10m45s LTspice model

dave slagle · 2009-03-06 10:25 pm

Title says it all. I googled around a bit with no luck. Does anybody have a spice model for the 10M45S?

thanks

dave

dsavitsk · 2009-03-06 10:55 pm

Dave, It's just a depletion mode mosfet, and basically the same as a DN2540, if that helps.

kenpeter · 2009-03-07 12:54 am

http://www.ixyspower.com/PSpice_Model/HIGH_VOLTAGE/High_Voltage_Current_Regulator.asp

10M90S pspice model might be close enough.

rdf · 2009-03-07 7:05 am

dsavitsk said:
Dave, It's just a depletion mode mosfet, and basically the same as a DN2540, if that helps.

Are you sure? Many times I've read it also contains an amplifier, never anything authoritative though.

edit: Is that P-Spice model LT compatible?

dsavitsk · 2009-03-07 7:14 am

rdf said:
Are you sure? Many times I've read it also contains an amplifier, never anything authoritative though.

I'm not sure of anything ... well, except that the 2540 will drop in as a replacement and that Walt Jung says they are both depletion mode mosfets.

http://www.audioxpress.com/magsdirx/ax/addenda/media/jung2779.pdf

Part one, for anyone that missed it is at http://www.audioxpress.com/magsdirx/ax/addenda/media/jung2778.pdf

revintage · 2009-03-07 9:54 am

I use the DN2540 model I got from Supertex website in LTSpice without problems.

TheGimp · 2011-10-17 9:17 pm

I downloaded the supertex.lib file from their web site and usd a .lib directive to point to it.

.lib "C:\LTC Spice\Models\supertex.lib"

However, I get an error message "Only a level 9 B3SOI can have 5 nodes" when I try to run the simulation. Does anyone know what this is?

TheGimp · 2011-10-18 4:00 am

Nerry Mind.

Apparently there was a miss-match between the symbol file (*.asy) and the model in terms of pin specifications I had selected.

Defiant · 2011-10-18 11:57 am

I hope LT Spice does a better job with semiconductor models than it does with tube models. I ran curves on some Norman Koren models (5687 and 12AT7) and the lower negative grid voltage curves are all skewed and erratic.

I miss having access to HSpice

An externally hosted image should be here but it was not working when we last tested it.

Michael Koster · 2011-10-19 4:58 pm

All these parts are simple depletion mode MOSFETs. Someone guessed (IOW made it up) that they are ICs inside and that misinformation got echo chambered. Great example of "I read it somewhere". Why post information if you're not certain?

They are also NOT drop-in interchangeable. They will work similarly in some circuits but definitely not in all circuits.

Whether the model for one device can be substituted for another in Spice depends entirely on how sensitive the circuit is to the actual Vth and device capacitance etc. For example, a self-bias CCS using a different device may need to have a different value of Rs to achieve the same idle current.

The problem with bad results is in the models and not in the Spice platform. many models, especially tube models, are not very sophisticated and only model the device properly under the more common operating conditions.

cheers,

Michael

rdf · 2011-10-19 5:37 pm

Michael Koster said:
Great example of "I read it somewhere". Why post information if you're not certain?

From here? http://ixapps.ixys.com/DataSheet/88ede06d-3a1c-4a5a-bab8-5b4e89b3323c.pdf

tomlang · 2012-08-10 9:38 pm

Hi, looking for this model. The link for the 10m90s no longer works.

I'll settle for the supertex.lib though. However, not sure what is meant by

.lib "C:\LTC Spice\Models\supertex.lib"

Do I type the above as a SPICE directive after putting the supertex.lib file in the Models folder of LTC Spice?

thanks!

sulcorebutia · 2014-02-08 7:02 am

tomlang said:
Hi, looking for this model. The link for the 10m90s no longer works.

I'll settle for the supertex.lib though. However, not sure what is meant by

.lib "C:\LTC Spice\Models\supertex.lib"

Do I type the above as a SPICE directive after putting the supertex.lib file in the Models folder of LTC Spice?

thanks!

Tom, how about this

? One circuit with 10m90s, LND150 and DN2540

SM468 · 2020-04-30 10:01 pm

Thanks for posting the gyrator simulation. The gyrator file works on my LTspice XVII for OS X but when I try to use the IXCP10M90S.lib in another simulation I created, "Could not open file IXCP10m90S.lib". Any hint will be appreciated.

gerrittube · 2020-05-01 3:01 pm

All I can say is that I used the 10M90S (not sure where I found this one) as a substitute for the 10M45S and the differences between the model and actual measurements are that big that I don’t trust this kind of simulation. My measurements and ears seem to do a much better job in this particular case. If necessary I will look again into the 10M45S LTspice model. So just be carefull not to make too much judgements based on the simulation.

Regards, Gerrit

Koonw · 2020-05-01 4:34 pm

Try this model , save as .inc or just directive, needs to patch asy file for it to work (see attached), save the new asy file in asy directory and insert component for 10m45s.

Code:

.subckt 10M45S A G K
+params: Aol=100 GBW=10meg ref=3
 
M1 A 5 K K MOSFET1
* V1 4 G 3
G1 G 5 4 K {Aol}
R1 5 G 1
C1 5 G {Aol/GBW/6.28318530717959}
G2 G 4 value={(ref+V(A,K)/500)}
R2 4 G 1
 
.model MOSFET1 VDMOS(Rg=2 Vto=4.85 Rd=1m Rs=1m Rb=1.2m Kp=33
+lambda=0.01 Cgs=1.4n Cgdmin=48p Cgdmax=1.9n Cjo=4n Is=2n Vds=450
+Ron=0.92 Qg=48n)
.ends

NMOS asy for 10m45s:-

Code:

Version 4
SymbolType CELL
LINE Normal 48 48 48 96
LINE Normal 16 80 48 80
LINE Normal 40 48 48 48
LINE Normal 16 48 40 44
LINE Normal 16 48 40 52
LINE Normal 40 44 40 52
LINE Normal 16 8 16 24
LINE Normal 16 40 16 56
LINE Normal 16 72 16 88
LINE Normal 0 80 8 80
LINE Normal 8 16 8 80
LINE Normal 48 16 16 16
LINE Normal 48 0 48 16
WINDOW 0 56 32 Left 2
WINDOW 3 56 72 Left 2
SYMATTR Value NMOS
SYMATTR Prefix X
SYMATTR 10M45S
PIN 48 0 NONE 0
PINATTR PinName A
PINATTR SpiceOrder 1
PIN 0 80 NONE 0
PINATTR PinName G
PINATTR SpiceOrder 2
PIN 48 96 NONE 0
PINATTR PinName K
PINATTR SpiceOrder 3

SM468 · 2020-05-02 1:37 am

Thanks, the 10M45S file does not work for me. Can't open file library in LTspice.

Koonw · 2020-05-02 3:16 am

SM468 said:
Thanks, the 10M45S file does not work for me. Can't open file library in LTspice.

I believe the error message you encountered is because you run sim using IXCP10m90S not 10M45S as 10M45S does not required a .lib file. If so, just click Tools, Control Panel to include the library search path for IXCP10m90S.lib, this is because the .lib directive does not seem to work hence additional search path.

Koonw · 2020-05-02 4:46 am

I create a new symbol asy for 10M45S to be consistent with 10M90S and include the .inc files as below and you should include the lib search path as before:-

Code:

Version 4
SymbolType BLOCK
RECTANGLE Normal 33 49 -48 -48
WINDOW 0 33 -47 Bottom 2
WINDOW 3 33 -7 Left 2
SYMATTR Value IXCP10M45S
SYMATTR Prefix X
SYMATTR ModelFile IXCP10M45S.inc
PIN 0 -48 TOP 8
PINATTR PinName A
PINATTR SpiceOrder 1
PIN -48 0 LEFT 8
PINATTR PinName G
PINATTR SpiceOrder 2
PIN 0 48 BOTTOM 8
PINATTR PinName K
 PINATTR SpiceOrder 3

IXCP10M45S.inc, only change the name, no other changes.

Code:

.subckt IXCP10M45S A G K
+params: Aol=100 GBW=10meg ref=3
 
M1 A 5 K K MOSFET1
* V1 4 G 3
G1 G 5 4 K {Aol}
R1 5 G 1
C1 5 G {Aol/GBW/6.28318530717959}
G2 G 4 value={(ref+V(A,K)/500)}
R2 4 G 1
 
.model MOSFET1 VDMOS(Rg=2 Vto=4.85 Rd=1m Rs=1m Rb=1.2m Kp=33
+lambda=0.01 Cgs=1.4n Cgdmin=48p Cgdmax=1.9n Cjo=4n Is=2n Vds=450
+Ron=0.92 Qg=48n)
.ends

10m45s LTspice model

Member

diyAudio Member

Member

Member

diyAudio Member

Member

Member

Member

Member

Member

Member

Member

Member

Attachments

Member

Member

Disabled Account

Member

Disabled Account

Attachments

Disabled Account

Attachments