Hi everyone, I need clarification please. I was simulating a circuit with a 2SK545 as the gain stage but I have a problem in the simulation. I have two SPICE models available, the first called 2SK545 which derives from a database taken on LTWiki works and it gain while the second model which I called 2SK545-2 and which I took directly from the ONSEMI site and entered in the database does not work. This confuses me as I expect the model taken from the site to be corrected. So where is the problem? I have attached the .asc file for those who have LtSpice and also the images as well as the spice models used.
.MODEL 2SK545 NJF BETA=0.14 VTO=-1.1 LAMBDA=0.038 RD=5.6 RS=6.5 IS=0.56f CGS=0.32p CGD=0.32p M=0.33 PB=0.62 FC=0.5 N=1.016 MFG=ONSemi
.MODEL 2SK545-2 NJF BETA=48u VTO=-1.2 LAMBDA=0.01 RD=5.6 RS=6.5 IS=0.16f CGS=0.32p CGD=0.32p M=0.33 PB=0.62 FC=0.5 N=1.016 MFG=ONSemi

Thanks

 

Hi

Which one of these looks right to you?

2SK545-2:


2SK545:

 

Hi @eetech00

if i see the datasheet where the Id is 1mA i think the 2SK545-2 may be correct but i'm not expert enough to read your graphs. However (perhaps wrongly) I cannot get a valid configuration to have gain. Its a very sensible component.

 

hi Dan,
The upper plot in those diagrams shows a Drain current in the microampere region and the lower plot milliampere region.

A Drain current of only microamperes is not much use.

E

 

Hi @eetech00

if i see the datasheet where the Id is 1mA i think the 2SK545-2 may be correct but i'm not expert enough to read your graphs.

Yes. The 2SK545-2 is a close match to the datasheet, Figure 1.

 

@ericgibbs @eetech00
Hello, yes i've seen the differences between the two diagrams and agree the uA range is not useful ( usually i seen dran from 10 to 100mA for Jfets) but is derived form the spice model downloaded from the site. So why the spice from the site would give me a uA drain if is correct?

https://www.onsemi.com/pub/collateral/2sk545-11_model_rev0.txt

 

@ericgibbs @eetech00
Hello, yes i've seen the differences between the two diagrams and agree the uA range is not useful ( usually i seen dran from 10 to 100mA for Jfets) but is derived form the spice model downloaded from the site. So why the spice from the site would give me a uA drain if is correct?

https://www.onsemi.com/pub/collateral/2sk545-11_model_rev0.txt

Ask OnSemiconductor support.

 

The biggest discrepancy between the two models is the Beta value. Just guessing, but perhaps '48u' was intended to be '48m' ?

 

Hello,

Sometimes there is interplay between the different parameters. That is, two different parameters have similar effects when their values are adjusted. For a quick numerical example, say you have two params A and B. If you adjust A to 1.2 and B to 3.4 and get a result that is say 23, then if you adjust A to 2.4 and B to 6.8 and get a similar result, that indicates a linear dependency which is indicative of a redundant parameter.
To declare a redundant parameter the results dont have to match exactly but they should match closely.

When a model of anything is analyzed the equations can be rotated such that every parameter exists along a separate orthogonal dimension. So if you had three parameters you would have 3 dimensions, 4 parameters 4 dimensions, etc. If you end up with say 7 parameters but with just 6 dimensions, then you have 1 redundant parameter. In that case you may see two different values for constants in a model that basically do the smae
thing.

For this thread though it looks as if something is just in error. Some data point may have not been shown properly. This happens a lot on the web with equations although i have yet to find a spice model that is very far off, even though not exactly in match with another model.

 

For what it’s worth, there is a Sanyo equivalent. It has the same curve as the OnSemi (figure 1) device. However strange, it seems to be correct.

 

For what it’s worth, there is a Sanyo equivalent. It has the same curve as the OnSemi (figure 1) device. However strange, it seems to be correct.

Hello,

If there is no real error and two models are very different, then it has to be investigated further.
We might have to order parts and do some real hands on bench top testing.
Another possibility is to find some designs that have been already done and see how the different models change any measurements such as at an output node. For example, if one part gives us an amplifier gain that is 10 and the other 2, one of them probably isnt right.
Sometimes a circuit is designed with the possibility of a wide range of a parameter in mind. A good example of this is with transistor Beta where circuits are often designed knowing beforehand that the Beta can change a lot with many different operating conditions such as current and temperature.

 

I looked for schematics that used the 2SK545 but found practically nothing of significance. CF Maybe it is good to send an email to the semicon support and ask them never seems strange to me that they publish an incorrect spice model. Maybe you have an application example scheme that doesn't exist on the product page either. Or it is simply a component that is not designed to provide gain.

 

hi Dan,
The datasheet 'suggests' a uAmp range of Drain currents for a range of Vgs.??
You could be correct ref the low Id values.

Will keep searching.

E

 

hi Dan,
A different type of simulation shows the sim tracks OK against the D/S graph.

E

Added: ref the hfe, note the wide range. 30uA > 300uA

 

I looked for schematics that used the 2SK545 but found practically nothing of significance. CF Maybe it is good to send an email to the semicon support and ask them never seems strange to me that they publish an incorrect spice model. Maybe you have an application example scheme that doesn't exist on the product page either. Or it is simply a component that is not designed to provide gain.

You still don't understand. By definition a SPICE model CANNOT be incorrect if the simulation runs. It may or may not represent an actual part or even a particular manufacturing run of a particular part. It is a model of behavior and makes no representation that it covers all possible variations of a part. It is a valid question to ask: "How close is the model to an actual part that I can obtain from my supplier(s)". There is no point in whining about the situation and you're unlikely to get much in the way of help from any vendors. This is legwork you'll have to do for yourself.

EDIT: As a matter of record, I have collected 13 different models of the TIP31 power transistor from different sources. Out of 13 models, I have four that I consider to be "most representative" of actual parts. Comparing the models was impossible using text comparison tools because the parameters were not specified in a consistent order. I had to transcribe all 13 models into a spread sheet and compare each column to all of the others. Then I ran side by side simulations of each model to select the ones that matched my empirical data. That is how muck legwork can be required. Not once did I complain about the models being wrong. My default assumption was that all of the models were representative of a particular objective reality at some point in time. In many cases the models came from companies that no longer exist or have been absorbed into larger companies. I had no expectation of finding help from the larger acquisitors.

 

Maybe I explained myself wrong. I'm not complaining about anything !.
I use simulators as a first feasibility study. If the circuit works then sometimes (not always) I can think of replicating it on the breadboard. I just want to understand if this JFet based on the spice models, allows to create a real circuit that allows a gain or not. I also know that the components are all different but there is a big difference here. The same LtSpice a confirms that one model apparently earns and the other does not. So my question was to understand: Which of the two is more reliable? Because if the one downloaded from the manufacturer is more accurate then this Jfet is not for me and I will not use it. If, on the other hand, I got the scheme wrong then I ask how to correct it to obtain the expected gain.

 

Maybe I explained myself wrong. I'm not complaining about anything !.
I use simulators as a first feasibility study. If the circuit works then sometimes (not always) I can think of replicating it on the breadboard. I just want to understand if this JFet based on the spice models, allows to create a real circuit that allows a gain or not. I also know that the components are all different but there is a big difference here. The same LtSpice a confirms that one model apparently earns and the other does not. So my question was to understand: Which of the two is more reliable? Because if the one downloaded from the manufacturer is more accurate then this Jfet is not for me and I will not use it. If, on the other hand, I got the scheme wrong then I ask how to correct it to obtain the expected gain.

The answer is that you cannot know what the relationship between a given model and an actual device is unless you verify it for yourself or have someone you trust verify it for you. There is no a priori reason why any given JFET will not produce gain. The devil is in the details of the circuit configuration, not the device or the model used in simulation.

 

The answer is that you cannot know what the relationship between a given model and an actual device is unless you verify it for yourself or have someone you trust verify it for you. There is no a priori reason why any given JFET will not produce gain. The devil is in the details of the circuit configuration, not the device or the model used in simulation.

Of the many models that I have tried this and perhaps another are the only ones that I cannot simulate and I wanted to understand where the error is. The first post I wrote I asked for suggestions to understand where the problem was. I have attached asc diagram, images and everything that could be useful so as not to waste anyone too much time. An example even written in pencil would have been enough to make it easier for me to understand.

 

Of the many models that I have tried this and perhaps another are the only ones that I cannot simulate and I wanted to understand where the error is. The first post I wrote I asked for suggestions to understand where the problem was. I have attached asc diagram, images and everything that could be useful so as not to waste anyone too much time. An example even written in pencil would have been enough to make it easier for me to understand.

Hi

The bottom line is the OnSemi datasheet correctly matches the 2SK545-2 model, so that model has been partially confirmed correct. I would not use the other model.

You now have to make an assessment as to whether or not the 2SK545 is even suitable for your design.

In my opinion, the spice model issue is resolved. You should open a different thread for circuit design help.

 

Interesting. From the ONsemi site I see one of the models you are using, the -2 model, as part of a subcircuit with the parasitic elements specified explicitly.
This sub circuit might be closer to the mark than just the bare model.