Displacement results: Correct values or computatiional noise?

[Alphaoo1]

Hello,

I am running a preCICE coupled simulation on an Abrasive Water Jet Nozzle.
I have particles impacting the solid.

I have the material of the Nozzle as Tungsten:

*MATERIAL, Name=EL
*ELASTIC
705000000000., 0.31

*DENSITY
 15570

.
I am monitoring displacements at two points.
The displacements are in the range of 1e-08m to 1e-07m.

After looking at the displacement visually, I can confirm that the displacements seem ok, as I can see maximum displacements at impact sight of particles.
Here is a plot of displacements:

How can I make sure these values are correct and not just computational noise?
(this is a question raised by one of the colleagues)

Here is the simulation type I am running:

*STEP, NLGEOM, INC=1000000
*DYNAMIC, DIRECT
1.E-6, 0.997
*RESTART,WRITE,FREQUENCY=1

Thank you.

[Calc_em]

@Alphaoo1

*DYNAMIC, DIRECT

Do you need direct incrementation for coupling or something ? Normally, it should be avoided in most cases.

What about the output frequency ? How often are the results saved ?

[Alphaoo1]

Do you need direct incrementation for coupling or something ? Normally, it should be avoided in most cases.

Yes, I am coupling CalculiX with [article and fluid solver using preCICE.

What about the output frequency ? How often are the results saved ?

The output frequency is the same as increment, each time-step i.e. every 1e-06s.

[vicmw]

You can run it with different time step and mesh sizes to confirm that the results are independent of those.

[JohnM]

Run a modsl analysis on your structure, you may find it is revealing a response frequency at 1100Hz.

[Alphaoo1]

Thank you for your replies @vicmw, @JohnM

You can run it with different time step and mesh sizes to confirm that the results are independent of those.

I will perform a mesh independence study, and get back.

Run a modsl analysis on your structure, you may find it is revealing a response frequency at 1100Hz.

The first mode frequency comes out to be 818Hz.
But I should point out the results seen above are from a coupled simulation.
There is a high pressure, high velocity water jet inside the nozzle as well as particles impacting, thus we should expect the stressed nozzle to have higher frequency, correct?

[vicmw]

thus we should expect the stressed nozzle to have higher frequency, correct?

Compressive stress usually decreases natural frequency and tensile stress increases it. If you have radial pressure on the inside of a tube, I imagine it could increase the frequency of some modes and decrease others because there would be both compressive and tensile stress.

Are you modelling individual particle impacts, which would have some sort of frequency distribution themselves?

[Disla]

I don’t have experience with FSI but ¿wouldn’t be expected a noticeble reduction in natural frequencies for the model submerged compared with the same model in vacuum?. There is a lot more mass (fluid) added to the system.

A quik search seems to support this intuitive idea. This file has some verification example for a cantilever beam with different aspect ratios.

Analyzing Free Vibration of a Cantilever Microbeam Submerged
in Fluid with Free Boundary Approach
K. Ivaz1†, D. Abdollahi1 and R. Shabani2

1100 Hz —> 818 Hz seems plausible.

As others has comment I would try to identify that periodic oscillation pattern. If I were on an evaluation board I would be courious about it.

[fgr]

@Alphaoo1
I have worked a little for the possibilities if i could manage to do some verification for impact between objects both in dynamic implicit and dynamic explicit.
For the test I used 2 bars as shown with the golden rules from the calculix manual, element type C3D8 and linear contact node to surface.

The manual recommend contact pressure between 5-50 times Young’s modulus. For some other reasons I choose to start some lower with the following rows of factors:
0.4, 0.6, 0.8, 1.0, 1.2, 1.4, 1.6, 2.0, 5.0, 50.0 multiplied with Young’s modulus.
Looking at the relative energy balance I got the following curves:

The curves made me suspicious why I decided to extract the velocity curves during the impact which looks like this:

As shown at the curves, then the velocity gets instable when the contact pressure get close to upper manual recommendation for the contact pressure, and what’s quite so important, the duration of impact vary with the value of contact pressure which also give a variation of the impact force or the damage.

So a question I actual could like to ask everyone in this forum:
What should be the correct contact pressure if I/one wanted to have the correct maximum impact force ?

[Disla]

Hi fgr,

Could you describe your objects dimensions and material properties?
I would like to look at one detail in your plot.

[fgr]

@Disla
The dimensions as follows:
0.01 x 0.01 x 0.03 m, density 7800 kg/m^3, Young’s modulus 2.1E+11 N/m^2, initial condition box 1, Vx = -1 m/sec, initial condition box 2, Vx =0 m/sec.

Initial distance between object = 0.0001 m for minimizing calculation time.

Key values from data set with contact pressure = Young’s modulus:

*Element, Type=C3D8, Elset=Box2
*Element, Type=C3D8, Elset=Box1

** center nodes of the opposite surface of contact surfaces
** to extract velocities during impact as a function of time
*Nset, Nset=Center
146, 251

*Material, Name=Steel
*Density
7800
*Elastic
2.10E+11, 0.3

*Solid section, Elset=Internal_Selection-1_Solid_section-1, Material=Steel

*Surface interaction, Name=Surface_interaction-1
*Surface behavior, Pressure-overclosure=Linear
2.10E+11, 2860000

*Contact pair, Interaction=Surface_interaction-1, Type=Node to surface, Adjust=0
Slave, master

*Initial conditions, Type=Velocity
Box1, 1, -1
Box2, 1, 0

*Step, Inc=10000
*Dynamic, Direct, Solver=Pardiso
1.0E-06, 0.0005

*Node file
RF, U, V
*Output, Frequency=1
*Node print, Nset=Center, Totals=Yes
V
*El file
ENER
*End step

I also composed a pure elastic transfer function for this case. Despite of the discussion whether this function can be more or less correct, it gave me values quite close to what obtained in a similar ANSYS simulation.

[Alphaoo1]

thus we should expect the stressed nozzle to have higher frequency, correct?

Compressive stress usually decreases natural frequency and tensile stress increases it. If you have radial pressure on the inside of a tube, I imagine it could increase the frequency of some modes and decrease others because there would be both compressive and tensile stress.

Are you modelling individual particle impacts, which would have some sort of frequency distribution themselves?

Yes, I have radial pressure acting from inside the tube.
Additionally, I am using a DEM solver to solve for particles, thus they give individual impacts.

AWJC Results if someone is interested in having a look: https://www.youtube.com/playlist?list=PLcRlzAyzOZyR9wpeDJEWgTdm3qVVLVzqL

Some of the old simulations with FEM use steel or some soft material to exaggerate the displacements.
Displacements for tungsten Nozzle with the plot for Vel. 4 : (https://youtu.be/dbStvp0VqhM)

@fgr Thanks a lot of the detailed response and input file, I will try and understand. I have more questions based on your question to the forum -_-

[Disla]

There is not too much accuracy as I’m measuring on the pdf but your perturbation has approximately:

1cicle / 0.000012 seconds = 83,333 Hz

NOTE:Do not care about units. It’s not mm but seconds. It’s my pdf software.

While a frequency analisys shows 90,174Hz for your first longitudinal mode.

That seems suspiciously close. May you have excited the first longitudinal mode as this is how you are applying the impact.

If that is confirmed (I would check if Strain Energy is showing the same pattern) the question would be , why some contact stiffness is able to excite that mode and not the others?.

Are you computing some cases with Explicit while others with Implicit?

[fgr]

For the first plot, all curves are generated in Dynamic Implict as written in the plot title.

For Dynamic Explicit they look like this, where at least 2 pair obviously is wrong since one pair come out with more energy than before the impact/collision and another with less energy.

[Disla]

@fgr

one pair come out with more energy than before the impact/collision and another with less energy

Don’t know. I can’t tell from that graph. Which one has less energy than before? I think Kinetic Energy would be more representative. Is that velocity the magnitude sqrt(vx^2+vy^2+vz^2) for some point?. Are you considering Strain Energy into the balance?

[fgr]

@Disla
You got me and thanks for that, I was wrong and didn’t imagine that change in the relative energy balance could be a matter of stored vibrating strain energy.

I also need to recognize that time duration of impact will converge when contact pressure get close to 50 times Young’s modulus which in this case also is close to what I obtained by a pure elastic analytic transfer of the energy.

For me the next question of interest could be, can it really be true for such relative short object that fluctuations of internal energy can cause up to 20% variation from the mean velocity of the object.
But in fact, reducing the length of the object should also reduce the stored strain energy pr. square unit in axial direction, so that could be an option I could try.

[JuanP74]

looks similar to the analysis of drill steels in rock drilling, and reflected waves inside the drill steel are highly dependent on geometry and length of the drill steel in what regards energy transfer:

The primary motivation in performing the analyses reported herein was the desire to
ascertain (1) what parameters affect the efficiency of conversion of the stress wave energy
in the drill steel into work done by the bit in breaking rock and (2) how high an efficiency
value can be obtained under optimum values of these parameters.
The present computations are limited to the ‘long’ drill steel case; that is, the drill steel
is assumed to be long enough for the stress wave at the junction between the anvil block
coupling and the top of the drill steel to have decayed to a negligible amplitude before the
wave reflected at the bit end of the drill steel returns to this location. This condition is
applicable to drilling machines with drill steels at least about 10 times as long as the strikers,
as seen from the results of the digital machine computations mentioned above. This excludes
the so-called ‘down-hole’ machines from the present considerations.
https://www.sciencedirect.com/science/article/abs/pii/0148906264900063