¿ªÔÆÌåÓý

  1. LTspice
  2. Topics

MJ11021 Darlington NPN & PNP pair model help needed.

 

Hello,
New LTspice user.
?
I am trying to build a model for MJ11021 to be used in an AB amplifier simulation.? Link to .
I made an attempt in building a model for the part PNP type first.? I also created a simulation to validate against the datasheet.
Validation part 1: DC simulation to Verify hFE and VCE.??
Never got past part 1!?
Part 2: Transient simulation? to measure switching time.
?
I have uploaded the files to temp directory under /g/LTspice/files/Temp/MJ11021.zip
?
It is not working and I am having a hard time figuring out how to fix the parameters in order to get it validated.? Any help and guidance in how to proceed to fix/tune the model parameters and how to setup the simulation to validate the model against key datasheet specs. would be greatly appreciated.
?
Thank you in advance.
?
?
 

On Tue, Apr 22, 2025 at 10:01 PM, nima wrote:
I am trying to build a model for MJ11021 to be used in an AB amplifier simulation.? Link to .
I made an attempt in building a model for the part PNP type first.? I also created a simulation to validate against the datasheet.
Validation part 1: DC simulation to Verify hFE and VCE.??
Never got past part 1!?
The main problem is this:? Your subcircuit pin-order is wrong.
?
The 'standard' SPICE pin-order for BJTs is C-B-E.? For .SUBCKT models you do not absolutely need to use that order, but it's a good idea if you do.? Your Darlington symbol uses that order.? But your .SUBCKT model definition has the wrong order, meaning that it does not agree with the Darlington symbol:
.SUBCKT MJ11021 B C E
Change that line, to this:
.SUBCKT MJ11021 C B E
and I think most of the problems go away; at least it gets you going in the right direction.
?
While you are editing the model file, also fix the last line:
.END
which must not be the .END command.? It should be this:
.ENDS
?
I also note that your .DC command has the wrong polarity for the increment value:
.dc V2 -1 -2.8 0.2
which should be:
.dc V2 -1 -2.8 -0.2
It might be better to use a current source instead of a voltage source, to drive the base pin.? But that's up to you.
?
Andy
?
 

¿ªÔÆÌåÓý

On 23/04/2025 03:01, nima via groups.io wrote:
I am trying to build a model for MJ11021 to be used in an AB amplifier simulation.? Link to .
I made an attempt in building a model for the part PNP type first.? I also created a simulation to validate against the datasheet.
Validation part 1: DC simulation to Verify hFE and VCE.??
Never got past part 1!?
Part 2: Transient simulation? to measure switching time.
?
I have uploaded the files to temp directory under /g/LTspice/files/Temp/MJ11021.zip
?
It is not working and I am having a hard time figuring out how to fix the parameters in order to get it validated.? Any help and guidance in how to proceed to fix/tune the model parameters and how to setup the simulation to validate the model against key datasheet specs. would be greatly appreciated.
Developing a SPICE model for a Darlington is a considerable undertaking. Unfortunately, the Onsemi datasheet is not quite comprehensive enough to derive an accurate one.

The good news is that although Onsemi don't provide SPICE models for either of these devices, it does for the similar MJH11021 and MJH11022 transistors. These will be the same die, but in TO-247 packages instead of TO-3. Perhaps you were unaware of these modern equivalents?




You should nevertheless validate these models, at least partially. I recommend you construct several testjigs to re-generate the the graphs in the datasheet. Unfortunately, graphs for the output characteristic and FT are not shown, but you should check:
  1. Switching Time (Figure 2)
  2. The "On" Voltage (Figure 8 in the MJH11021/22 datasheet
  3. Figure 6 - DC Current Gain
  4. Figure 7 - Collector Saturation Region
--
Regards,
Tony

 

Andy,
Thank you for pointing out my mistakes. I will correct them. I started with current source as the obvious choice. I will go back to it.?
Thank you for your help.
Nima
 

Tony,
I was not aware!
I will use them and test.
Thank you for your prompt response.
Nima
 

On Wed, Apr 23, 2025 at 04:14 AM, Tony Casey wrote:
The good news is that although Onsemi don't provide SPICE models for either of these devices, it does for the similar MJH11021 and MJH11022 transistors. These will be the same die, but in TO-247 packages instead of TO-3. ...
If they are the same die, then their SPICE models would be the same.? SPICE transistor models usually do not include the package (unless they are for upper RF frequencies).
?
Andy

1 - 6 of 6