I need Pspice model for UC1844A & TLV3011? Please can you support.
This thread has been locked.
If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.
Hi,
We do not provide the model for UCC1844A/2844A/3844A on website.
I just googled and found maybe this page can help you.
http://cbasso.pagesperso-orange.fr/Spice.htm
Regards
Hi.
Thank you for the prompt reply.
Can you suggest the nearest part for which Spice model would be available ?
-Bala
Hi Bala,
What software are you using?
I found UC3844's model in simetrix which is also a spice model.
The code are:
.subckt UC3844-%REF% Vout Osc Vp Comp Sense Vfb Ref Gnd
A$U2 [U6_OUT U5_IN4] U2_OUT nand
A$U3 [U2_OUT U7_OUT] U5_IN4 nand
X$ARB1 R1_P Sense ARB1_OUT $$arbsourceARB1 pinnames: N1 N2 OUT
.subckt $$arbsourceARB1 N1 N2 OUT
B1 OUT 0 V=tanh(v(n1,n2)*1000)*2.5+2.5
.ends
A$U16 U12_OUT U16_OUT DA
X$U1 Vfb Ref Vp Comp Gnd R5_N $$error_amp_2 pinnames: VINN BIAS VP VOUT VN VINP
A$U17 U9_OUT U17_OUT DA
A$U6 U12_OUT U6_OUT inv
V1 S2_P 0 5V
A$U7 U15_OUT U7_OUT delay1
A$U15 ARB1_OUT U15_OUT AD
A$U4 Vp U4_OUT schmitt
A$U5 [U10_OUT U12_OUT U8_QP U5_IN4] U11_IN1 or
A$U12 Osc U12_OUT schmitt_osc
I2 R1_N Comp 10u
A$U13 U11_OUT U13_OUT DA
A$U10 U4_OUT U10_OUT inv
A$U11 U11_IN1 U11_OUT inv_dead
I1 Gnd I1_N 40m
A$U18 U4_OUT U18_OUT DA
A$VCC2 VCC2_P DIG_VCC
D1 Comp D1_N Diode
D2 D1_N R1_N Diode
D3 R1_P I1_N Diode
Q2 Vp S1_N Vout 0 N1 20
R4 S1_N Gnd 1K
R5 Ref R5_N 10k
X$S4 Osc 0 U16_OUT 0 gen_switch : RON=250 ROFF=100Meg VON=3 VOFF=2 pinnames: P N CP CN
A$U8 VCC2_P U12_OUT U8_SET U8_SET U8_QP U8_QN Toggle
A$GND2 U8_SET DIG_GND
R6 R5_N Gnd 10k
A$U9 U11_IN1 U9_OUT dead
Q1 Vout U17_OUT Gnd 0 N1 20
X$S2 S2_P Ref U18_OUT 0 gen_switch : RON=1 ROFF=100Meg VON=3 VOFF=2 pinnames: P N CP CN
R1 R1_P R1_N 20k
X$S3 Vp 0 U18_OUT 0 gen_switch : RON=1.36k ROFF=30k VON=3 VOFF=2 pinnames: P N CP CN
R2 Gnd R1_P 10k
.ic Osc 0
R3 I1_N Gnd 10
X$S1 Vp S1_N U13_OUT Gnd gen_switch : RON=1 ROFF=1Meg VON=3 VOFF=2 pinnames: P N CP CN
.model inv d_inverter
.model or d_or
.model DIG_GND d_pulldown strong=true out_family="FORCE5"
.model DIG_VCC d_pullup strong=true out_family="FORCE5"
.model toggle d_tff
.model delay1 d_buffer rise_delay=150n fall_delay=150n
.model dead d_buffer rise_delay=20n fall_delay=1n
.model inv_dead d_inverter rise_delay=20n fall_delay=1n
.model nand d_nand
.model and d_and
.model Diode D(IS=1.6f CJO=0.3p M=0.3 VJ=0.75 ISR=2.6n)
.model N1 NPN BF=300 TF=0.5n CJC=0.3p VAF=100
.model P1 PNP BF=150 TF=2n CJC=0.3p VAF=150
.model D1 D
.model schmitt_osc adc_schmitt in_low=1 in_high=3
* 842/4
.model schmitt adc_schmitt in_low=10 in_high=16
* 843/5
*.model schmitt adc_schmitt in_low=7.6 in_high=8.4
.subckt gen_switch 1 2 3 4
S1 1 2 3 4 SW
.model SW VSWITCH RON={ron} ROFF={roff} VON={von} VOFF={voff}
.ends
.model AD adc_bridge in_low=2.1 in_high=2.2 rise_delay=1e-12 fall_delay=1e-12 out_family = "UNIV" out_low = 0 out_high = 5 clamp_bias=0.5 clamp_res=10
.model DA dac_bridge out_high=5 input_load=-31p t_rise=2n t_fall=2n g_pullup=0.024 g_pulldown=0.034 g_hiz=1e-9 knee_low = 2.0 knee_high =2.75 v_smooth = 0.5 in_family="UNIV"
.subckt $$error_amp_2 VINN BIAS VP VOUT VN VINP
Q8 Q6_C Q6_C VN 0 N1
Q9 Q10_B Q6_C VN 0 N1
V1 D2_N VN 5.5
Q10 VOUT Q10_B Q10_E 0 N1
C1 C1_P Q10_B 270p
D1 Q10_E VN D1
D2 VOUT D2_N D1
E1 C1_P 0 VOUT 0 1
G2 VP G2_N BIAS VN 20u
Q6 Q6_C R2_P G2_N 0 P1
Q7 Q10_B R3_P G2_N 0 P1
R2 R2_P VINN 2.7k
X$S1 VP VOUT BIAS 0 gen_switch : RON=30k ROFF=1G VON=3 VOFF=2 pinnames: P N CP CN
R3 R3_P VINP 2.7k
.subckt gen_switch 1 2 3 4
S1 1 2 3 4 SW
.model SW VSWITCH RON={ron} ROFF={roff} VON={von} VOFF={voff}
.ends
.model N1 NPN BF=200 TF=0.15n CJC=0.3p VAF=100
.model P1 PNP BF=150 TF=5n CJC=30p VAF=150 RB=100
.model D1 D
.ends
.ends
Hi.
I am using Cadence Pspice for Simulation. I think this model would help. This looks a bit helpful. I can create PSpice model from this. Let me see what I can do at.
Thank you for the data.
-bala