1. Home
  2. Electronics Computer-Aided Design
  3. Pspice Mosfet Headaches

Pspice Mosfet Headaches

I've been trying to use Fairchild's RFP30N06LE (logic level n-channel Mosfet) Pspice model.

The datasheet with the model is here:

formatting link

The model fails to converge in a simple switching a resistive load test cct, let alone the cct I want to use it in. I have tried all typical approaches to resolve this such as relaxing the tolerances, GMIN stepping, increasing ITL4 and skipping DC bias point. I've also tried other mosfet models based on this same subcircuit and none of them converge like the RF1S23N06LE and RF1S30N06LE. Placing the FDN359AN in the exact same cct the cct converges, so I know there is nothing wrong with the test cct.

I'm hoping someone knowledgeable in FET modeling could take a look at the model and provide some insight. The model text is below as well.

Thank you.

PSPICE Electrical Model

SUBCKT RFP30N06LE 2 1 3; rev 6/2/93

CA 12 8 1 3.34e-9 CB 15 14 3.44e-9 CIN 6 8 0 1.343e-9

DBODY 7 5 DBDMOD DBREAK 5 11 DBKMOD DESD1 91 9 DESD1MOD DESD2 91 7 DESD2MOD DPLCAP 10 5 DPLCAPMOD

EBREAK 11 7 17 18 75.39 EDS 14 8 5 8 1 EGS 13 8 6 8 1 ESG 6 10 6 8 1 EVTO 20 6 18 8 1

IT 8 17 1

LDRAIN 2 5 1e-9 LGATE 1 9 7.22e-9 LSOURCE 3 7 6.31e-9

MOS1 16 6 8 8 MOSMOD M = 0.99 MOS2 16 21 8 8 MOSMOD M = 0.01

RBREAK 17 18 RBKMOD 1 RDRAIN 50 16 RDSMOD 11.86e-3 RGATE 9 20 2.52 RIN 6 8 1e9 RSCL1 5 51 RSLVCMOD 1e-6 RSCL2 5 50 1e3 RSOURCE 8 7 RDSMOD 26.6e-3 RVTO 18 19 RVTOMOD 1

S1A 6 12 13 8 S1AMOD S1B 13 12 13 8 S1BMOD S2A 6 15 14 13 S2AMOD S2B 13 15 14 13 S2BMOD

VBAT 8 19 DC 1 VTO 21 6 0.5

ESCL 51 50 VALUE = {(V(5,51)/ABS(V(5,51)))*(PWR(V(5,51)*1e6/89,7))

.MODEL DBDMOD D (IS = 3.80e-13 RS = 1.12e-2 TRS1 = 1.61e-3 TRS2 =

6.08e-6 CJO = 1.05e-9 TT = 3.84e-8) .MODEL DBKMOD D (RS = 1.82e-1 TRS1 = 7.50e-3 TRS2 = -4.0e-5) .MODEL DESD1MOD D (BV = 13.54 TBV1 = 0 TBV2 = 0 RS = 45.5 TRS1 = 0 TRS2 = 0) .MODEL DESD2MOD D (BV = 11.46 TBV1 = -7.576e-4 TBV2 = -3.0e-6 RS = 0 TRS1 = 0 TRS2 = 0) .MODEL DPLCAPMOD D (CJO = 0.591e-9 IS = 1e-30 N = 10) .MODEL MOSMOD NMOS (VTO = 1.94 KP = 139.2 IS = 1e-30 N = 10 TOX = 1 L = 1u W = 1u) .MODEL RBKMOD RES (TC1 = 1.07e-3 TC2 = -3.03e-7) .MODEL RDSMOD RES (TC1 = 5.38e-3 TC2 = 1.64e-5) .MODEL RSLVCMOD RES (TC1 = 1.75e-3 TC2 = 3.90e-6) .MODEL RVTOMOD RES (TC1 = -2.15e-3 TC2 = -5.43e-6) .MODEL S1AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -4.05 VOFF = -1.5) .MODEL S1BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -1.5 VOFF = -4.05) .MODEL S2AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -2.2 VOFF = 2.8) .MODEL S2BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = 2.8 VOFF = -2.2) .ENDS
Reply to
Hammy
Loading thread data ...

[snip]

...Jim Thompson

--
|  James E.Thompson, P.E.                           |    mens     |
|  Analog Innovations, Inc.                         |     et      |
|  Analog/Mixed-Signal ASIC\'s and Discrete Systems  |    manus    |
|  Phoenix, Arizona            Voice:(480)460-2350  |             |
|  E-mail Address at Website     Fax:(480)460-2142  |  Brass Rat  |
|       http://www.analog-innovations.com           |    1962     |
             
         America: Land of the Free, Because of the Brave
Reply to
Jim Thompson

Hi Jim:

Thanks for your response. Regarding your question I don't see any VCS's in the FDN359AN. This is a more recent model made in 2002 according to the text. This is the FDN359AN

.SUBCKT FDN359AN 20 10 30 50

*20=DRAIN 10=GATE 30=SOURCE 50=VTEMP Rg 10 11x 1 Rdu 12x 1 1u M1 2 1 4x 4x DMOS L=1u W=1u .MODEL DMOS NMOS(VTO=1.9 KP=2.25E+1 +THETA=.1 VMAX=0.8E5 LEVEL=3) Cgs 1 5x 420p Rd 20 4 1.5E-2 Dds 5x 4 DDS .MODEL DDS D(M=3.55E-1 VJ=6.33E-1 CJO=226p) Dbody 5x 20 DBODY .MODEL DBODY D(IS=4.96E-12 N=1.127089 RS=.001349 TT=12.63n) Ra 4 2 1.5E-2 Rs 5x 5 0.5m Ls 5 30 0.5n M2 1 8 6 6 INTER E2 8 6 4 1 2 .MODEL INTER NMOS(VTO=0 KP=10 LEVEL=1) Cgdmax 7 4 260p Rcgd 7 4 10meg Dgd 6 4 DGD Rdgd 6 4 10meg .MODEL DGD D(M=7.3E-2 VJ=3.11E-1 CJO=260p) M3 7 9 1 1 INTER E3 9 1 4 1 -2 *ZX SECTION EOUT 4x 6x poly(2) (1x,0) (3x,0) 0 0 0 0 1 FCOPY 0 3x VSENSE 1 RIN 1x 0 1G VSENSE 6x 5x 0 RREF 3x 0 10m *TEMP SECTION ED 101 0 VALUE {V(50,100)} VAMB 100 0 25 EKP 1x 0 101 0 .0195 *VTO TEMP SECTION EVTO 102 0 101 0 .002 EVT 12x 11x 102 0 1 *DIODE THEMO BREAKDOWN SECTION EBL VB1 VB2 101 0 .08 VBLK VB2 0 30 D 20 DB1 DBLK .MODEL DBLK D(IS=1E-14 CJO=.1p RS=.1) EDB DB1 0 VB1 0 1 .ENDS FDN359AN *FDN359AN (Rev.A1) 5/15/02 **ST

This was my original choice for what I'm building, and then I got 20 RFP30N06LE for a good price (free) .The RFP30N06LE is overkill for what I'm doing but easier to work with in a T0-220 packages, versus the microscopic SOT-23 of the FDN359AN.

I'm sure I can find other uses for RFP30N06LE which is why I'm interested in the model.

Reply to
Hammy

"Hammy" schrieb im Newsbeitrag news: snipped-for-privacy@4ax.com...

Hello Hammy,

I have tried to run the subcircuit and got error messages.

How have you solved the the two erros in the subcircuit regarding the three pins of the capacitors?

CA 12 8 3.34e-9

CIN 6 8 1.343e-9

One more change.

.SUBCKT RFP30N06LE 2 1 3

I have tested the "repaired" model with LTspice and PSPICE demo 10.5. My test circuit has worked in both simulators.

Where is your netlist?

---------------------

Best regards, Helmut

Reply to
Helmut Sennewald

Hi Helmut:

Thanks for your assistance. I did the corrections you suggested (I'm using OrCAD demo 10.5 to), but I still get convergence problems. I also get several errors in my output file.

This is my test circuit netlist.

  • source FRFTR R_R8 N81164 N81004 2 V_V4 N81004 0 44 X_U1 N81164 N80914 0 RFP30N06LE/HA R_R12 0 N80914 22k V_V5 N81706 0
+PULSE 0 5 0 20n 20n 3.82u 26u R_R14 N81706 N80914 22

This is my output file section with errors.

ERROR -- End of expression not seen .MODEL DBKMOD D (RS = 1.82e-1 TRS1 = 7.50e-3 TRS2 = -4.0e-5)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL DBKMOD D (RS = 1.82e-1 TRS1 = 7.50e-3 TRS2 = -4.0e-5)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL DESD1MOD D (BV = 13.54 TBV1 = 0 TBV2 = 0 RS = 45.5 TRS1 = 0 TRS2 = 0)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL DESD2MOD D (BV = 11.46 TBV1 = -7.576e-4 TBV2 = -3.0e-6 RS = 0 TRS1 = 0 TRS2 = 0)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL DPLCAPMOD D (CJO = 0.591e-9 IS = 1e-30 N = 10)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL MOSMOD NMOS (VTO = 1.94 KP = 139.2 IS = 1e-30 N = 10 TOX = 1 L=

1u W = 1u)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL RBKMOD RES (TC1 = 1.07e-3 TC2 = -3.03e-7)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL RDSMOD RES (TC1 = 5.38e-3 TC2 = 1.64e-5)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL RSLVCMOD RES (TC1 = 1.75e-3 TC2 = 3.90e-6)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL RVTOMOD RES (TC1 = -2.15e-3 TC2 = -5.43e-6)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL S1AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -4.05 VOFF = -1.5)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL S1BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -1.5 VOFF = -4.05)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL S2AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -2.2 VOFF = 2.8)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .MODEL S2BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = 2.8 VOFF = -2.2)

-----------------------------------------------------------------------------------------------------$ ERROR -- End of expression not seen .ENDS

Reply to
Hammy

Hi Helmut:

A correction to my netlist, for this line:

X_U1 N81164 N80914 0 RFP30N06LE/HA

Should be just:

X_U1 N81164 N80914 0 RFP30N06LE

Thanks for any assistance.

Reply to
Hammy

"Hammy" schrieb im Newsbeitrag news: snipped-for-privacy@4ax.com...

Hello Hammy,

And here is the working example. You have overlooked the broken lines. The SPICE syntax requires a "+" character in the first column for multiline SPICE-lines.

May I mention that I got with two mouse clicks the average power dissipation of the MOSFET with LTspice. It's 4.86Watt in your example. . Best regards, Helmut

Netlist "RFP30N06E_test2.cir"

  • RFP30N06LE_test2.asc XM1 DRAIN GATE 0 RFP30N06LE V1 VG 0 PULSE 0 5 0 20n 20n 3.82u 26u V2 V44 0 44 RL V44 DRAIN 2 RG GATE 0 22k RS VG GATE 22 .include RFP30N06LE.lib
  • .dc V1 0 4 10m .tran 0 100u 0 1u .probe .end

Library file "RFP30N06LE.lib" Hopefully the lines are short enough for your news reader.

  • Fairchild
  • PSPICE Electrical Model
*; rev 6/2/93
  • PSPICE Electrical Model
.SUBCKT RFP30N06LE 2 1 3 *CA 12 8 1 3.34e-9 CA 12 8 3.34e-9 CB 15 14 3.44e-9 *CIN 6 8 0 1.343e-9 CIN 6 8 1.343e-9 DBODY 7 5 DBDMOD DBREAK 5 11 DBKMOD DESD1 91 9 DESD1MOD DESD2 91 7 DESD2MOD DPLCAP 10 5 DPLCAPMOD EBREAK 11 7 17 18 75.39 EDS 14 8 5 8 1 EGS 13 8 6 8 1 ESG 6 10 6 8 1 EVTO 20 6 18 8 1 IT 8 17 1 LDRAIN 2 5 1e-9 LGATE 1 9 7.22e-9 LSOURCE 3 7 6.31e-9 MOS1 16 6 8 8 MOSMOD M = 0.99 MOS2 16 21 8 8 MOSMOD M = 0.01 RBREAK 17 18 RBKMOD 1 RDRAIN 50 16 RDSMOD 11.86e-3 RGATE 9 20 2.52 RIN 6 8 1e9 RSCL1 5 51 RSLVCMOD 1e-6 RSCL2 5 50 1e3 RSOURCE 8 7 RDSMOD 26.6e-3 RVTO 18 19 RVTOMOD 1 S1A 6 12 13 8 S1AMOD S1B 13 12 13 8 S1BMOD S2A 6 15 14 13 S2AMOD S2B 13 15 14 13 S2BMOD VBAT 8 19 DC 1 VTO 21 6 0.5 ESCL 51 50 VALUE = {(V(5,51)/ABS(V(5,51)))*(PWR(V(5,51)*1e6/89,7))} .MODEL DBDMOD D (IS = 3.80e-13 RS = 1.12e-2 TRS1 = 1.61e-3
  • TRS2 = 6.08e-6 CJO = 1.05e-9 TT = 3.84e-8) .MODEL DBKMOD D (RS = 1.82e-1 TRS1 = 7.50e-3 TRS2 = -4.0e-5) .MODEL DESD1MOD D (BV = 13.54 TBV1 = 0 TBV2 = 0 RS = 45.5
  • TRS1 = 0 TRS2 = 0) .MODEL DESD2MOD D (BV = 11.46 TBV1 = -7.576e-4
  • TBV2 = -3.0e-6 RS = 0 TRS1 = 0 TRS2 = 0) .MODEL DPLCAPMOD D (CJO = 0.591e-9 IS = 1e-30 N = 10) .MODEL MOSMOD NMOS (VTO = 1.94 KP = 139.2 IS = 1e-30
  • N = 10 TOX = 1 L = 1u W = 1u) .MODEL RBKMOD RES (TC1 = 1.07e-3 TC2 = -3.03e-7) .MODEL RDSMOD RES (TC1 = 5.38e-3 TC2 = 1.64e-5) .MODEL RSLVCMOD RES (TC1 = 1.75e-3 TC2 = 3.90e-6) .MODEL RVTOMOD RES (TC1 = -2.15e-3 TC2 = -5.43e-6) .MODEL S1AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -4.05 VOFF = -1.5) .MODEL S1BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -1.5 VOFF = -4.05) .MODEL S2AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -2.2 VOFF = 2.8) .MODEL S2BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = 2.8 VOFF = -2.2) .ENDS
  • NOTE: For further discussion of the PSPICE model,
  • consult A New PSPICE Sub-Circuit for the Power MOSFET
  • Featuring Global Temperature Options;
  • IEEE Power Electronics Specialist Conference Records 1991.
Reply to
Helmut Sennewald

Hi Helmut:

Thank you for your patience. The problem still persists.

I tried to run your netlist and got the following error:

ERROR -- Less than 2 connections at node DRAIN

I then copied your model text with the corrections over the existing model txt. This took care of all the syntax errors (or at least Pspice isn't reporting them).The output file is below. The same test cct I posted earlier.

ERROR -- Convergence problem in transient analysis at Time = 185.5E-09 Time step = 2.028E-15, minimum allowable step size =

4.000E-15

These voltages failed to converge:

V(X_U1.12) = 3.091V \\ 3.189V V(X_U1.8) = 606.39mV \\ 705.10mV V(X_U1.15) = 3.090V \\ 3.189V V(X_U1.14) = 1.744V \\ 1.843V V(X_U1.6) = 3.091V \\ 3.189V V(X_U1.7) = 42.26mV \\ 140.97mV V(X_U1.5) = 1.744V \\ 1.843V V(X_U1.11) = 75.43V \\ 75.53V V(X_U1.91) = 189.52mV \\ 288.23mV V(X_U1.9) = 3.286V \\ 3.384V V(X_U1.10) = 606.39mV \\ 705.10mV V(X_U1.17) = 1.606V \\ 1.705V V(X_U1.18) = 606.39mV \\ 705.10mV V(X_U1.13) = 3.091V \\ 3.189V V(X_U1.20) = 3.090V \\ 3.189V V(X_U1.16) = 1.495V \\ 1.594V V(X_U1.21) = 3.591V \\ 3.689V V(X_U1.50) = 1.746V \\ 1.844V V(X_U1.51) = 1.744V \\ 1.843V V(X_U1.19) = -393.61mV \\ -294.90mV

These devices failed to converge: X_U1.ESCL

ERROR -- Discontinuing simulation due to convergence problem

Last node voltages tried were:

NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE

(N80914) 3.2938 (N81004) 44.0000 (N81706) 5.0000 (X_U1.5)

1.7439

(X_U1.6) 3.0905 (X_U1.7) .0423 (X_U1.8) .6064 (X_U1.9)

3.2855

(N810301) 1.7616 (X_U1.10) .6064 (X_U1.11) 75.4320 (X_U1.12) 3.0905 (X_U1.13) 3.0905 (X_U1.14) 1.7439 (X_U1.15) 3.0904 (X_U1.16) 1.4948 (X_U1.17) 1.6064 (X_U1.18) .6064 (X_U1.19) -.3936 (X_U1.20) 3.0904 (X_U1.21) 3.5905 (X_U1.50) 1.7455 (X_U1.51) 1.7439 (X_U1.91) .1895

**** Interrupt ****

As you may have guessed I'm not exactly an expert on spice.

Could this be the problem "X_U1.ESCL" What exactly does ESCL stand for on the model schematic the symbol looks like a DC source?

I like LTSpice too but it doesn't have a layout tool.

Reply to
Hammy

Hello Hammy,

I have sent my files to your email address. Please try it.

Just open the .cir file with PSPICE-AD and press RUN(->).

Have you changed the default convergence settings?

I recommend you send me your files for a check. You can tell me a lot about your netlist and library file, but I only believe that when I can verify this with your files.

Best regards, Helmut

If you don't simulate the whole board, you have to change the schematic anyway for PSPICE. So it's not so far from drawing it again in another tool.

Reply to
Helmut Sennewald

Hi Helmut:

Thanks much for your help it's working!!

I set all simulation settings to there default,and it worked.

You will probably get your email back the email addy with my name is bogus. Sorry but I'm new to newsgroup posting,and didnt want to get more "spam". My email address is snipped-for-privacy@hotmail.com .

Again thanks alot you saved me a lot of time,hopefully I can return the favour in the future.

Reply to
Hammy

May I mention that with no mouse clicks I get the average power of any device in SuperSpice:-)

--
Kevin Aylward
kaEXTRACT@anasoft.co.uk
www.anasoft.co.uk
Reply to
Kevin Aylward

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.