Hi Ray, Try this
2HNK60_ runs in LT-IV and LT-XVII while 2HNK60h only runs correctly in LT-XVII.
The datasheet was lite on temp co's. If you can check the ST model temp co's and change them to suit, also body diode params if you need an accurate body diode model (but normally not needed for linear apps).
Code:
*VDMOS with subthreshold (c) Ian Hegglun
.model 2HNK60_ VDMOS (Rg=20 Vto={4.55-(6m-1m)*(Temp-25)} Lambda=3m
+ Rs={35m*(1+3.5m*(Temp-25))} Kp={1*((Temp+273)/(25+273))**-(2.4-1.5)}
+ Ksubthres={0.23*(1+4m*(Temp-25))} Mtriode={0.15} Rd={3*(1+5m*(Temp-25))}
+ Cgdmax=260p Cgdmin=10p a=2 Cgs=300p Cjo=100p m=0.3 VJ=0.75
+ Is=4n N=1.5 Eg=1.05 Rb={0.1*(1+2.5m*(Temp-25))}
+ Vds=600 Ron=4 Qg=11nC mfg=STIH2106)
*VDMOS with subthreshold (c) Ian Hegglun
.model 2HNK60h VDMOS (Rg=20 Vto=4.55 Kp=1
+ Rs=35m Ksubthres=0.23 Mtriode=0.15 Rd=3 Lambda=3m
+ Bex=-2.4 Vtotc=-6m Tksubthres1=4m Trs1=3.5m Trd1=5m
+ Cgdmax=260p Cgdmin=10p a=2 Cgs=300p Cjo=100p
+ m=0.3 VJ=0.75 IS=4n N=1.5 Eg=1.05 Rb=0.1 Trb1=2.5m
+ Vds=600 Ron=4 Qg=11nC mfg=STIH2106)The datasheet was lite on temp co's. If you can check the ST model temp co's and change them to suit, also body diode params if you need an accurate body diode model (but normally not needed for linear apps).
Thanks, Ian. I'm still trying to learn about the VDMOS models and I appreciate your help. I looked at the attached subcircuit model and it doesn't appear to have any tempco data in it, saying only that the subcircuit is valid at 25 degrees C.
Is there any information in the subcircuit that can be used to update the VDMOS model?
Thanks again.
Is there any information in the subcircuit that can be used to update the VDMOS model?
Thanks again.
Code:
*
* _/_/_/_/_/_/
* _/ _/
* _/_/ _/ STMicroelectronics
* _/ _/
* _/_/_/ _/
* [URL="http://www.st.com"]www.st.com[/URL]
*
*
*****************************************************
* Model Generated by STMicroelectronics *
* All Rights Reserved *
* Commercial Use or Resale Restricted *
*****************************************************
* CREATION DATES: 17-11-2006 *
* *
* POWER MOSFET Model (level 3) *
* *
* EXTERNAL PINS DESCRIPTION: *
* *
* PIN 1 -> Drain *
* PIN 2 -> Gate *
* PIN 3 -> Source *
* *
* ****C**** *
* ********************** *
* *************************************** *
* PARAMETER MODELS EXTRACTED FROM MEASURED DATA *
* <<<<<<<<<<<>>>>>>>>>>> *
* *************************************** *
* THIS MODEL CAN BE USED AT TEMPERATURE: 25 °C *
* *
*****************************************************
* MODELLING FOR STF2HNK60Z
.SUBCKT STF2HNK60Z 1 2 3
LG 2 4 7.5E-09
LS 12 3 7.5E-09
LD 6 1 4.5E-09
RG 4 5 6.001
RS 9 12 0.151
RD 7 6 3.487
RJ 8 7 0.354E-01
CGS 5 9 0.324E-09
CGD 7 10 0.357E-09
CK 11 7 0.427E-11
DGD 11 7 DGD
DBS 12 6 DBS
DBD 9 7 DBD
MOS 13 5 9 9 MOS L=1u W=1u
E1 10 5 101 0 1
E2 11 5 102 0 1
E3 8 13 POLY(2) 6 8 6 12 0 0 0 0 0.255E-01
G1 0 100 7 5 1u
D1 100 101 DID
D2 102 100 DID
R1 101 0 1MEG
R2 102 0 1MEG
.MODEL MOS NMOS
+ LEVEL = 3
+ VTO = 4.807
+ PHI = 0.836
+ IS = 0.1E-12
+ JS = 0
+ THETA = 0.776E-01
+ KP = 2.922
.MODEL DGD D
+ IS = 0.1E-12
+ CJO = 0.375E-10
+ VJ = 0.776
+ M = 0.349
.MODEL DBD D
+ IS = 0.1E-12
+ CJO = 0.169E-10
+ VJ = 0.793
+ M = 0.336
.MODEL DBS D
+ IS = 0.1E-12
+ BV = 625
+ N = 1
+ TT = 0.199E-06
+ RS = 0.479E-02
.MODEL DID D
+ IS = 0.01E-12
+ RS = 0
+ BV = 635
.ENDS STF2HNK60Z
* END OF MODELLINGHi Ray,
The only change Rg=6.
The temp co's I used were taken from the IRF610 model as a best guess.
You could do a simple bench tests to get the main temp co - Vtotc
In my quest to learn more about VDMOS models I came across the following link:
Create An Accurate MOSFET Model For LTSpice — The Maxwell Times
This references a utility that can automatically generate LTspice VDMOS models from datasheet information. Has anyone used (or even tried) this utility? I'd like to get some opinions from the experts here before diving into this.
Thanks to all who can help.
Create An Accurate MOSFET Model For LTSpice — The Maxwell Times
This references a utility that can automatically generate LTspice VDMOS models from datasheet information. Has anyone used (or even tried) this utility? I'd like to get some opinions from the experts here before diving into this.
Thanks to all who can help.
It looks like no one had any interest in this utility other than me. 
Just to close the issue, I did play with it a little and although it did generate models as advertised I found that determining model parameters from datasheets was not as straightforward as I had hoped. So I probably won't pursue this any further myself.
Thanks to Ian and Bob for the earlier help.
Just to close the issue, I did play with it a little and although it did generate models as advertised I found that determining model parameters from datasheets was not as straightforward as I had hoped. So I probably won't pursue this any further myself.Thanks to Ian and Bob for the earlier help.
Hi Ray,
Thanks.
I was assuming you had a copy of my VDMOS tutorial (Part 1 PDF) from here
VDMOS - PAK2 devo
If you missed it, I summarize Hendrik Jan Zwerver equations from 'LTspice built in VDMOS model', 04 Dec 2006 here http://www.magma.ca/~legg/SR5/LTspice_build_in_VDmos_model.pdf
Then I tweak these parameters and you can see plots using my jigs sowing the changes versus the datasheet plots.
-------
Since writing that tutorial I have figured out how to use the OpenOffice spreadsheet to extract model parameters with the Sun Solver (an add-in utility). Around 1999 I used Excel's Solver to do this in the Level 1 MOSFET model with a User Defined Function, but their Solver algorithm was inadequate for the job. I have just discovered the Sun Solver add-in utility to Open Office and is a big improvement. But I haven't used it for VDMOS extractions yet.
One option is to include a slider for each parameter and plot half a dozen Vgs, Vds, Id (x,y) points on X,Y graphs. This doesn't need Solver to program this in a spreadsheet, you just need to add-in macros and enable them to use sliders in OpenOffice (or Excell etc)..
The advantage of a spreadsheet over VB (or whatever it is called now) is it can run on most OS's, and most spreadsheet coding can be understood by anyone.
BTW I have found Open Office spreadsheet Save As xls and runs 99.9% OK (as long as no macros are used). The complication is then the add-in's and macros.
Maybe the slider method could be automated using Solver? The sliders automatically move to the best positions by running Solver. Then, if you want different or better curves you can manually tweak using the sliders.
Just thinking aloud. Any thoughts on a strategy to automate the Zwerver equations and my tutorial into a useful piece of software that is easy to use?
Cheers,
IanH
Thanks.
I was assuming you had a copy of my VDMOS tutorial (Part 1 PDF) from here
VDMOS - PAK2 devo
If you missed it, I summarize Hendrik Jan Zwerver equations from 'LTspice built in VDMOS model', 04 Dec 2006 here http://www.magma.ca/~legg/SR5/LTspice_build_in_VDmos_model.pdf
Then I tweak these parameters and you can see plots using my jigs sowing the changes versus the datasheet plots.
-------
Since writing that tutorial I have figured out how to use the OpenOffice spreadsheet to extract model parameters with the Sun Solver (an add-in utility). Around 1999 I used Excel's Solver to do this in the Level 1 MOSFET model with a User Defined Function, but their Solver algorithm was inadequate for the job. I have just discovered the Sun Solver add-in utility to Open Office and is a big improvement. But I haven't used it for VDMOS extractions yet.
One option is to include a slider for each parameter and plot half a dozen Vgs, Vds, Id (x,y) points on X,Y graphs. This doesn't need Solver to program this in a spreadsheet, you just need to add-in macros and enable them to use sliders in OpenOffice (or Excell etc)..
The advantage of a spreadsheet over VB (or whatever it is called now) is it can run on most OS's, and most spreadsheet coding can be understood by anyone.
BTW I have found Open Office spreadsheet Save As xls and runs 99.9% OK (as long as no macros are used). The complication is then the add-in's and macros.
Maybe the slider method could be automated using Solver? The sliders automatically move to the best positions by running Solver. Then, if you want different or better curves you can manually tweak using the sliders.
Just thinking aloud. Any thoughts on a strategy to automate the Zwerver equations and my tutorial into a useful piece of software that is easy to use?
Cheers,
IanH
Ian,
Thank you for the very detailed message. It's clear that I have a lot to learn about the VDMOS models and I'll study the references you cited. A spreadsheet based approach does have more appeal than a standalone program from which the calculations are more difficult to decipher.
My primary goal is to be able to generate a model for a new (to me) MOSFET without having to bother the helpful people in this forum. For the time being, I think I have what I need for the devices that I design with most often. This will get me by until I can get a better grasp for how these models are developed.
Thanks again for your many informative posts.
Thank you for the very detailed message. It's clear that I have a lot to learn about the VDMOS models and I'll study the references you cited. A spreadsheet based approach does have more appeal than a standalone program from which the calculations are more difficult to decipher.
My primary goal is to be able to generate a model for a new (to me) MOSFET without having to bother the helpful people in this forum. For the time being, I think I have what I need for the devices that I design with most often. This will get me by until I can get a better grasp for how these models are developed.
Thanks again for your many informative posts.
5 generic electrothermal subcircuit 'widgets' for LTspice
Hi All,
This is to announce updated electrothermal subcircuits for LTspice. There are now 5 generic subcircuits covering BJT's, VDMOS, JFET's, Diodes and IGBT's.
'Generic' means they are add-on's to existing models for BJT's, VDMOS, JFET's, Diodes and IGBT's. You drag an drop the subcircuit on top of these parts in your circuit and convert that part to an electrothermal model rather than a fixed temperature.
You do this for the semiconductors that heat up, like power transistors, drivers and Vbe multipliers. But don't do more than necessary because the simulation will run too slow or it might never get started. I have had 9 widgets running in an amp and things starts slowing dramatically with more than 5.
A tutorial PDF for using these widgets and the LTspice demo jigs for the tutorial are here https://paklaunchsite.jimdofree.com/spice-models/
and examples of their recent use can be seen in this thread https://www.diyaudio.com/community/...ching-auto-bias-power-amp.375141/post-6885244
One area where they are really helpful is output stages that do not use any emitter resistors or source resistors to check the thermal stability and bias loops in standard amplifiers. They are also useful for checking for current hogging of parallel devices.
I have posted here because the idea for thermal interpolation came from keantoken by PM way back about 2013. So thanks again keantoken for your cool idea. It has been a great challenge and joy for me to get them to this stage for general use.
Questions, comments, bug reports and suggestions are all very welcome. If there is enough interest a new thread will be started.
Cheers,
Ian Hegglun
Hi All,
This is to announce updated electrothermal subcircuits for LTspice. There are now 5 generic subcircuits covering BJT's, VDMOS, JFET's, Diodes and IGBT's.
'Generic' means they are add-on's to existing models for BJT's, VDMOS, JFET's, Diodes and IGBT's. You drag an drop the subcircuit on top of these parts in your circuit and convert that part to an electrothermal model rather than a fixed temperature.
You do this for the semiconductors that heat up, like power transistors, drivers and Vbe multipliers. But don't do more than necessary because the simulation will run too slow or it might never get started. I have had 9 widgets running in an amp and things starts slowing dramatically with more than 5.
A tutorial PDF for using these widgets and the LTspice demo jigs for the tutorial are here https://paklaunchsite.jimdofree.com/spice-models/
and examples of their recent use can be seen in this thread https://www.diyaudio.com/community/...ching-auto-bias-power-amp.375141/post-6885244
One area where they are really helpful is output stages that do not use any emitter resistors or source resistors to check the thermal stability and bias loops in standard amplifiers. They are also useful for checking for current hogging of parallel devices.
I have posted here because the idea for thermal interpolation came from keantoken by PM way back about 2013. So thanks again keantoken for your cool idea
. It has been a great challenge and joy for me to get them to this stage for general use.Questions, comments, bug reports and suggestions are all very welcome. If there is enough interest a new thread will be started.
Cheers,
Ian Hegglun
Hi keantoken,
Nice to hear from you again. Yes, the BJT requires a different approach to the MOSFET for interpolation in the low current region which is exponential.
The key is the BJT requires base-emitter voltage sources that are scaled with Tj using scale factors of "Eg" (the energy gap voltage, for Si 1.11V) and XTI (the saturation current "Is" exponent with Tj), where the cold BJT is scaled with Tj (increasing) and the hot BJT is scaled with Tj2-Tj (decreasing).
You can spot these voltage sources using multipliers (E8 & E7) in the 'QthB.asc' subcircuit (attached).
Sources E3 and E4 are y-intercept offset voltages for the cold and hot transistors multipliers.
For more details see the tutorial PDF here https://paklaunchsite.jimdofree.com/spice-models/
This seems to work OK without needing the parameter XTI.
Nice to hear from you again. Yes, the BJT requires a different approach to the MOSFET for interpolation in the low current region which is exponential.
The key is the BJT requires base-emitter voltage sources that are scaled with Tj using scale factors of "Eg" (the energy gap voltage, for Si 1.11V) and XTI (the saturation current "Is" exponent with Tj), where the cold BJT is scaled with Tj (increasing) and the hot BJT is scaled with Tj2-Tj (decreasing).
You can spot these voltage sources using multipliers (E8 & E7) in the 'QthB.asc' subcircuit (attached).
Sources E3 and E4 are y-intercept offset voltages for the cold and hot transistors multipliers.
For more details see the tutorial PDF here https://paklaunchsite.jimdofree.com/spice-models/
This seems to work OK without needing the parameter XTI.
Thank you Ian for all of your hard work on this great contribution. It is a Christmas gift to our community.5 generic electrothermal subcircuit 'widgets' for LTspice
Hi All,
This is to announce updated electrothermal subcircuits for LTspice. There are now 5 generic subcircuits covering BJT's, VDMOS, JFET's, Diodes and IGBT's.
'Generic' means they are add-on's to existing models for BJT's, VDMOS, JFET's, Diodes and IGBT's. You drag an drop the subcircuit on top of these parts in your circuit and convert that part to an electrothermal model rather than a fixed temperature.
You do this for the semiconductors that heat up, like power transistors, drivers and Vbe multipliers. But don't do more than necessary because the simulation will run too slow or it might never get started. I have had 9 widgets running in an amp and things starts slowing dramatically with more than 5.
A tutorial PDF for using these widgets and the LTspice demo jigs for the tutorial are here https://paklaunchsite.jimdofree.com/spice-models/
and examples of their recent use can be seen in this thread https://www.diyaudio.com/community/...ching-auto-bias-power-amp.375141/post-6885244
One area where they are really helpful is output stages that do not use any emitter resistors or source resistors to check the thermal stability and bias loops in standard amplifiers. They are also useful for checking for current hogging of parallel devices.
I have posted here because the idea for thermal interpolation came from keantoken by PM way back about 2013. So thanks again keantoken for your cool idea
Questions, comments, bug reports and suggestions are all very welcome. If there is enough interest a new thread will be started.
Cheers,
Ian Hegglun
Merry Christmas and Happy New Year!
Cheers,
Bob