[SOLVED] Orcad PSice Creed Z-FET models

Status
Not open for further replies.
O

OB_1

Junior Member level 1
Joined
Feb 8, 2013
Messages
15
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,283
Activity points
1,387
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:


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

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.
 
Reactions: OB_1

    O

    OB_1

    Points: 2
    Helpful Answer Positive Rating
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.
 



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!
 

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.
 

Attachments

  • Cree_Z-FET_Models_Rev0p3.zip
    1.7 KB · Views: 146
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!
 
Last edited:
Reactions: Mr.Cool

    Mr.Cool

    Points: 2
    Helpful Answer Positive Rating
Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…