1
\$\begingroup\$

I'm studying a circuit with BJT's and I'm asked to determine the input resistances of the two amplification steps of the circuit. The circuit I'm analyzing is the following one:

enter image description here

To determine the input resistances I performed an AC analysis and obtained the following results:

enter image description here

I know that the values are not perceptible but they are Rin1=23.272231 kohm and Rin2=220.77106 kohm. I decided to choose a somewhat random value in the zone of the graphic where the curves are constant (I'm not sure if this is correct...).

Well this value are very different from what I obtained when I analyze the theoretical values of the input resistances.

Using:

$$R_{i2}=(β+1) R_{E3}//R_L+r_{π2}$$

where r_{π2} is 9.375 kohm and beta is 300. I obtained R_i2=240.375 kΩ

And for Ri1

$$R_{i1}=R_1//R_2//(r_π1+R_{E1} (1+β))$$ I obtained R_i1=20.183kohm.

I used the small-signal analysis models to determine this...

Now this is odd. I'm getting an error of about 15% on Ri1 and 7% on Ri2. Am I doing something wrong or are this deviations perfectly normal and dependent on the methods used on the theoretical analysis and on LTSpice. Can someone help me clarify this?

\$\endgroup\$
  • \$\begingroup\$ Your uploaded picture needs re-saving and re-uploading. Have you used the transistors, separately, to determine their values? Models usually differ from real life. Also, you could try to use a current source at the input, and plot 1/V(vs), but I suspect it will be the same. \$\endgroup\$ – a concerned citizen Apr 22 '18 at 6:42
  • \$\begingroup\$ How do you determine the r_pi value? Also, LTspice includes ro resistance and VT at 27 degrees, \$\endgroup\$ – G36 Apr 22 '18 at 8:53
1
\$\begingroup\$

How does the SPICE model differ from hybrid-pi? Are those differences important?

\$\endgroup\$
  • \$\begingroup\$ Beta is slightly different (294.3 versus 300). Also the values of r_pi might be a little bit different, because the currents are slightly different than 0.8 mA. Will that be enough reason? \$\endgroup\$ – Granger Obliviate Apr 22 '18 at 2:44
0
\$\begingroup\$

At \$1 \textrm{kHz}\$ the \$C_E\$ capacitor reactance is around :

\$X_C \approx \frac{0.16}{F \cdot C}\approx 1.6\textrm{k}\Omega\$

So the \$Z_E\$ impedance will be around:

\$Z_E = R_{E1} + R_{E2}||X_{C_E} \approx 1.2 \textrm{k}\Omega \$

And input impedance is:

\$R_{in1} = R_1||R_2||(Z_E + r_e)(\beta+1) \approx 23.232 \textrm{k}\Omega\$

Rin1 = 1/( 1/68 + 1/39+1/((1.2+0.0325)*301))

I assume \$I_C = 0.8 \textrm{mA}\$ and \$r_e = \frac {26\textrm{mV}}{I_C} = 32.5\Omega\$

As for \$R_{in2}\$ is equal around:

\$ R_{in2} = (R_{E3}||R_L||r_o)(\beta+1)+r_{\pi2}\$

Because the LTspice includes \$r_o\$ (Early effect).

So to get almost exactly the same result you need to know \$ro\$ or Early voltage \$ \textrm{VAF}\$ in LTspice.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.