[ghorrocks]

This thread discusses many ways to do it.

You can use the <Variable>.Time Derivative method - this is preferred if it works for the variable you want.

You can write a user fortran routine to do it. Then you can do anything, but user fortran requires a bit of work to learn to use.

You can use the TRANS_LOOP approach. Most of this thread is on this approach, but note it is unsupported and does not seem to work for soem cases.

[zh&c]

I followed the method in this literature but the expression for the last time step I don t know how to determine.



https://www.researchgate.net/publica...l_in_ANSYS-CFX

[ghorrocks]

Doesn't that paper and lots of posts on this thread explain how to do it?

If you are having problems with getting it to work then you need to tell us what your problem is (like an error message).

[zh&c]

There seems to be no problem with the setting, the calculation has converged, but the results are not accurate, I calculated the data of three cardiac cycles.

This is my CEL.





Beta = C*R2/Deta t
Blood Density = 1050[kg/m^3]
C = (1.7529*10^(-10))[m^3/Pa]
Deta t = 0.02[s]
Inlet Flow = Function Inlet Flow 3(t)*Blood Density
Normal V = ((w)-(w.Time Derivative*dtstep))
P = (((R1+R2+R1*Beta)*QN+Beta*Previous Outlet Pressure \
-R1*Beta*Previous Outlet Flow )/(1+Beta))
P0 = 96.2327[mmHg]
PN = areaAve(Pressure )@OUTLET
Previous Flow = abs(areaInt(Normal Velocity )@OUTLET)
Previous Pressure = (areaAve(Pressure )@OUTLET-(Pressure.Time \
Derivative*dtstep))
Q0 = 0.39[l/min]
QN = abs(areaInt(w)@OUTLET)
R1 = (2.4875*10^8)[Pa*s/m^3]
R2 = (1.8697*10^9)[Pa*s/m^3]

ADDITIONAL VARIABLE: Normal Velocity
Option = Definition
Tensor Type = SCALAR
Units = [m/s ]
Update Loop = TRANS_LOOP
Variable Type = Specific
END
ADDITIONAL VARIABLE: Previous Outlet Flow
Option = Definition
Tensor Type = SCALAR
Units = [ml/s]
Update Loop = TRANS_LOOP
Variable Type = Volumetric
END
ADDITIONAL VARIABLE: Previous Outlet Pressure
Option = Definition
Tensor Type = SCALAR
Units = [mmHg ]
Update Loop = TRANS_LOOP
Variable Type = Specific
END

[ghorrocks]

There is a LOT more to getting an accurate result than a bit of CCL. Did the calculations of the previous values you included work?

[zh&c]

I use the data in the literature, but there is a big gap between my results and the literature, so I think there is still a problem with the expression of my export flow. I use the area score of the normal speed of the export, but this seems to have a certain error with the expression of CFX: massFlow() @OUTLET / Blood Density.

[Jiricbeng]

Hello guys,

for some kind of reason, the approach based on creating the expression with .Time Derivative does not work.
I tried Pressure.Time Derivative, Velocity u.Time Derivative, Temperature.Time Derivative... I always get the error message about unrecognised name.
I save each time step. Is there needed any special setting in CFX Pre ?

Do you have any idea please?

[ghorrocks]

Can you attach the CCL of your simulation? You can export this from CFX-Pre.

[Jiricbeng]

Please, see the attachment..

[Opaque]

Originally Posted by Jiricbeng

Hello guys,

for some kind of reason, the approach based on creating the expression with .Time Derivative does not work.
I tried Pressure.Time Derivative, Velocity u.Time Derivative, Temperature.Time Derivative... I always get the error message about unrecognised name.
I save each time step. Is there needed any special setting in CFX Pre ?

Do you have any idea please?

What release version are you using? I used it all the time, and your syntax is correct.

[Antanas]

Originally Posted by Opaque

What release version are you using? I used it all the time, and your syntax is correct.

According to info in the file this is 2022 R2.

[Jiricbeng]

Yes, the version 2022 R2. However, version 2023 R2 does not work either (I opened the results in CFD Post). But I do not think it is matter of version as this did not work to me even a few years ago.
May that be some defaults, e.g. something dug in inside the expert parameters?

[Opaque]

Originally Posted by Antanas

According to info in the file this is 2022 R2.

That should work; however, the answer is conditional.

.Time Derivative ONLY works in the CFX-Pre/Solver environment. It does NOT work in CFD-Post unless the variable is already written by the solver.

Then, where are you trying to use it? CFX-Pre, or CFD-Post.?

[Jiricbeng]

I am sorry for the late answer. I did it also in CFD Pre as expression:

Pressure.Time Derivative


But when clicking on this in CFD Post, it says: The following unrecognised name was referenced: Pressure.Time Derivative.

I tried also areaAve(Velocity u.Time Derivative)@rotating in CFX Pre, as the previous case is "variable", but there is still the same error in CFD Post.

[Opaque]

Originally Posted by Jiricbeng

I am sorry for the late answer. I did it also in CFD Pre as expression:

Pressure.Time Derivative


But when clicking on this in CFD Post, it says: The following unrecognised name was referenced: Pressure.Time Derivative.

I tried also areaAve(Velocity u.Time Derivative)@rotating in CFX Pre, as the previous case is "variable", but there is still the same error in CFD Post.

If the variable XXX.Time Derivative is not already in the results file, CFD-Post will show that error message -> The variable does not exist, and it is NOT able to compute it.

It seems you were able to finish the simulation using XXx.Time Derivative in your expressions, correct?

[Jiricbeng]

Originally Posted by Opaque

It seems you were able to finish the simulation using XXx.Time Derivative in your expressions, correct?

Yes, I defined the expression in CFX Pre, computation ran without problems and finished. And this message appears in CFD Post.

[Jiricbeng]

Any ideas please? May I share the file with you to test it? Or vice versa, if some of you could share the cfx file where it works...

[Opaque]

Originally Posted by Jiricbeng

Any ideas please? May I share the file with you to test it? Or vice versa, if some of you could share the cfx file where it works...

CFD-Post does not support those variables, XXX.Time Derivative UNLESS they ARE already in the results file.

[Jiricbeng]

Opaque, thank you for clarifying.
So, to sum it up again, how shall I understand it - I defined the variable "Pressure.Time Derivative" in Pre, then ran the solver and opened the result file in CFD Post. But for some reason this variable does not work in CFD Post.
I understood that situation to be strange and that it should work. Or, please, did I miss some step in between?

[ghorrocks]

Have you tried going to the CFX-Pre output tab and putting [variable].Time Derivative in the results file? It looks like by default they are not included in the results file.