[SOLVED] Orcad PSice Creed Z-FET models

[OB_1]

Orcad PSpice Creed Z-FET models

Hi everyone,
I’m having troubles using PSpice models of the J-FET built by Cree. After importing “.lib” and “.olb” files the simulation stops with the following:

** Creating circuit file "bias.cir"
** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS

*Libraries:
* Profile Libraries :
* Local Libraries :
* From [PSPICE NETLIST] section of C:\OrCAD\OrCAD_16.0\tools\PSpice\PSpice.ini file:
.lib "C:\OrCAD\OrCAD_16.0\tools\pspice\library\Cree_Z-FET_Models_Rev0p3.lib"
.lib "C:\OrCAD\OrCAD_16.0\tools\pspice\library\EPC.lib"
.lib "C:\OrCAD\OrCAD_16.0\tools\pspice\library\small_signal_L0.lib"
.lib "C:\OrCAD\OrCAD_16.0\tools\pspice\library\small_signal.lib"
.lib "C:\OrCAD\OrCAD_16.0\tools\pspice\library\OptiMOS3_150V_200V_250V.lib"
.lib "C:\OrCAD\OrCAD_16.0\tools\pspice\library\CoolMOS_simplified_Spice_models.lib"
.lib "C:\OrCAD\OrCAD_16.0\tools\pspice\library\CoolMOS_standard_PSpice.lib"
.lib "C:\OrCAD\OrCAD_16.0\tools\pspice\UserLib\ina122_2.lib"
.lib "C:\OrCAD\OrCAD_16.0\tools\pspice\UserLib\INA122.lib"
.lib "nom.lib"

*Analysis directives:
.AC DEC 500 1 3G
.PROBE V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*))
.INC "..\SCHEMATIC1.net"



**** INCLUDING SCHEMATIC1.net ****
* source CREE
V_V5 0 N23716 AC 2V
+SIN 0V 2V 1MHz 0 0 0
R_R1 N23456 0 1k
X_U7 N23456 N23432 N23446 CMF10120
R_R3 N23712 0 1k
V_V2 N23432 N23446 0Vdc
V_V6 N23692 N23878 0Vdc
X_U12 N23716 N23692 N23878 GMOS
X_U8 N23586 N23540 N23576 CMF20120
X_U10 N23460 N23432 N23446 CMF10120
V_V3 0 N23590 AC 2V
+SIN 0V 2V 1MHz 0 0 0
R_R2 N23586 0 1k
V_V4 N23540 N23576 0Vdc
X_U9 N23712 N23692 N23878 GMOS
X_U11 N23590 N23540 N23576 CMF20120
V_V1 0 N23460 AC 2V
+SIN 0V 2V 1MHz 0 0 0

**** RESUMING bias.cir ****
.END

WARNING -- Library file C:\OrCAD\OrCAD_16.0\tools\pspice\library\Cree_Z-FET_Models_Rev0p3.lib has changed since index file Cree_Z-FET_Models_Rev0p3.ind was created.
WARNING -- The timestamp changed from Wed May 29 21:28:44 2013 to Wed May 29 22:05:34 2013.
Making new index file Cree_Z-FET_Models_Rev0p3.ind for library file Cree_Z-FET_Models_Rev0p3.lib
Index has 5 entries from 1 file(s).


**** EXPANSION OF SUBCIRCUIT X_U7 ****
.param af1 1
X_U7.xgmos params xgmos.af af1
---------------------------$
ERROR -- Invalid number
$
ERROR -- Bad value
X_U7.Ls1 N23446 X_U7.s1 7e-9
X_U7.Rs2 N23446 X_U7.s1 100
X_U7.Rg1 X_U7.g1 X_U7.g2 {14/af1}
X_U7.Lg1 N23432 X_U7.g2 7e-9
X_U7.rdrain N23456 X_U7.d1 {0.08/af1} tc1
--------------------------------------$
ERROR -- unknown parameter
+ 0.000835209 tc2 2.94329E-05
X_U7.XCGD params XCGD.af af1
-------------------------$
ERROR -- Invalid number
$
ERROR -- Bad value


**** EXPANSION OF SUBCIRCUIT X_U8 ****
.param af1 2
X_U8.xgmos params xgmos.af af1
---------------------------$
ERROR -- Invalid number
$
ERROR -- Bad value
X_U8.Ls1 N23576 X_U8.s1 7e-9
X_U8.Rs2 N23576 X_U8.s1 100
X_U8.Rg1 X_U8.g1 X_U8.g2 {(14/af1)-2}
X_U8.Lg1 N23540 X_U8.g2 7e-9
X_U8.rdrain N23586 X_U8.d1 {(0.08+0.01)/af1} tc1
---------------------------------------------$
ERROR -- unknown parameter
+ 0.000835209 tc2 2.94329E-05
X_U8.XCGD params XCGD.af af1
-------------------------$
ERROR -- Invalid number
$
ERROR -- Bad value


**** EXPANSION OF SUBCIRCUIT X_U10 ****
.param af1 1
X_U10.xgmos params xgmos.af af1
----------------------------$
ERROR -- Invalid number
$
ERROR -- Bad value
X_U10.Ls1 N23446 X_U10.s1 7e-9
X_U10.Rs2 N23446 X_U10.s1 100
X_U10.Rg1 X_U10.g1 X_U10.g2 {14/af1}
X_U10.Lg1 N23432 X_U10.g2 7e-9
X_U10.rdrain N23460 X_U10.d1 {0.08/af1} tc1
----------------------------------------$
ERROR -- unknown parameter
+ 0.000835209 tc2 2.94329E-05
X_U10.XCGD params XCGD.af af1
--------------------------$
ERROR -- Invalid number
$
ERROR -- Bad value


**** EXPANSION OF SUBCIRCUIT X_U11 ****
.param af1 2
X_U11.xgmos params xgmos.af af1
----------------------------$
ERROR -- Invalid number
$
ERROR -- Bad value
X_U11.Ls1 N23576 X_U11.s1 7e-9
X_U11.Rs2 N23576 X_U11.s1 100
X_U11.Rg1 X_U11.g1 X_U11.g2 {(14/af1)-2}
X_U11.Lg1 N23540 X_U11.g2 7e-9
X_U11.rdrain N23590 X_U11.d1 {(0.08+0.01)/af1} tc1
-----------------------------------------------$
ERROR -- unknown parameter
+ 0.000835209 tc2 2.94329E-05
X_U11.XCGD params XCGD.af af1
--------------------------$
ERROR -- Invalid number
$
ERROR -- Bad value

Has anyone ever faced this issue yet?
Thanks a lot!

 

[abhajn]

On a quick look, it appears that the line
X_U10.rdrain N23460 X_U10.d1 {0.08/af1} tc1
has extra parameter name at the end without a value.

If you modify the .subckt for CMF10120 and CMF20120, and remove the tc1 in the rdrain statement, the Unknown parameter errors will go away.

Also, the "Invalid number" error for the statement X_U10.XCGD params XCGD.af af1
shows that the XCGD instance statement in the subckt needs to be rewritten as something like:
XCGD params: af= {af1}
The curly braces are necessary for PSpice to know that this is an expression and needs to be evaluated.


Hope this makes the simulation work.
If the lib doesnt work after these fixes, please upload the lib as well, or share its link.

 

[hzare]

I think you should add the Pspice model related to your device into lib. you can find it in websites by searching the device name.
Hope getting proper response.

 

[OB_1]

On a quick look, it appears that the line
X_U10.rdrain N23460 X_U10.d1 {0.08/af1} tc1
has extra parameter name at the end without a value.

If you modify the .subckt for CMF10120 and CMF20120, and remove the tc1 in the rdrain statement, the Unknown parameter errors will go away.

Also, the "Invalid number" error for the statement X_U10.XCGD params XCGD.af af1
shows that the XCGD instance statement in the subckt needs to be rewritten as something like:
XCGD params: af= {af1}
The curly braces are necessary for PSpice to know that this is an expression and needs to be evaluated.


Hope this makes the simulation work.
If the lib doesnt work after these fixes, please upload the lib as well, or share its link.

Thanks a lot for the replay.
I have modified the .lib file following your hints, but unfortunately it doesn’t fix the problem:
- deleting tc1 and tc2 parameter could be useful, but is it sure those numbers are not needed?
- using curly braces {af1} gives a error stating that “ …there is no sub-circuit to expand…”
In any case I’m attaching the .lib file --> View attachment Cree_ZFET_Models.zip
I extracted the .lib file and copied it to the folder where all other PSpice models are. Then, to create the .olb file, I went on “PSpice Model Editor”, File > Open (Cree_Z-FET_Models_Rev0p3.lib), then File > Export to Part Capture Library and created the .olb. Finally I imported the two mentioned files in Capture and PSpice.
Thanks again!

 

[abhajn]

Hi,
I have uploaded a modified version of the lib to make it PSpice-compatible. This should work.
Changes made:
- Changed TC1, TC2 to TC
- Changed ln to LOG
- Added param statements to subckts.

Please try it out.

 

[OB_1]

Dear abhajn,
thank you very much for your help. There were some other troubles in the .lib file, but I managed to fix them … partially:
I’ve made the same changes described in your previous post for the second component of the library and it works!! So really thanks, because I would not have made it without your help.
There still is a third component in the library, the “gmos”, that doesn’t work. Is seems like a 2 gate MOS, so I’ve to define 4 pins of the device, but there always is a floating pin error. More over, the simulation results from previous two devices look like they are not 100% reliable … I guess they didn’t put much interest in delivering they spice models.
If you want to give a look to the latest version of the .lib file here it is --> View attachment Cree_Z-FET_Models_Rev0p3_modified.rar
In any case, thanks again!