AND9002/D
Use of NCP5217A Pspice
Model
Prepared by: Gang Chen
ON Semiconductor
http://onsemi.com
APPLICATION NOTE
Overview
and loop stability. Figure 2 shows a typical simulation
circuit with the NCP5217A Pspice model. An inherent input
voltage feed−forward function of the NCP5217A makes
transient response and stability almost independent to input
voltage variation, so that users do not need to provide input
voltage information in simulation. Also the behavior of the
external MOSFETs has been embedded into the NCP5217A
Pspice model to simplify the simulation system since the
MOSFETs have little effect on either transient response or
stability. This simulation note is to illustrate a simulation
procedure with the NCP5217A Pspice model.
The NCP5217A is a synchronous step−down controller
for high performance battery−powered systems likes
notebook applications. The IC is packaged in QFN14.
Figure 1 shows a typical application circuit. The range of the
input voltage VIN is from 4.5 V to 27 V. The range of the
output voltage VOUT is from 0.8 V to 3.3 V. The internal
reference voltage (FB voltage) is 0.8 V.
To provide very fast simulation results and an initial
design of system parameters before a real board design in
applications, a NCP5217A averaged behavior model in
Pspice has been developed to simulate transient response
Figure 1. Typical Application Circuit
U1
SWN
NCP5217A
CS+
SWN
1
L
1uH
Rcs
4K
1
CS+
2
CS−
2
DCR
3.3m
ESR
6m
I1
Co
440uF
0mVac
0Vdc
I1 = 0
I2 = 10A
TD = 220u
TR = 1u
TF = 1u
PW = 50u
PER = 1
V1
0
0
5
4
Vout
Ccs
100nF
FB
COMP
CS−
3
C1
COMP
C2
180pF
6p
R1
10K
FB
R2
180K
R3
1K
Vout_FB
C3
180pF
R4
11.429K
0
Figure 2. Typical Simulation Circuit
© Semiconductor Components Industries, LLC, 2011
April, 2011 − Rev. 0
1
Publication Order Number:
AND9002/D
AND9002/D
DETAILED DESCRIPTION
Download Pspice Model
Users can download the NCP5217A Pspice model from ON Semiconductor website, which is a zipped file
“NCP5217_PSPICE.ZIP” including one Pspice model lib file “NCP5217_PSPICE.LIB”, one schematic symbol olb file
“NCP5217_PSPICE.OLB”, and one design dsn file “NCP5217A.DSN”. Save all the extracted files in a folder.
Model Installation
1. Create New Project
Users need to run ORCAD Capture or Allegro Design Entry CIS first, and then create a new blank project in Capture as shown
in Figure 3.
Figure 3. Create New Blank Simulation Project
2. Import Design File
Add the design file “NCP5217A.DSN” into the Design Resources to replace the blank design.
Figure 4. Import Design File into Design Resources
http://onsemi.com
2
AND9002/D
3. Import Symbol File
Add the symbol file “NCP5217_PSPICE.OLB” into the Design Resources as shown in Figure 5.
Figure 5. Import Symbol File into Design Resources
4. Open Schematic
Open the schematic “Page 1” in the “Schematic1” under the design file as shown in Figure 6. Users can edit the schematic
according to real applications.
Figure 6. Open Schematic in Design File
http://onsemi.com
3
AND9002/D
5. Create Simulation Profile and Run Simulation
In order to run simulations, a new simulation profile has to be created. In the simulation setting of the simulation profile,
users need to use browser to add the Pspice lib file “NCP5217_PSPICE.LIB” into the design library of the simulation
configuration files, as shown in Figure 8. The Pspice model of the NCP5217A is able to support both time domain transient
simulation and AC frequency domain simulation. Users can set both configurations in the simulation profile.
Figure 7. Create a New Simulation Profile
Figure 8. Add Pspice Lib File into the library of the Configuration Files
Time Domain Transient Simulation
U1
SWN
NCP5217A
CS+
SWN
1
L
1uH
Rcs
4K
1
CS+
2
CS−
2
DCR
3.3m
ESR
6m
I1
Co
440uF
0mVac
0Vdc
V1
0
0
5
4
Vout
Ccs
100nF
FB
COMP
CS−
3
C1
COMP
C2
180pF
6p
R1
10K
FB
R2
180K
R3
1K
Vout_FB
C3
180pF
R4
11.429K
0
Figure 9. Typical Schematic for Time Domain Transient Simulation
http://onsemi.com
4
I1 = 0
I2 = 10A
TD = 220u
TR = 1u
TF = 1u
PW = 50u
PER = 1
AND9002/D
Figure 9 shows a typical schematic for a time domain transient simulation. An AC source V1 is set to 0 V as its AC and DC
components. Users can edit parameters of the pulse current source I1 to simulate load transient in the output VOUT. In order
to reduce simulation time, a 100 ms (instead of 1.1 ms in the NCP5217A datasheet) internal soft start has been implemented
in the model. A typical time-domain simulation profile setting is shown in Figure 10. Users can review simulation waveforms
in Pspice A/D after running a simulation. Figure 11 shows an example of the simulation results regarding to a load transient
event.
Figure 10. Simulation Setting for Time Domain Simulation
Figure 11. Typical Simulation Results of Time Domain Simulation
http://onsemi.com
5
AND9002/D
Due to a benefit from the averaged behavior model, the total simulation time is just a few seconds and thus it is good for users
to optimize the system by running a parameter sweep simulation. Before running a parameter sweep simulation, at least one
“PARAM” part from the “SPECIAL.OLB” needs to be added in the schematic. Figure 12 shows an example schematic that
is able to be used to run parameter sweep for the capacitor C3 in the compensation network. Users can program a pattern of
the parameter sweep in the simulation profile as shown in Figure 13.
U1
SWN
NCP5217A
CS+
SWN
1
L
1uH
Rcs
4K
1
CS+
2
CS−
2
DCR
3.3m
ESR
6m
I1
Co
440uF
0mVac
0Vdc
I1 = 0
I2 = 10A
TD = 220u
TR = 1u
TF = 1u
PW = 50u
PER = 1
V1
0
0
5
4
Vout
Ccs
100nF
FB
COMP
CS−
3
C1
COMP
6p
R1
10K
FB
Vout_FB
PARAMETERS:
C2
180pF
R2
180K
R3
1K
C3
{C3}
C3 = 180pF
R4
11.429K
0
Figure 12. Typical Schematic for Parametric Sweep in Time Domain Transient Simulation
Figure 13. Simulation Setting for Parametric Sweep in Time Domain Simulation
http://onsemi.com
6
AND9002/D
Figure 14 shows multiple simulation results after the parameter sweep simulation. It is very easy for users to see the
parameter impact on the transient response.
C3=100pF
C3=180pF
C3=360pF
C3=100pF
C3=180pF
C3=360pF
Figure 14. Typical Simulation Results of Parametric Sweep in Time Domain Simulation
http://onsemi.com
7
AND9002/D
AC Frequency Domain Simulation
With the NCP5217A Pspice model, users are able to use almost the same schematic to do AC frequency domain simulation
as what is used in the time domain simulation. The main difference is in the setting of the AC voltage source V1 shown in
Figure 15. In the frequency domain simulation, usually a small AC voltage such as 10 mV ~ 100 mV is used.
U1
SWN
NCP5217A
CS+
SWN
1
L
1uH
Rcs
4K
1
CS+
2
CS−
2
DCR
3.3m
ESR
6m
I1
Co
440uF
10mVac
0Vdc
I1 = 0
I2 = 10A
TD = 220u
TR = 1u
TF = 1u
PW = 50u
PER = 1
V1
0
0
5
4
Vout
Ccs
100nF
FB
COMP
CS−
3
C1
COMP
C2
180pF
6p
R1
10K
FB
R2
180K
R3
1K
Vout_FB
C3
180pF
R4
11.429K
0
Figure 15. Typical Schematic for AC Frequency Domain Simulation
Figure 16 shows a simulation setting for an AC frequency domain simulation and Figure 17 shows typical simulation results.
Users can read close-loop bandwidth and phase margin from the bode plot.
Figure 16. Simulation Setting for AC Frequency Domain Simulation
http://onsemi.com
8
AND9002/D
Figure 17. Typical Simulation Results of AC Frequency Domain Simulation
http://onsemi.com
9
AND9002/D
Users also can run parametric sweep in an AC frequency domain simulation. Figure 18 is an example schematic which is
very similar to the schematic shown in Figure 12 but with a 10mV AC component in the AC voltage source V1. Figure 19 shows
a corresponding simulation setting, and Figure 20 shows typical simulation results. Users can see the parameter impact on the
close-loop stability.
U1
SWN
NCP5217A
CS+
SWN
1
L
1uH
Rcs
4K
1
CS+
2
CS−
2
DCR
3.3m
ESR
6m
I1
Co
440uF
10mVac
0Vdc
I1 = 0
I2 = 10A
TD = 220u
TR = 1u
TF = 1u
PW = 50u
PER = 1
V1
0
0
5
4
Vout
Ccs
100nF
FB
COMP
CS−
3
C1
COMP
C2
180pF
6p
R1
10K
FB
R2
180K
R3
1K
Vout_FB
C3
{C3}
PARAMETERS:
C3 = 180pF
R4
11.429K
0
Figure 18. Typical Schematic for Parametric Sweep in AC Frequency Domain Simulation
Figure 19. Simulation Setting for Parametric Sweep in AC Frequency Domain Simulation
http://onsemi.com
10
AND9002/D
C3=360pF
C3=180pF
C3=100pF
C3=360pF
C3=180pF
C3=100pF
Figure 20. Typical Simulation Results of Parametric Sweep in AC Frequency Domain Simulation
ON Semiconductor and
are registered trademarks of Semiconductor Components Industries, LLC (SCILLC). SCILLC reserves the right to make changes without further notice
to any products herein. SCILLC makes no warranty, representation or guarantee regarding the suitability of its products for any particular purpose, nor does SCILLC assume any liability
arising out of the application or use of any product or circuit, and specifically disclaims any and all liability, including without limitation special, consequential or incidental damages.
“Typical” parameters which may be provided in SCILLC data sheets and/or specifications can and do vary in different applications and actual performance may vary over time. All
operating parameters, including “Typicals” must be validated for each customer application by customer’s technical experts. SCILLC does not convey any license under its patent rights
nor the rights of others. SCILLC products are not designed, intended, or authorized for use as components in systems intended for surgical implant into the body, or other applications
intended to support or sustain life, or for any other application in which the failure of the SCILLC product could create a situation where personal injury or death may occur. Should
Buyer purchase or use SCILLC products for any such unintended or unauthorized application, Buyer shall indemnify and hold SCILLC and its officers, employees, subsidiaries, affiliates,
and distributors harmless against all claims, costs, damages, and expenses, and reasonable attorney fees arising out of, directly or indirectly, any claim of personal injury or death
associated with such unintended or unauthorized use, even if such claim alleges that SCILLC was negligent regarding the design or manufacture of the part. SCILLC is an Equal
Opportunity/Affirmative Action Employer. This literature is subject to all applicable copyright laws and is not for resale in any manner.
PUBLICATION ORDERING INFORMATION
LITERATURE FULFILLMENT:
Literature Distribution Center for ON Semiconductor
P.O. Box 5163, Denver, Colorado 80217 USA
Phone: 303−675−2175 or 800−344−3860 Toll Free USA/Canada
Fax: 303−675−2176 or 800−344−3867 Toll Free USA/Canada
Email: [email protected]
N. American Technical Support: 800−282−9855 Toll Free
USA/Canada
Europe, Middle East and Africa Technical Support:
Phone: 421 33 790 2910
Japan Customer Focus Center
Phone: 81−3−5773−3850
http://onsemi.com
11
ON Semiconductor Website: www.onsemi.com
Order Literature: http://www.onsemi.com/orderlit
For additional information, please contact your local
Sales Representative
AND9002/D