light dimmer circuit

Thread Starter

denison

Joined Oct 13, 2018
91
attached is a schematic for Tina-T1 software. This is from texas instruments. A 240vac source charges a capacitor which fires the triac when the diac is at approx. 32v. This circuit does work in practice. Can anybody explain why I can't get the software to work for this simple circuit?
Lt spice does not have diac or triac models.
The file from Tina was a tsc file and this was not allowed as a file type. also tried pdf file and didn't work. had no trouble with files from ltspice. how can I fix this problem?
 

Bordodynov

Joined May 20, 2015
2,604
attached is a schematic for Tina-T1 software. This is from texas instruments. A 240vac source charges a capacitor which fires the triac when the diac is at approx. 32v. This circuit does work in practice. Can anybody explain why I can't get the software to work for this simple circuit?
Lt spice does not have diac or triac models.
The file from Tina was a tsc file and this was not allowed as a file type. also tried pdf file and didn't work. had no trouble with files from ltspice. how can I fix this problem?
If you are not lazy, LTspice will have many diac and triac models. And many other models that are not in Tina TI.
http://bordodynov.ltwiki.org/
 

ericgibbs

Joined Jan 29, 2010
10,042
hi denison,
Please post your LTSpice asc file/circuit diagram for the project.
For the Triac/Diac modules, use Search feature in Windows to look thru the Documents/LTSpice folder, they do exist.
Also as @Bordodynov points out they are also included in his models.

E
 

Bordodynov

Joined May 20, 2015
2,604
See. At lower wattages, the lamp has a lower temperature. The resistance of the thread is less and therefore the amplitude of the current is greater.
2020-05-29_14-54-03.png
 

Thread Starter

denison

Joined Oct 13, 2018
91
Hi Mr Bordodynov, I have just downloaded your library of extra parts for ltspice. I see that there is a triac model there which I need. Just not sure now how to proceed. I see that the ltspice edition is 4 IV. my edition is 17 xv11.
I see that in my edition the triac model has not been added to the symbol.
How do I get these extra models into my spice edition? When I tried to open the triac model got the answer I needed an app. I think the app might be edition 4 of lt spice. Do I need now to download edition 4?
Please advise on how to proceed now. thanks.
 

Rich2

Joined Mar 3, 2014
172
I find it quicker and easier to build the circuit than faffing about with software, even if I get the software to run after many hours, I don't know what on earth it's doing. I suppose I just haven't got the patience for it :)
 

Bordodynov

Joined May 20, 2015
2,604
No you do not need to download LTspice!
The Triac symbol has no model. It is intended for use with third models. My additional libraries are in the ZZZ folder and the triacs in the ZZZ/Triac folder. If you have installed my library correctly, please see:Triac2.pngTriac.png
 

ci139

Joined Jul 11, 2016
1,463
triacs have different triggering currents / voltages for different quadrants (see datasheet) ... usually they are all unequal
... i don't see the models utilizing this feature
 

Attachments

Last edited:

Bordodynov

Joined May 20, 2015
2,604
* 2N6075 ; Triac ; Silicon (Si) ; Motorola ; TO-225AA
* Level 1
.SUBCKT MOT_2N6075 3 2 1
* | | |
* | | MT2
* | G
* MT1
*
Q1 5 4 3 NPNMOD OFF
Q2 5 6 7 NPNMOD OFF
Q3 5 4 2 NPNMOD .3 OFF
Q4 6 5 3 PNPMOD OFF
Q5 4 5 7 PNPMOD OFF
D1 4 5 DMOD OFF
D2 6 5 DMOD OFF
R1 4 3 46.66667
R2 7 6 46.66667
R3 2 4 46.66667
R4 4 6 600000
*R5 7 8 7.38368E+05
R6 1 7 0.1
.MODEL DMOD D (IS=1.6E-15 RS=9.333333E-02 BV=600 IBV=0.000001 EG=1.11)
.MODEL NPNMOD NPN (IS=1.6E-13 BF=3 TF=2.55E-06 TR=3.642857E-04
+ CJC=1.665659E-10 CJE=8.328294E-10 EG=1.11)
.MODEL PNPMOD PNP (IS=1.6E-13 BF=1 CJE=8.328294E-10 EG=1.11)
* DATASHEET/DATABOOK: Motorola DL137, Rev.4, Q4/92
* VERSION: 2.0/0
* (C) ISD 04.11.1998 16:34:45 Prometheus V2.0.0
.ENDS
Above, I brought a Triac model on transistors. I think it can be adjusted to different control currents as you like. I think resistors R1, R2 and R3 are responsible for the values of control currents. Make them different and you get different control currents. I focus on the maximum control current. The control circuit must provide this current. And if you want to go your way and make the triac work badly, it is your right. It's all in your hands and you can simulate different control currents if you want to. I don't think it's important and judging by the models, I'm not the only one.
 

ci139

Joined Jul 11, 2016
1,463
good - but there is more to it - as the temperature rises the ON OFF control varies along . . . there might be more (i've not lately being busy by ...)

-- it's a complex device to model or to trust the simulation of . . . you must know what to expect as from the simulation as from the real device . . . especially if you are switching high power . . . things get wrong very fast if you can't predict and handle such . . . everything's COOL as long the load takes most of the power . . .
 

Bordodynov

Joined May 20, 2015
2,604
Even with temperature-independent shunt resistors, the required control currents are reduced as the temperature increases. Having added temperature dependence of resistors (increase in resistance at temperature increase) will slightly increase this temperature dependence.
There is a good negative example of the complexity of Infineon's field-effect transistor models. A slightly more complex circuit and there are almost insurmountable computational problems. And with these complex models, you can only calculate a simple circuit. You can of course make a similar model for triacs with thermal constants, but I am not interested.
 

ci139

Joined Jul 11, 2016
1,463
the only thing i'm trying to point out is that the REALITY and the SIMULATION are might be very different with devices such as triacs transistors bjt mosfet j-Fet . . . lesser with diodes , diacs . . . the small signal model of the BJT is hyper sensitive compared to real transistors (mostly -- depends on the particular circuit ...)

e.g. one thing is to run a simulation ... another thing is to run your actual circuit . . . as to my experience "Most of the time (90%) the SPICE can be used O_N_L_Y as an illustrative guide for a TEST setup. Only the 10% of the real world circuits´ll match the model \(\leftarrow\ \leftarrow\ \leftarrow\ \leftarrow\) read again. There are 60% "interesting" , 29% conceptually right , 9% matching / numerically-right , 2% such simulations that in real work up to a lot better."
 
Top