Wolfspeed SiC Mosfet LTspice Quick Start Guide Rev 2.0 Feb 2018x Si C 2018

User Manual:

Open the PDF directly: View PDF .
Page Count: 14

Download
Open PDF In Browser	View PDF

Wolfspeed SiC MOSFET LTspice Model
Quick Start Guide
Power Applications
Rev2.0

Wolfspeed SiC MOSFET LTspice Model Quick Start Guide Rev 2.0, 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
6.2
7.

Introduction ................................................................................................................................................................. 3
LTspice 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 LTspice model to others SPICE softwares ...................................................................... 8
Simulation Examples ................................................................................................................................................. 9
Simulation Example1................................................................................................................................................. 9
Simulation Example 2.............................................................................................................................................. 12
Revision History ....................................................................................................................................................... 1 3

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 LTspice model is to allow the users to create a converter circuit
and understand it’s design and performance parameters. With the simulation of LTspice 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 LTspice models contain CXM0XXXXXXX and
CPMX-XXXX-XXXXX electro-thermal LTspice models for the packaged device and bare die. LTspice
models included a provision of self-heating to observe the change in junction temperature of the
device. These LTspice 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. LTspice Software
2.1 Prerequisite:
LTspice simulation software (http://www.linear.com/designtools/software/#LTspice)

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.
LTSPICE Device Symbol (nmos TO247_3L.asy, nmos TO247_4L.asy & nmos
TO263_7L.asy)
LTSPICE Die Symbol (nmos_die.asy)

2.3 Software Requirement:
This model has been developed and optimized for LTspice. It is the responsibility of the user to be
well-versed with the basic operation of LTspice simulation tool.
Using this model library on other SPICE 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 LTspice 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 (. asy) and paste it into the LTspice symbol
directory. Typical installation path is given by (C:\Program
Files
(x86)\LTC\LTspiceIV\lib\sym ). 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. LTspice provides the option for
changing the visibility of the labels associated with the terminals.

Figure 1. Device symbol in a schematic (reference purpose only).
Wolfspeed SiC MOSFET LTspice Model Quick Start Guide Rev 2.0, 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 LTspice library directory.
Typical installation path is given by (C:\Program Files (x86)\LTC\LTspiceIV\lib\).

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

Optimized for 25°C & 150°C temperature 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.
Valid for temperature range -55°C to 150°C
Optimized and verified for 25°C & 150°C temperature 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)
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 is not modeled .

Simulation Guidelines:

The SiC LTspice 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 can be used for different MOSFET models if the pin count is the same. For
example nmos TO247_4L.asy can be used for MOSFET model C3M0065100K, C3M0120100K or any
Wolfspeed SiC MOSFET LTspice Model Quick Start Guide Rev 2.0, 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 nmos7.asy for MOSFET model C3M0065100J,
C3M0120090J or any MOSFETs with 7 leads. To achieve that, move the mouse pointer to the
symbol and right click. Then component attribute editor will appear, enter the MOSFET model
number at the attribute “Value” like figure 2.

Figure 2: Component Attribute Editor

Users are required to manually include the library path at each circuit design. This is to provide
LTspice the path where the library is located.
Example:
.lib "C:\Program Files (x86)\LTC\LTspiceIV\lib\C3M0120100K.lib"
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.
Wolfspeed SiC MOSFET LTspice Model Quick Start Guide Rev 2.0, 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.

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 to 25°C
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.
Wolfspeed SiC MOSFET LTspice Model Quick Start Guide Rev 2.0, 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.

In order 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 150°C for DC simulation.

Migrating Wolfspeed LTspice model to others SPICE softwares

Wolfspeed MOSFET SPICE models are both LTspice and OrCad Pspice compatible. To use
Wolfspeed MOSFET SPICE model on other SPICE softwares, user may need to do few more steps
to get it work. Some SPICE software use different extension like SIMetrix uses library with extension
.lb whereas Ltspice and Pspice 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 user to verify the model against datasheet after changing the format of
the model.

6. Simulation Examples
6.1 Simulation Example1:
The schematic in Figure 5 shows the LTspice 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. LTspice model of the Boost converter

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

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

Figure 7. SiC MOSFET Turn-ON Event

Figure 8. SiC MOSFET Turn-OFF Event
Wolfspeed SiC MOSFET LTspice Model Quick Start Guide Rev 2.0, 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.

6.2 Simulation Example 2:
Example 2 shown in figure 9 is a 3 phase 2 level inverter with output filter. The purpose of this
example is to show the connection of Kelvin source of TO263-7, and gate drive.

Figure 9. 3phase 2Level Inverter with output filter

Output inverter phase a voltage (Blue) and current (Green) waveforms are shown in figure 10.

Figure 10. Waveform captured from LTspice Simulation of 3phase inverter

Revision History

Date
12/21/2017
02/21/2018

Revision
V1.0
V2.0

Changes
Initial release
SPICE model is both LTspice and
Pspice compactible

Source Exif Data:

File Type                       : PDF
File Type Extension             : pdf
MIME Type                       : application/pdf
PDF Version                     : 1.7
Linearized                      : No
Warning                         : Info object (166 0 obj) not found at 1765882

EXIF Metadata provided by EXIF.tools

Wolfspeed SiC Mosfet LTspice Quick Start Guide Rev 2.0 Feb 2018x Si C 2018

Navigation menu

Versions of this User Manual:

Views

Navigation