Bad voltage output using the TI supplied TPS2557 TINA-TI to PSpice Conversion in LTSpice

Question

I pulled the converted PSpice file for the TI TPS2557 Power Switch directly from the TI website. Copied the contents into LTSpice and created a symbol using the LTSpice auto symbol creator. Verified X prefix is present. So far so good.

Run the transient simulation - no errors. Great! I probe OUT_1 to find that the output does something, but is virtually zero. It should be 5V. (tried higher resistances as well) Probing other nodes I see the expected voltages. Seems related to output only.

Combing through the subckt I see several subckts are being used.. and that's OK, ALL subckts are defined and accounted for. However, there are a few subckts defined in the file that are not used: CESR and SWITCH_PS... hmmm.

Enter TINA-TI. I open the TI version of the model using TINA-TI and see that they have a CESR capacitor outside of the TPS2557 macro. Back to LTSpice, autogenerate the symbol and attach X prefix to use CESR supplied subckt. Same problem. No voltage output.

I am curious if adding this unused subckt SWITCH_PS will help. Unfortunately I am not sure what it is or if it is needed. It has 3 nodes and appears to be a "switch" with a couple custom FETs. I assume it is specific to the TINA-TI simulation but can't find solid documentation. Anyone experienced this problem before? Suggestions? I can use TINA for this switch, but I am REALLY interested in the TPS2561, which only has PSPICE not TINA.

.SUBCKT NSW_PS D G S PARAMS: RONval=10k VTHval=0.7 VCHARval=0.01 CGval=0.01pF CDval=0.01pF CSval=0.01pf
RDDUM D 0 1e11
RSDUM S 0 1e11
RGDUM G 0 1e11
CG G D {CGval}
CD D S {CDval}
CS G S {CSval}
***EEXP F1 0 VALUE={LIMIT(((V(G,S)-VTHval)/VCHARval),-80,80)} 
Etest test 0 VALUE={IF(V(D) > V(S), V(G,S), V(G,D))}
GOUT D S VALUE={V(D,S)/(RONval*(1+EXP(-LIMIT(((V(test)-VTHval)/VCHARval),-80,80))))}
.ENDS NSW_PS
*$

.SUBCKT PSW_PS D G S PARAMS: RONval=10k VTHval=0.7 VCHARval=0.01 CGval=0.01pF CDval=0.01pF 
RDDUM D 0 1e11
RSDUM S 0 1e11
RGDUM G 0 1e11
CG G D {CGval}
CD D S {CDval}
***EEXP F1 0 VALUE={LIMIT(((V(S,G)-VTHval)/VCHARval),-80,80)} 
Etest test 0 VALUE={IF(V(S) > V(D), V(S,G), V(D,G))}
GOUT S D VALUE={V(S,D)/(RONval*(1+EXP(-LIMIT(((V(test)-VTHval)/VCHARval),-80,80))))}
.ENDS PSW_PS
*$

.SUBCKT SWITCH_PS A SWD SWC PARAMS: vth=500e-3 ron=1e3 roff=1e6 tdelay=1e-9 trise=1e-9 tfall=1e-9 initval=0
*
VS VSUP 0 DC 1
***** boolean ************
EBUF1 Ypp 0 VALUE={IF(V(A) > ({vth}), {1-initval}, {initval})}
ROUTpp Ypp 0 1e11
***** add delay lines ****
XNSW1 OUTp Ypp 0 NSW_PS PARAMS: RONval={(tdelay+1e-15)/(1e-12*0.693)} VTHval=0.5
XPSW1 OUTp Ypp VSUP PSW_PS PARAMS: RONval={(tdelay+1e-15)/(1e-12*0.693)} VTHval=0.5
CDEL1 OUTp 0 1pF
ETHRESH Yp 0 VALUE={IF(V(OUTp) > 0.5, 1, 0)}
ROUTp Yp 0 1e11
** Add rise and fall *****
XNSW2 OUTr Yp 0 NSW_PS PARAMS: RONval={(trise+1e-15)/(1e-12*2.3)} VTHval=0.5
XPSW2 OUTr Yp VSUP PSW_PS PARAMS: RONval={(tfall+1e-15)/(1e-12*2.3)} VTHval=0.5
CDEL2 OUTr 0 1pF
***Switch ************
EOUT VG1 SWC VALUE={V(OUTr)}
XNSW3 SWD VG1 SWC NSW_PS PARAMS: RONval={ron} VTHval=0.5
.ENDS SWITCH_PS
*$

Answer 1

I duplicated your circuit and got the same problem. I first opened up the SPICE Error Log with CTRL-L and it gives some errors worth addressing:

LTspice does not like when there are two curly braces in a row. To fix that, you have to edit the .LIB file and do a find&replace for {{ to { and then also for }} to }.

---

However, that's not enough to fix the problem you're having. I played around a bit and decided to tie the EN pin low, and that apparently "fixed" it. Well...it turns out the EN pin doesn't really function properly. I put a voltage ramp on the EN pin to see its behavior better.

Looks backwards, so I tried the TPS2556 PSpice model thinking they might've goofed up the two since that one is supposed to be the other way around...but it's apparently screwed up in its own way. Anyway, I was able to fix the TPS2557 by swapping the inputs to the analog comparator instance which compares the EN voltage against a fixed 0.88V with 55mV hysteresis. That would be this line here:

X_U1_U48         EN U1_N7637958 U1_N7643981 U1_N16726884 COMPHYS_BASIC_GEN

And switching the first two nodes would result in this:

X_U1_U48         U1_N7637958 EN U1_N7643981 U1_N16726884 COMPHYS_BASIC_GEN

Which gives me the expected output below:

NOTE: To fix the TPS2556 version, I had to do the same fix above and additionally remove the XNOR gate that's after the comparator. Welcome to the wonderful world of fixing TI SPICE models! We have T-shirts.