Originally posted by JoeJester@Jan 11 2006, 05:37 PM
So as I was revising the simulation, it came to me that the transistor would have to overcome the 1 mA current generator before the transistor could begin to conduct.

The current source internal resistance is set to infinite. Changing it to 1M didn't make much of a difference.

Anyways ... what am I missing in the simulation?

[post=13044]Quoted post[/post]​

Is that an initial condition (.IC) element connected to the transistor base in your circuit diagram? If so, why do you need to set it to 5V? The current source would try to sink the 1mA and the Ib and Ic would start conducting across the base-emitter and collector-emitter junctions on their own and reach a DC balance without any .IC condition or adjusting the current source resistance.

What simulation program (SPICE) are you using?

I've attached a partial output listing (I've cut out most of the rubbish and license info) of HSPICE run of the circuit below. Feel free to have a browse. Note that with the BJT model that I used I obtained:

Vb=1.92V
Ve=1.23V
Vc=1.54V
Vbe=0.69V

Ib=0.31mA
Ic=0.69mA

Those values might be a little bit difficult to find in the listing, but they are mostly under the *** operating point information **** heading.

 

Originally posted by JoeJester@Jan 11 2006, 11:37 AM

Now it has me wondering if the two resistors are tied to a +5V supply.

[post=13044]Quoted post[/post]​

I had the same question about the +5V connection when I looked at the schematic the first time. I do believe that the intent was that both the 10k base resistor and the 5K collector load resistor are tied to +5v.

One thing no one has touched on yet is the meaning of the given constraint that Va = infinite. I really don't know what that refers to.

hgmjr

 

Originally posted by hgmjr@Jan 11 2006, 07:44 PM
I had the same question about the +5V connection when I looked at the schematic the first time. I do believe that the intent was that both the 10k base resistor and the 5K collector load resistor are tied to +5v.

One thing no one has touched on yet is the meaning of the given constraint that Va = infinite. I really don't know what that refers to.

hgmjr

[post=13050]Quoted post[/post]​

VA or VAF is the forward early voltage. It determines the output conductance in forward region. If you plot the Ic against Vce for different values of Ib (transistor characteristic curves, ilustrated in this page) we wouldn't actually get perfectly horizontal lines in that region as illustrated. But instead those lines would have slightly positive gradients. If we extrapolated the lines towards the negative x axis, they would all converge to one single point on the negative x axis. This x value of this point is the early voltage. Although the point is negative early voltage is usually quoted as positive value.

VA is used to model the effect of base width modulation due to the Vce values (actually base-collector reverse bias voltage). If VA is infinite then the lines would all be perfectly horizontal (the extrapolations do not intersect the negative x axis), which means for a given Ib, different values of Vce in that region don't have any effect on the Ic (Beta is constant irrespective of Vce). This is not true for real-life device.

 

I'm using TINA which uses algorithms and models fully compatible with the 3F5 Berkeley Spice.

I ran a transient analysis, starting with zero values and it's congruent with your readings.

Anyways, the attachment is the results from the transient analysis.

I did change the transistor to a 2N3904. When I went back to the 2N4400, there wasn't significant differences in the transient results.

 

Originally posted by n9352527@Jan 11 2006, 02:06 PM
VA or VAF is the forward early voltage. It determines the output conductance in forward region. If you plot the Ic against Vce for different values of Ib (transistor characteristic curves, ilustrated in this page) we wouldn't actually get perfectly horizontal lines in that region as illustrated. But instead those lines would have slightly positive gradients. If we extrapolated the lines towards the negative x axis, they would all converge to one single point on the negative x axis. This x value of this point is the early voltage. Although the point is negative early voltage is usually quoted as positive value.

VA is used to model the effect of base width modulation due to the Vce values (actually base-collector reverse bias voltage). If VA is infinite then the lines would all be perfectly horizontal (the extrapolations do not intersect the negative x axis), which means for a given Ib, different values of Vce in that region don't have any effect on the Ic (Beta is constant irrespective of Vce). This is not true for real-life device.

[post=13052]Quoted post[/post]​

That is good information. I will be on the look out for that parameter in the future.

Thanks,
hgmjr

 

Originally posted by JoeJester@Jan 11 2006, 02:33 PM
I'm using TINA which uses algorithms and models fully compatible with the 3F5 Berkeley Spice.

I ran a transient analysis, starting with zero values and it's congruent with your readings.

Anyways, the attachment is the results from the transient analysis.

I did change the transistor to a 2N3904. When I went back to the 2N4400, there wasn't significant differences in the transient results.

[post=13056]Quoted post[/post]​

joejester,

I set up a pspice circuit just as you did using Orcad's Pspice Lite and I too ran into differences in the model's behaviour versus the desired parameters.

Since this is a quiescent DC anaylsis I decided to tweak the circuit to make it better fit the problem's stated givens.

For example, the transistor model I used ended up with a Vce(sat) of around 35 mV. Since the problem called for a Vce(sat) of 300mV, I decided to try introducing a dc voltage source in line with the collector and the 5K collector load resistor of 265 mV. I then proceeded to add another dc voltage source in line with the base of my model and the 10K base resistor. I set the value of this dc voltage to make up the difference between the Vbe that my model was yielding and the 700 mV called for by the problem statement.

Now, before you get to laughing too hard, I will admit that the tweaks I performed are highly unorthodox and would not be appropriate nor sanctioned in a real-world dynamic analysis. It was just an experiment I tried in order to get my model to better comform to the problems stated requirement. Since the voltage sources I used were "ideal" dc voltage sources, I think I did not stray too far from the intent of the problem and the results that I got were in very close agreement with the calculated values arrived at by N9352527.

All this being said, I would be interested in learning if your TINA spice program would give you closer agreement with the calculated values if you tried similar adjustments to your circuit.

hgmjr

 

hgmjr,

Yeah, we can force it closer with N93's numbers with the additioinal perfect supplies ... as seen below.

I did find a few interesting points. All involve the spice models. In the latest Tina, I have my choice of two different spice models for the 2N3904. Neither are consistent with the model that N93 used, and if I'm not mistaken, there are slight differences than the Fairchild Semiconductor spice model found in the datasheet at http://www.fairchildsemi.com/pf/2N/2N3904.html

The University of Rhode Island has an interesting treatise on the spice model for the 2N3904 ... found at http://www.ele.uri.edu/Courses/ele343/tuto.../q2n3904.model/

I haven't collated all the parameters from the different spice models I have, but I'll do that tomorrow. It would be interesting to see a side by side comparison of the different models.

 

Originally posted by JoeJester@Jan 12 2006, 12:28 AM
hgmjr,

Yeah, we can force it closer with N93's numbers with the additioinal perfect supplies ... as seen below.

I did find a few interesting points. All involve the spice models. In the latest Tina, I have my choice of two different spice models for the 2N3904. Neither are consistent with the model that N93 used, and if I'm not mistaken, there are slight differences than the Fairchild Semiconductor spice model found in the datasheet at http://www.fairchildsemi.com/pf/2N/2N3904.html

The University of Rhode Island has an interesting treatise on the spice model for the 2N3904 ... found at http://www.ele.uri.edu/Courses/ele343/tuto.../q2n3904.model/

I haven't collated all the parameters from the different spice models I have, but I'll do that tomorrow. It would be interesting to see a side by side comparison of the different models.

[post=13068]Quoted post[/post]​

The results you obtained agree nicely with the ones I obtained with my modified circuit. I think in the future when I am faced with a hypothetical static dc problem similar to this one, I will be more likely to consider resorting to a bit of circuit tweaking as a means of cross-checking the hand calculations using spice. I'm a bit of a novice when it comes to working with spice down at the device model level.

The two links you supplied were helpful in shedding light on some of the things that can be done at the device model level.

Thanks,
hgmjr

 

If you are interested in tweaking the models, curious on how SPICE simulates any physical element or just want to compare how the real physical devices differ with the ideal devices commonly taught and use in manual calculations you could browse through this HSPICE manual.

It has complete equations for various devices and elements. It is a big pdf file though, more than 10MB and close to 2000 pages.

 

Here's a easier link for the hspice model and quick reference guides from Stanford.

http://www.stanford.edu/class/ee133/hspice.html

 

Originally posted by JoeJester@Jan 12 2006, 11:05 AM
Here's a easier link for the hspice model and quick reference guides from Stanford.

http://www.stanford.edu/class/ee133/hspice.html

[post=13083]Quoted post[/post]​

I thank you all for joining me here. Your union and critics are unfathomable, and is a great joy.

regards,
CrktMan

 

To complete the spice reference ... you can get the pspice manual at:
http://www.ee.bilkent.edu.tr/~ee411/pspice...nce%20guide.pdf