Tube DIY Asylum

Do It Yourself (DIY) paradise for tube and SET project builders.

Return to Tube DIY Asylum


Message Sort: Post Order or Asylum Reverse Threaded

IXYS 10M45 High Voltage CCS SPICE?

63.246.183.223

Posted on October 25, 2014 at 12:37:51
Triode_Kingdom
Audiophile

Posts: 10012
Location: Central Texas
Joined: September 24, 2006
Anyone know if this is available? I visited the IXYS site, but only found SPICE for the IXCP10M90S. I assume it's not the same.



 

Hide full thread outline!
    ...
RE: IXYS 10M45 High Voltage CCS SPICE?, posted on October 25, 2014 at 13:13:45
jazbo8
Audiophile

Posts: 70
Location: Europe
Joined: January 16, 2012
I got this from the Yahoo user group, I think...
===
.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

 

RE: IXYS 10M45 High Voltage CCS SPICE?, posted on October 25, 2014 at 14:43:57
Triode_Kingdom
Audiophile

Posts: 10012
Location: Central Texas
Joined: September 24, 2006
Thanks, I'll give it a try. What symbol do you use with this? A three-terminal MOSFET? I need to pick something out of the LTSPICE list.

EDIT: After a lot of effort, I still couldn't get this model to work. I'm not sure it's compatible with LTSPICE, and my SPICE language skills aren't sufficiently refined to convert it (if that's even possible). On a better note, I've switched to the DN2540 in cascode for the sim I'm working on. According to one source, it performs better than the 10M45 at higher frequencies, so maybe it's a better choice anyway. Thanks just the same!

 

RE: IXYS 10M45 High Voltage CCS SPICE?, posted on October 25, 2014 at 19:14:35
jorisdallaire
Audiophile

Posts: 356
Location: Quebec city
Joined: July 26, 2012
Hello mr. TK,

Personally i use the model for the 10M90 without problems (knock on wood). Contrary to you, i assumed they were the same except for the voltage rating. But then, this habit of assuming things has gotten me problems in the past :-)


I could not use the standard n-type mosfet symbol because the pinout is not the same. I modded the stock mosfet symbol and changed the pin assignment. However that is not the problem with the previous poster's model - its pinout fits standard nmos symbol.

I can make it to work this way:
Use the nmos symbol, go to advanced setting, set the "prefix" parameter to "X" and the "spicemodel" parameter to "10M45S" (without quotes). Of course the model goes into and .inc directive or in a included file.

In any case, here is a link to my symbol file that works with the 10M90 model. Save as into the Program Files/LTC/LTspiceIV/lib/sym directory or in your project's directory and it can be selected in the symbols menu.

Hope that helps.
Joris

 

Got it to work., posted on October 25, 2014 at 19:35:07
jorisdallaire
Audiophile

Posts: 356
Location: Quebec city
Joined: July 26, 2012
I can make it to work this way:
Use the nmos symbol, go to advanced setting, set the "prefix" parameter to "X" and the "spicemodel" parameter to "10M45S" (without quotes). Of course the model goes into and .inc directive or in a included file.

Results are different than for the 10M90S - The 10M45 model gives way too high current when Rset is lower than about 200 ohms, so I'd use the 10M90 model. FWIW my 10M90 sims corresponded to measurements made on an actual circuit that was using the 10M45S.

 

RE: Got it to work., posted on October 25, 2014 at 21:31:32
jazbo8
Audiophile

Posts: 70
Location: Europe
Joined: January 16, 2012
Sorry that the model did not work... I also neglected to include the comments that came with the model which may provide some clues about its behavior.

******************************************************
* Model generated on 27 Apr 2010
* Model format: LTspice
* IXCP10M45 macro model
* External node designations
* Node A -> anode (1)
* Node G -> gate (2)
* Node K -> cathode (3)
*
* G1, R1 & C1 model an idealized op-amp. Aol controls
* its open loop gain. Based on LT opamp.lib.
* The op-amp controls a MOSFET M1, to make the Voltage
* drop across a resistor between G & K equal a Voltage
* reference. The Vref source is made up by G2 & R2.
* It is altered by a fraction of V(A,K) to achieve a
* dynamic resistance of 160k where bias resistor = 300R,
* giving nominally 10mA of Ik.
******************************************************

.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

 

Thanks Guys!, posted on October 26, 2014 at 06:49:36
Triode_Kingdom
Audiophile

Posts: 10012
Location: Central Texas
Joined: September 24, 2006
I modeled the circuit using a pair of DN2450, but I've saved this info for future reference. Thanks!

 

Page processed in 0.027 seconds.