I was attempting to simulate my design using TIs TPS1H100A-Q1.
I keep getting an error that I have less than two connections at the CL pin. ERROR(ORPSIM) -15141): Less than 2 connections at node CL.
Unable to solve this I opened up TIs refernce design in TI PSPICE, I use ORCAD 17.4, but get the same error.
I have not made any changes to the circuit. Just oepened it up and ran the simulation.
Error log is below.
Any suggestions?
** Creating circuit file "tran.cir"
** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS
*Libraries:
* Profile Libraries :
* Local Libraries :
.LIB "../../../tps1h100a-q1_trans.lib"
* From [PSPICE NETLIST] section of C:\Users\H357321\AppData\Roaming\SPB_Data\cdssetup\OrCAD_PSpiceTIPSpice_Install\17.4.0\PSpice.ini file:
.lib "nom_pspti.lib"
.lib "nom.lib"
*Analysis directives:
.TRAN 0 1m 0 20n
.OPTIONS ADVCONV
.OPTIONS ABSTOL= 10n
.OPTIONS ITL1= 1500
.OPTIONS ITL2= 400
.OPTIONS ITL4= 400
.OPTIONS VNTOL= 10u
.PROBE64 V(alias(*)) I(alias(*))
.INC "..\TPS1H100A-Q1 Timing Response.net"
**** INCLUDING "TPS1H100A-Q1 Timing Response.net" ****
* source TPS1H100A-Q1_TRANS
V_V2 DIAG_EN 0 5V
R_RLoad OUT 0 10 TC=0,0
V_V1 VS 0
+PULSE 0 13.5 0 100n 100n 1 2
V_V3 IN 0
+PULSE 0 5 0.3m 10n 10n 0.4m 2
R_RCL CL 0 1.233k TC=0,0
X_U1 IN DIAG_EN N16800324 CL N16791011 N16797670 N16790983 VS VS VS OUT
+ OUT OUT 0 0 TPS1H100A-Q1_TRANS
**** RESUMING tran.cir ****
.END
ERROR(ORPSIM-15141): Less than 2 connections at node CL.
ERROR(ORPSIM-15141): Less than 2 connections at node N16790983.
ERROR(ORPSIM-15142): Node N16791011 is floating
Copyright © 2020 Cadence Design Systems, Inc. All rights reserved.
Something doesn't seem right here. The order of the names in the subcircuit definition for TPS1H100A-Q1_TRANS
don't line up with the PSpiceTemplate property of the TPS1H100A-Q1_TRANS part.
Template=> X^@REFDES %IN %DIAG_EN %STB %CL %NC1 %NC2 %NC3 %VS1 %VS2 %VS3 %OUT1 %OUT2 %OUT3 %GND %PAD @MODEL
SubCir Def=> .SUBCKT TPS1H100A-Q1_TRANS DIAG_EN VS_1 VS_2 VS_3 CL IN ST_CS_N NC_1 NC_2 NC_3 PAD OUT_1 OUT_2 OUT_3 GND
I see what you mean. Odd. ORCAD put up a message that it updated the library pats when I opened TI PSPICE.
I wonder if the order of the template versus subckt was changed at that time.
It must have worked when TI released the part.
This is my first time using PSPICE for TI. Sadly not a good experience so far. I did run another test using a TI INA137 and that worked fine so at least I know the tool can work.
I got this transient simulation to work in PSpiceforTI by doing the following:
1) Tie each of pins STB, NC1, NC2, and NC3 through a separate 1G resistor to GND.
2) Select U1 then select Edit Properties
3) Replace the PSpiceTemplate property with:
X^@REFDES %DIAG_EN %VS1 %VS2 %VS3 %CL %IN %STB %NC1 %NC2 %NC3 %PAD %OUT1 %OUT2 %OUT3 %GND @MODEL
P.S. This is not the first time I've had problems with TI's models.
Al,
Excellent! It works now.
Thanks so much for your help.
This gives me a clue as to what kinds of things to look for in the future.
If a simulation is lying though in the future due to a subckt problem...I don't know.
I like to start off simple with an outcome I already know to gain confidence.
Thats why I went to the TI design. Figured it would work then I could just modify their circuit.
Wondering how this could have ever been tested.
Thanks for your help.
Now that the component seems to work I can model my circuit.
Steve
The main idea of this part is to control current into a load.
I placed a current marker at the OUT pin or RLoad.
I also have a voltage marker on the pin. PSPICE is not reporting any current but does report the voltage.
Would this be a problem with the model or my ability to use it?
Obvioulsy I can use a calculator but then what is the purpose of the tool?
This is my first time using PSPICE for TI or ORCAD PSPICE so I might be missing something.
Typicallly I use LTSPICE but thought it would be nice if I could model my TI circuits as well to help ensure 1st time success with a board.
Don't think you can mess up this part as value changes would solve most problems. (TPS1H100A-Q1)
Thought using PSPICE for TI with an actual TI circuit might aid my learning curve by working on a known good circuit.
That theory is now blown.
Thanks for all of the help out there.
Steve
Silly me. The cursor was on a 0V section of the transient response on the graph. I'm used to seeing a current pulse as well as a voltage pulse during the transient. (LTSPICE)
Once I turned on the values at the bottom of the graph and drug the cursor over to a positive pulse I could see a current readout.
Not quite what I'm used to but the information is there. Guess there is a bit to learn about the tool yet.
Steve
Greetings! It appears to be really intriguing.I have a strong sense of aesthetics and beauty, and I make it a practice to carefully notice even the slightest aspects in my work. I just came across some amazing concepts like squeegee . This revelation has motivated me to develop new templates and investigate novel design ideas.
Hey there!