Large signal PSpice transistor models

BFR93a in the file I have has CJE of 3.2E-15, similar to BFP405. If this is altered to 2.2pF, an emitter excursion to -2.5V occurs.

RL

There is also an issue with CJC, in combination with RB, that defines the delay and speed of the falling edge of the emitter-follower rectifier. Capacitance with the same orders of magnitude difference show up, producing a spike, if significant.

Gummel-Poon BJT modeling is aimed at small-signal representations, where DC-biased variables are roughly static (even if non-linear). I've seen this combated with look-up tables, but it's slooooow.

Still can't see femtofarads in bipolar parts, considering size and packaging.

RL

Wrong. If you properly extract all the parameters it correctly models everything but deep saturation and injection into substrate. PSpice adds the ability to model that region (used to be useful in TTL days ;-); and also provides an alternate model, MEXTRAM.

The intrinsic device might go that low if the emitter is implanted rather than diffused.

From an Atmel process (Atmel46K, that I've run at 5GHz :-)....

cje_ceb_1x_mean = 1.02114E-14 ; 0.01pF !! ...Jim Thompson

Could you identify the parameters that ensure this accuracy? Does it include any of those presently missing?

RL

Wow! Were did you find 2N222s? Obsolete for decades, and damn expensive.

Gummel-Poon, particularly as implemented in Spice, IS a non-linear model...

NOT a trivial model ;-) ...Jim Thompson

Come on! In the Spice catalog, they're really cheap!

They were never 'cheap'.

The Spice ones are. You can't get much cheaper than LTSpice.

You sure?

Methinks the SPICE catalog says "Please Call".

Tim

You have spice models for '60s vintage three digit transistors?

Strange, I got it directly from NXP

Could you post your whole model, to check if there are more differences?

Pere

I still have some of them :) And Farnell still has them on stock (from several manufacturers...:

etc.

BTW, the interesting measurements are not on the 2N2222...

Pere

Ooops, seems that I missed one of the "2" on my post. Didn't get it on time!

Pere

Actually a BFR91A model, relabelled BFR93A, in an SOT23 package from Philips in 1995......BFR91A was SOT37. Same die.

Check out the Seimens model, though:

These are the values used in the LTspice distro.

I would like to see the Telefunken file, if there ever was one, but Vishay seems to have divested it's bipolar semiconductors entirely, since having 'incorporated' their ass.

RL

The last Telefunken (Temic) datasheet for bfr93 lists S parameters.

It looks like the Siemens spice model has a typo fF for pF. There's no way CJC could be three orders of magnitude larger than CJE in the same part.

RL

Here's what I have (from a Kevin Alyward - SuperSpice/Anasoft/Philips library)...

.SUBCKT BFR93A Q1 6 5 7 7 BFR91A

• SOT23 parasitic model Lb 4 5 .4n Le 7 8 .83n L1 2 4 .35n L2 1 6 .17n L3 3 8 .35n Ccb 4 6 71f Cbe 4 8 71f

• PHILIPS SEMICONDUCTORS Version: 1.0
• Filename: BFR91A.PRM Date: Feb 1992
• .MODEL BFR91A NPN
• IS = 1.32873E-015
• BF = 1.02000E+002
• NF = 1.00025E+000
• VAF = 5.19033E+001
• IKF = 8.15511E+000
• ISE = 1.39029E-014
• NE = 1.51292E+000
• BR = 1.76953E+001
• NR = 9.94038E-001
• VAR = 3.28032E+000
• IKR = 1.00000E+001
• ISC = 1.04297E-015
• NC = 1.18993E+000
• RB = 1.00000E+001
• IRB = 1.00000E-006
• RBM = 1.00000E+001
• RE = 7.63636E-001
• RC = 9.00000E+000
• EG = 1.11000E+000
• XTI = 3.00000E+000
• CJE = 2.03216E-012
• VJE = 6.00000E-001
• MJE = 2.90076E-001
• TF = 6.55790E-012
• XTF = 3.89752E+001
• VTF = 1.09308E+001
• ITF = 5.21078E-001
• CJC = 1.00353E-012
• VJC = 3.40808E-001
• MJC = 1.94223E-001 .ENDS ...Jim Thompson

Ok, so I tested this

C-----*-----3.3V Gen--50R---B | E 10nF | | 1k gnd | gnd

measuring Vb and Ve. Transistors: 2N2222a and BFR93a.

BFR93a: Generator is adjusted to Vdc=2.3V and 5Vpp.

At 1 MHz, the emitter signal waveform is a nice trapezoidal signal with a steeper slope when leaving the upper clipping level. The simulator predicts rounded tops and a somewhat upwards sloping bottom. At 27 MHz the Spice model predicts negative signal excursions. I could not observe them. But if I add some 5-10 pF at the emitter resistance to account for the probe, simulations and reality almost match.

At 27 MHz, Spice model predicts sinusoidal signal centered around 0 approx +-2.3. On the scope I see max +1.8 and min -1.5, i.e. there is some loss but the qualitative shape is ok. Of course, this is not what the circuit is expected to do, but indicates the model is ok. At 1 MHz, Spice model predicts bottom clipping but with positive slope of 1.9V/us. Measurements more or less confirm this.

At 27 MHz, a quite sinusoidal output signal of 4Vpp can be measured adjusting Vdc=1.3. The simulator predicts the same, although with a

Conclusion:

The Spice models are ok and they do model large signal behavior. It was my error to assume that there could be no negative signal excursions: this is only true at low frequencies. Somehow I thought that 27 MHz was dc for a 5 GHz transistor. But his is not the case for a high input impedance circuit, as JT pointed out.

Thanks to all.

Pere

This is the same Philips model listed in the LTspice group comparison, and currntly offered for download from NXP, though a later date is attributed to the file:

If the Siemens/Infineon model's CJE is altered from xE-15 to xE-12, it's performance more closely resembles the other three versions, in simulation.

RL