[newuser!]

Hi all,

I try to run a FSI using ANSYS WB with transient structural and FluidFlow (CFX). My model consists of a rigid pipe, filled with water and closed by a thin membrane at one end.

Now I would like to apply a static pressure load on the other end of the fluid. The water should not exit the pipe --> only inflow.

My questions using CFX are:
1) Which kind of Boundary type I have to choose in CFX? Opening or Inlet
I think I should take inlet, because flow only enters the pipe. Is that correct?

2) Applying a static pressure of 250Pa instantaneous (Mass and Momentum-Option-static pressure), the solver fails immediately. How can I apply a static pressure e.g. with a timedependent, linear ramp in CFX?
For expression I can define P=(250*(t/1[s]))[Pa] using P for BC static pressure value. Would that be correct for a linear pressure ramp with pmin=0Pa and pmax=250Pa, if T=1sec? How I can define a Ramp like this: (t=0s/P=0Pa), (t=0.1s/P=250Pa), (t=T=1s/P=250Pa)?
Di I have to use user functions with tabular data?


Thank you very much,
regards
Philipp

[Soolmaz]

Hi,

For the first question, it really depends on the model, physics, ... but as I know in general, if you set bc to inlet/outlet, it complaines in the Solver Manager while running and advises to change bc to OPENING if the behavior persist.

For the second question, I would say you can define a 1D interpolation function. Either you can do it manually with each data, or the wiser way is to IMPORT DATA. Consider to insert dimensions in the Argument and Result parts, so for your cas for example it may be [s] and [Pa], respectively.

Generally I advise that you run just in cfx frist and then go for FSI.

[singer1812]

Are you using slightly incompressible water?

With fixed properties, the pressure at the inlet is going to try to transfer instantaneously throught the fluid. This would be highly unstable.

I think you are on the right track. Ramp the pressure, make the water slightly compressible. I assume your ramp in pressure is akin to the real ramp. This will allow the pressure wave to travel through the fluid.

[newuser!]

Thank you very much for your hints.

I now use a pressure ramp (0ms/0Pa), (7ms/250Pa), (100ms/250Pa). My reference pressure is pref=1atm=101325Pa.
The material properties of the predefined material "water" I modified adding for the density the expression: "( 997 / (1 - (Absolute Pressure - 101325 [Pa] ) / 2.04e9 [Pa] )) [kg m^-3]".
So I would expect pressure waves in the fluid and the max. abs. pressure should be round about p=p_ref+p_load = 101500Pa. For table generation I set max. abs. pressure=1e8Pa (min abs press: 500Pa).

The solver starts, but
CFX returns after 55time steps the first warning, which persists until the simulation fails: "Independent variables were clipped during table generation at: END OF TIME STEP"
"0 detailed warnings were printed because the maximum number of warning messages was exceeded."

The error for aborting the simulation occurs in ANSYS:
"Excessive thickness change in Element 798. "

I think it's due to the excessive high Force Fz at the interface, as noticed in the .stdout file of CFX:
FORCE SUM FOR FIELD 1 ACROSS INTERFACE 1
RECEIVING FORCE FX SUM = 0.11597
RECEIVING FORCE FY SUM =-0.19948
RECEIVING FORCE FZ SUM = -1910.8

So my questions are:
1) Why I get so high absolute pressure values especially at the Fluid-Structure Interface (see appendix pabs_Interface)? These values causes high Fz and lead to element distortion, or?

2) Why occurs warnings regarding CFX table generation even though I do dot reach pabsmax=1e8Pa? The pabs at the loading surface remain in a resonable range....

Any hints are appreciated ...

Kind regards
Philipp

[tonyOdili]

Good day every one,

Please I am new to simulation and I need help in carrying out a simulation work.

I am working on "The Effect of varrying blade angles of an impeller in a multage stage centrifugal pump". I am to varry the exit blade angles of a three stage centrifugal pump to see the effect it has on the output discharge, pressure and efficiency of the pump.

Anyone who is willing to help should mail me "odilianthony24@gmail.com" and we can discuss more on the topic and how much I will pay to get the work done.

Thank you.

[mvoss]

How much under-relaxation did you apply?
How tight did you solve for the meshmovement? Try to use a smooth function (n^3, tan,...) for the pressure function-e.g.

ramp = (-2*(min((t)/RampLength,1))^3+3*(min((t)/RampLength,1))^2)
RampLength= 0.1[s]

Oscillation and exploding forces,pressure, deformation can arise from the artificial-added-mass effect. Kicks in on low density ratios and small time-steps...-->tighten up the convergence in the z-dir for the interface convergence. Set the relaxation to 1 for the deformation and completely damp the system by applying relaxation to the transferred forces.