or other obvious names for this property since they may collide with a default property in Spice and you will pull your hair why nothing is working.
- Add the temperature dependent parts to the schematic, the REL_TEMP default value 0 should be visible.
- Double click this property in each part you want to sweep the temperature and replace the 0 with {Tmpr}.
- Create a DC sweep simulation. On the Primary sweep, select Global parameter and enter Tmpr as the parameter name, then the start, stop and increment values (for the temperature).
Cross your fingers and run the DC sweep simulation. If you did everything right, you should have it working right away. The slightest mistake will make the simulation fail with all kind of obscure error messages, none of which will point you to the true error source (syntax or semantics). If you run into such, you'd be better to scrap everything and start over.
Thank you Waly.
I Analyzed your approach, and I think that is definitely right and very good way to simulate the local temperature.
I used your method step by step. experienced several errors, but all the error are model creation error, something like the npn changing to pnp, and changing the order of anode and cathode of a diode.
After several times of devoutly Crossing my fingers, I think I have realized the simulation.
For me, the next question is how to get a stable bias point. such as how to make the collector current of power BJT(NJL3281 and NJL1302) does not change with temperature rise.
Best Regards
Xixi
- Status
- Not open for further replies.