Need help in simulation

Post the sim project file.


Regards, Dana.

I just have tried to upload the *.asc file as a text file. I was not able to upload the *.asc file.

try this for using step directive

.op sets the operating point
you have not directed spice to do any analysis

suggest you use step 1000 1600 100
this should give 6 steps. while 1000 1600 10 should give 60 steps which means you'll just have a pretty repeating rainbow

this circuit is sufficiently straightforward that you can do it without the computer

I chose a 50 us transient test after re-drawing properly


Save .asc file, (rename version) then repeat but select it and send to "compressed file" to be attached here.

engr_joni_ee said:

Hi, I am trying to run the simulation in LT Spice but I am not sure what is missing.

Click to expand...

You have a parameter PT but it's not referenced in the circuit. Review LTspice help to learn the required syntax for parametric circuits. The component name "PT" is no correct parameter reference. Resistor component designator need to start with R, e.g. Rpt. A parameter reference for component value has the form {PT}.

Changing Reference Designation (REFDES) from PT to Rpt or even Rt1, made no different to the lack of step functions, but still functioned as a fixed resistor.

I define the variable resistor as a parameter {X}. The out put voltage is constant. It should not be like that.

The voltage across R_PT at 1000 Ohm and at 1600 Ohm is given below.

At R_PT = 1000 Ohm
Vmin = (1000/(1000 + 3900))*5 = 1.02 V

At R_PT = 1600 Ohm
Vmax = (1600/(1600 + 3900))*5 = 1.45 V

When these two voltages are subtracted by the REF = +1.02 V and amplified by the Gain 7.5. This gives the following results.

Vout_min = ( Vmin - 1.02 ) x 7.5 = 0 V
Vout_max = ( Vmax - 1.02 ) x 7.5 = 3.25 V

But in simulation, the output of the OpAmp is a constant voltage. I understand that this is a very simple circuit. But I am trying to simulate such circuit in LT Spice.

Hi,

I´m happy to you see you did some math on your own.

Before you go for "variable" values I recommend to verify your math with FIXED values in the simulation.
Then you find out that something is not like expected.
Use the simulation, disconnect wires, meausre the voltages of the nodes, see how the voltages change when you connect new parts of the schematic, measure currents.

To be honest, this circuit is somehow tricky. But you are on the right track. Go on this way.

Klaus

The step command start working. But the output voltage is not proportional to the change in resistance at R_PT. I use step command as .step param X 1000 1600 200. There should be four points, 1000, 1200, 1400, 1600. The output voltage and also input voltage is not proportional.

I suggest you use the RT LTspice model and their circuit design to compare with yours.
It was easy to find on the web. (hint)



TI also said this:


Extract zip to your preferred \lib\sim folder or make an RTD subfolder in that.

I'm not sure the best folder to put the component. asc and the circuit design.asc files

engr_joni_ee said:

The step command start working. But the output voltage is not proportional to the change in resistance at R_PT. I use step command as .step param X 1000 1600 200. There should be four points, 1000, 1200, 1400, 1600. The output voltage and also input voltage is not proportional.

Click to expand...

Problem is insufficient voltage range of AD8039. You can e.g. use AD824.

The reason this is better is because it measures resistance with constant current sink.



I still DO NOT recall any design specs for T range and max error tolerance. !!
Pls advise.

engr_joni_ee said:

But the output voltage is not proportional to the change in resistance at R_PT.

Click to expand...

It won't be when using a resistive divider for the sensor output as you have.
If you want a linear output then the PT sensor needs a constant-current source, as the circuit in post #13 does.
Some ways of doing this are by using the sensor as the inverting op amp feedback resistor, or driving the sensor with a Howland constant-current op amp circuit.

FvM said:

Problem is insufficient voltage range of AD8039. You can e.g. use AD824.

View attachment 190190

Click to expand...

Inspite of all the advice given, PT100's are good but not perfectly linear. I gave the formulae for S/W error correction from TI.
U1 in my schema does the CC error correction with Rsense from ADI.

If you don't understand my comments, ask questions? If you don't ask, then I cannot help it.

All suggestions about Pt1000 linearization, constant current drive etc. are surely relevant but essentially not answering the more elementary problem of post #1 original circuit and follow up questions.

To recall, post #1 deals with LTspice syntax and misspelled node names, post #10 with OP output voltage range. I think it's appropriate to analyze the primary problem before advancing to improved Pt1000 sensor circuits.

Please also notice thread title.

FvM said:

All suggestions about Pt1000 linearization, constant current drive etc. are surely relevant but essentially not answering the more elementary problem of post #1 original circuit and follow up questions.

To recall, post #1 deals with LTspice syntax and misspelled node names, post #10 with OP output voltage range. I think it's appropriate to analyze the primary problem before advancing to improved Pt1000 sensor circuits.

Please also notice thread title.

Click to expand...

I agree with you. I think the original problem was using a 50 µs transient mode test which was used when it failed. But there are other settings not displayed on the schematic. Normal or alternative simulation in setup) etc.

The simulation of a fixed R worked regardless of the reference label to the part. 1.014V indicates 1k as shown in step. And likewise for the original REFDES.

My link has models for both Pt100/1000.

You can share the non-obvious differences you think made it step.

.tran 0 50u 0 1u (did not work)
.op (Worked)

My personal view is to solve the bigger design problem and understand user expectations (specs) rather than the lesser on the nagging issue of LTspice idiosyncrasies. My solution did both (!). without an explanation. Yours also worked on steps and low voltage margin with the label PT instead of R_pt or whatever.

Both LTspice and design may be important skills to learn. LTspice still has bugs and a learning curve and ADI has made upgrades (see help) but still has some non-obvious settings that make either slow or fail. (No program setup fault detection). The latest version has a bug with plot grids missing too.

On this plot , I don’t see how the Problem is insufficient voltage range of AD8039. affects the step function yet the output still worked.

D.A.(Tony)Stewart said:

On this plot , I don’t see how the Problem is insufficient voltage range of AD8039. affects the step function yet the output still worked.

Click to expand...

OP output is obviously in soft saturation. You see the expected output when you put in a suitable rail-to-rail OP



Of course. the voltage output isn't linear in temperature. In the first place affected by Rpt/(Rpt + R5) transfer function, secondly by nonlinear Pt-sensor characteristic. The appropriate solution depends on circuit application range and requirements, both have been never mentioned. A simple R5 + Rpt voltage divider along with a ratiometric ADC and some software can make a pretty accurate (< 0.1 K error) digital thermometer.

I had some problem with LT Spice. I just installed the latest version. I also manage to run the simulation. For some reason we need to use OpAmp AD8397. I attach the simulation results. I am not sure the reason the red curve Vout is piece wise linear.

One reason could be, I don't have constant current source running through the PT.

I got this :




Regards, Dana