Stats

  • Locked Locked
  • Replies 3
  • Subscribers 65
  • Views 14896
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Infineon CoolMOS Spice problem

Elektrofreak

 Hello,

 i want to use an Infineon CoolMOS in a medium/high power switching application. The chip of choise is the IPD60R600E6. The spice model can be found here:

www.infineon.com/.../CoolMOS_simplified_Spice_models_C6E6CFD2_

I copied the source code from the file to a new .spi file. Then i added a new Item to my schematic, a nmos4 from the analogLib. I changed the model name to IPD60R600E6 an added the spice file to the library list.

 Then i changed the pin setup in the spice file to

.SUBCKT IPD60R600E6_L0 source gate bulk drain

because in the nmos4 lib it says that Source is pin 1, Gate is pin 2 etc. The bulk contact in the spice file is not connected because in the spice model it is connected to source.

Plotting the transfer characteristic i get far too high currents in the range of kA. Even with Vgs = 1V the transistor seems to conduct with the same current... (Vth>= 2.1V)

Any idea what i did wong? Is it the correct way to use a analogLib nmos4 and change the model name? I did the same with a IRF430 MOSFET and this worked without a problem.

 

Thanks in advance!

 

 

  • Seems OK to me, I just used the LIB file "as is", created "default rectangular" parts and wired up a trivial test circuit, I am getting currents of the order of Amps so I would reckon that to be "pretty normal". I suspect that you may have some issues with the pin mapping between the schematic part and the LIB file. Try the "default rectangle" symbols first and then move on to a "proper" symbol, this will at least confirm that the model / configuration is OK and the issue is with the pin mapping. There are some issues with the "Model Import Wizard and Pin Number mapping so, if you used this method, it might explain why this is not working. Personally, I would tend to leave the LIB file text alone and work from there.

  • Hi, thanks for your response!

     

    oldmouldy said:
    [...]I just used the LIB file "as is", created "default rectangular" parts and wired up a trivial test circuit[...]

     What do you mean with "default rectangular"parts? Could you describe what you did to make it work?

    What i did was not using the import wizard because it fails with unknown model parameters for the MOSFETs (after creating a portmap for all unknown devices). I just used a standard NMOS from the analogLib and changed the model name to the one in the spice file. This is what i also did with a IRF430 spice file and this worked out very well. Using the same pin mapping on the CoolMOS model it did not work. The plot of the transfer characteristics has nearly the right form but the current is in the order of 25 to 75 uA (DC Sweep over Vds from 0V to 500V, Vgs = 5V = const.).

  • Use the Model Editor, under PSpice Accessories in the product Program Group. Save the original model LIB file to a convenient location, File>Open in the Model Editor to open the LIB file, File>Save to write the PSpice formatting, File>Export to Capture Part Library, this will create an OLB file to use in Capture to place the parts in the schematic, these parts will have a "default rectangular" appearance for the subcircuit defined parts like the one that you are using. Since the model pins are named Source, Gate, Drain they should be readily identified for connecting.

    Another issue may well be that the IRF430 is defined as a Model, .model statement for the LIB definition and the part that you are trying to use is defined as a Sub-circuit, .subckt statement for the LIB definition. This will need a change to the PSpice Template from M^@REFDES ... for the mosfet model to X^@REFDES ... for a subcircuit. (If you create the "default" Capture symbol, you will see the PSpice Template definition for that graphical symbol in the properties.)

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.