Wolfspeed SiC Mosfet OrCad Pspice Quick Start Guide Rev 1.0 Feb 2018x Si C Or Cad 2018

User Manual:

Open the PDF directly: View PDF .
Page Count: 13

Download
Open PDF In Browser	View PDF

Wolfspeed SiC MOSFET SPICE Model
Quick Start Guide
Power Applications
Rev1.0

Wolfspeed SiC MOSFET SPICE Model Quick Start Guide Rev 1.0, 02-2018
Copyright © 2018 Cree, Inc. All rights reserved.
The information in this document is subject to change without notice.
Cree, the Cree logo, and Zero Recovery are registered trademarks of Cree, Inc.

Table of Contents
1.
2.
2.1
2.2
2.3
2.4
3.
3.1
3.2
4.
5.
6.
6.1
7.

Introduction ................................................................................................................................................................. 3
OrCad Pspice Software.............................................................................................................................................. 3
Prerequisite.................................................................................................................................................................. 3
Package Contents....................................................................................................................................................... 3
Software Requirement .............................................................................................................................................. 4
Model Installation Guidelines .................................................................................................................................. 4
Model Specifications.................................................................................................................................................. 5
Model features............................................................................................................................................................. 5
Model Limitation......................................................................................................................................................... 5
Simulation Guidelines ............................................................................................................................................... 5
Migrating Wolfspeed SPICE model to others SPICE software ........................................................................... 8
Simulation Examples ................................................................................................................................................. 9
Simulation Example1................................................................................................................................................. 9
Revision History ........................................................................................................................................................ 12

DISCLAIMER
Models provided by WOLFSPEED are not warranted by WOLFSPEED, CREE as fully representing
all the specifications and operating characteristics of the semiconductor product to which the
model relates. The model describes the characteristics of a typical device. In all cases, the
current data sheet information for a given device is the final design guideline and the only
actual performance specification. Although models can be a useful tool in evaluating device
performance, they cannot model exact device performance under all conditions, nor are they
intended to replace laboratory testing for final verification. This model is preliminary and
subject to change without notice. CREE will not be responsible for any error or simulation issue
arising due to the editing of the model library file.

Introduction

The primary intention of building a SPICE model is to allow the users to create a converter circuit
and understand it’s design and performance parameters. With the simulation of SPICE model,
designers can save a lot of time by reducing the design cycles that lead to the early introduction
of the product into the market. Wolfspeed MOSFET SPICE models contain CXM0XXXXXXX and
CPMX-XXXX-XXXXX electro-thermal SPICE models for the packaged device and bare die. SPICE
models included a provision of self-heating to observe the change in junction temperature of the
device. These SPICE models provide a reasonable approximation for the MOSFET in the third
quadrant. However, the body diode threshold voltage was modeled at V GS = -4V (Gen 3) or -5V
(Gen2) and assumes this is fixed for all values of VGS. However, the effect of a slight change in the
turn-ON voltage of the body diode over the range of -4V ≤ V GS ≤ 0V is not modeled. 3rd quadrant of
the MOSFET is optimized and verified for Tc=25°C & 150°C at VGS = 15V (Gen 3) or 20V (Gen2). The
Model is most accurate at the IDS (DC) @ Tc=25°C & 150°C operating conditions as shown in the
device data sheet.

2. OrCad Pspice Software
2.1 Prerequisite:
OrCad Pspice simulation software

2.2 Package Contents:







SPICE Library Packaged Device Model (CXM0XXXXXXXD.lib) – Device model includes TO247 3Leads package.
SPICE Library Packaged Device Model (CXM0XXXXXXXK.lib or CXM0XXXXXXXP.lib) – Device
model includes TO-247 4Leads package.
SPICE Library Packaged Device Model (CXM0XXXXXXXJ.lib) – Device model includes TO263 7Leads package.
SPICE Library Bare Die Model (CPMX-XXXX-XXXXX.lib) – Die model does not include any
package parasitic.
PSPICE Device Symbol (Wolfspeed-TO247-3L.OLB, Wolfspeed-TO247-4L.OLB &
Wolfspeed-TO263-7L.OLB)
PSPICE Die Symbol (Wolfspeed-Die.OLB )

2.3 Software Requirement:
This model has been developed and optimized for Pspice. It is the responsibility of the user to be
well-versed with the basic operation of Pspice simulation tool.
Using this model library on other Pspice simulation tool may result in
convergence error or incorrect simulation result. Please use the
recommended software or verify the result before use.

2.4 Model Installation Guidelines:
1.
2.
3.
4.

Download the SPICE model at http://go.wolfspeed.com/all-models
Extract the zip file.
Verify the presence of all the files indicated in the package contents.
Copy the Wolfspeed Device Symbol file (.OLB) and paste it into the Pspice symbol directory.
Typical installation path is given by (C:\Cadence\SPB_XX\tools\capture
\library\pspice\modeled\ ). It is recommended to create a folder just for Wolfspeed
MOSFET at the path mentioned above. This would make the device symbol appear in the
component selection window. A software restart may be required to observe the change.
5. The device symbol will be like the one shown in figure 1. Pspice provides the option for
changing the visibility of the labels associated with the terminals.

Figure 1. Device symbol (reference purpose only).
Wolfspeed SiC MOSFET SPICE Model Quick Start Guide Rev 1.0, 02-2018
Copyright © 2018 Cree, Inc. All rights reserved.
The information in this document is subject to change without notice.
Cree, the Cree logo, and Zero Recovery are registered trademarks of Cree, Inc.

6. Copy the Wolfspeed MOSFET library file (.lib) and paste it into the Pspice library directory.
Typical installation path is given by ( C:\Cadence\SPB_XX\tools\pspice\library\
Wolfspeed diode).

3. Model Specifications
3.1 Model features







Optimized for 25°C & 150°C temperatures and gate to source voltage (V GS) of 15V (Gen 3) or
20V (Gen2). Modest accuracy on the rest of Vgs for 25 oC & 150oC temperatures.
Valid for temperature range -55°C to 150°C
Optimized and verified for 25°C & 150°C temperatures and gate to source voltage (V GS) of
15V (Gen 3) or 20V (Gen2) for 3rd Quadrant only.
Body diode operation optimized for VGS = -4V (Gen 3) or -5 (Gen 2)
The model includes self-heating and transient thermal capability.
Parasitic inductance associated with electrodes will be included in the model .

3.2 Model Limitation




Parasitic BJT and its associated effects not modeled.
Avalanche multiplication process not modeled.
Variation of body diode turn-ON voltage with gate to source voltage (V GS) is not modeled.

Simulation Guidelines:

The SiC Pspice model is provided with the following terminals:







Drain
Gate
Kelvin (Except on TO-247- 3 lead package & die model)
Source
Junction Temperature terminal - Tj
Case Temperature – Tc (Except on die models)

The same symbol consists of different MOSFET models if the pin count is the same. For example,
Wolfspeed-TO247_4L.OLB consists of MOSFET models like C3M0065100K, C3M0120100K or any
Wolfspeed SiC MOSFET SPICE Model Quick Start Guide Rev 1.0, 02-2018
Copyright © 2018 Cree, Inc. All rights reserved.
The information in this document is subject to change without notice.
Cree, the Cree logo, and Zero Recovery are registered trademarks of Cree, Inc.

MOSFETs with 4 leads. It is also applied to Wolfspeed-TO263-7.OLB symbol for MOSFET model
C3M0065100J, C3M0120090J or any MOSFETs with 7 leads. Once the symbol is selected from
libraries, a list of available MOSFETs with their part numbers will be shown on the part list to allow
the user to pick a MOSFET to perform the simulation.

Figure 2: Wolfspeed-TO247-3L with a list of available 3 leads MOSFETs

The user is required to include the library path at each circuit design. This is to provide Pspice the
path where the library is located and it can be done at “simulation profiles”.

The model library file (.lib) should not be edited under any circumstance
as it may result in convergence error, incorrect simulation result or longer
simulation time.

The terminals Tj and Tc were specifically included in the design to analyze the self-heating of the
device as a function of time. The terminal Tc represents the case temperature and Tj represents
the junction temperature. The temperature connections are working as voltage pins. Therefore, a
potential difference of 1V refers to a temperature difference of 1°C.
The Junction Temperature terminal (Tj) can either be used to read
junction temperature or to apply a junction temperature. This terminal
can be left floating.

The voltage at the Tj node contains the information about the time-dependent junction
temperature which in turn acts directly on the temperature-dependent electrical model.
The Case Temperature terminal (Tc) must be connected to either a voltage
source or a Heat Sink RC Network. This terminal can be left floating.

The Tc terminal should be connected to either a voltage source (which denotes the case
temperature) or to an external RC network (heat sink model) to observe its effect on the junction
temperature. Figure 3 shows the connection of Tc terminal to an ambient temperature of 25°C.

Figure 3: Fixing Case Temperature (Tc) to 25°C
Wolfspeed SiC MOSFET SPICE Model Quick Start Guide Rev 1.0, 02-2018
Copyright © 2018 Cree, Inc. All rights reserved.
The information in this document is subject to change without notice.
Cree, the Cree logo, and Zero Recovery are registered trademarks of Cree, Inc.

Either Tj or Tc must be connected to a voltage source to converge properly.

To perform DC simulation, the junction temperature (Tj) must be
connected to a voltage source to fix the junction temperature to a
constant value.

To use the model for generating DC characteristics at a particular junction temperature, the
junction temperature has to be fixed at a constant value. This can be achieved by connecting the
terminal Tj to a fixed voltage source as shown in figure 4.

Figure 4: Junction maintained at a constant temperature of 125°C for DC simulation.

Migrating Wolfspeed SPICE model to others SPICE software

Wolfspeed MOSFET SPICE models are both LTspice and OrCad Pspice compatible. To use
Wolfspeed MOSFET SPICE model on other SPICE software, the user may need to do few more steps
to get it work. Some SPICE software uses different extension like SIMetrix uses the library with
extension .lb whereas Pspice and LTspice use extension .lib. Besides that, Pspice, LTspice &
SIMetrix uses their own symbol format thus user should create their own symbol.
Note: It is the responsibility of the user to verify the model against datasheet after changing the format
of the model.
Wolfspeed SiC MOSFET SPICE Model Quick Start Guide Rev 1.0, 02-2018
Copyright © 2018 Cree, Inc. All rights reserved.
The information in this document is subject to change without notice.
Cree, the Cree logo, and Zero Recovery are registered trademarks of Cree, Inc.

6. Simulation Examples
6.1 Simulation Example1:
The schematic in Figure 5 shows the Pspice model of the Boost converter. The purpose of this
example is to show the connection of Kelvin source, Junction temperature terminal and including
the library path.

Figure 5. PSPICE model of the Boost converter

If encountered convergence error, the user can enable the Advanced Convergence and
Auto Converge simulation setting. If the error persists, adding capacitance between 1E14 to 1E-12 at cshunt will help to solve the issue. It is the responsibility of the user to
ensure that the addition of small capacitance has not affected the simulation result.

Waveforms of Drain Voltage (Green) and Drain Current (Blue) are shown in figure 6, 7 & 8.

Figure 6. Waveform Screenshot obtained from Pspice Simulation of Boost converter

Figure 7. SiC MOSFET Turn-ON Event

Figure 8. SiC MOSFET Turn-OFF Event

Revision History

Date
02/21/2018

Revision
V1.0

Changes
Initial release

Source Exif Data:

File Type                       : PDF
File Type Extension             : pdf
MIME Type                       : application/pdf
PDF Version                     : 1.7
Linearized                      : No
Warning                         : Info object (160 0 obj) not found at 1488861

EXIF Metadata provided by EXIF.tools

Wolfspeed SiC Mosfet OrCad Pspice Quick Start Guide Rev 1.0 Feb 2018x Si C Or Cad 2018

Navigation menu

Versions of this User Manual:

Views

Navigation