Dynamic meshing of bending tube

  • 352 Views
  • Last Post 08 January 2018
  • Topic Is Solved
wbmckinney posted this 01 December 2017

I have tube that is approximately 100 mm long and the last 10 mm of the tube (the tip) will deflect from 30 degrees to -30 degrees. I will have a velocity inlet with pressure outlet. I have already run a static case, where I have kept the tip angle fixed but I would like to run a dynamic case to simulate fluid flowing through the moving tip. I was wondering if this is possible to simulate in ANSYS Fluent. If so, I am guessing I would have to use dynamic meshing. If anyone has some thoughts or pointers on how I would go about doing this please let me know.

Thanks.

Order By: Standard | Newest | Votes
peteroznewman posted this 01 December 2017

Will the tip deflection be an applied displacement that varies over time, or is the tip deflecting due to the forces of the fluid exiting the tube? In other words, is it like something is holding the end of the tube and moving it, or is something holding the tube 10 mm back and it is just free to deflect? Which direction is gravity relative to the tube axis?

wbmckinney posted this 01 December 2017

The tip deflection will be an applied displacement that varies over time (something holding end of tube and moving it). The tube is horizontal with the tip deflecting 30 degrees from the horizontal axis. Gravity is perpendicular (down) relative to tube axis.

peteroznewman posted this 01 December 2017

When you say 30 degrees from the horizontal axis, do you mean up 30 degrees and back down to 0 degrees? What is the period of motion in seconds for one cycle of up/down?

I know about structures, but am a beginner on Fluid-Structure-Interaction (FSI), but one thing I recall is you get to choose if you want a one-way FSI or a two-way FSI.

A one-way FSI would be where the structure deforms then the fluid follows the structure walls. A more typical one-way FSI is where the fluid flow is solved first, then the pressure from the flow is applied as a load to the structure to see how much it has deformed, but those are steady state analyses.

A two-way FSI is where the forces of the fluid flow deform the structure as well as the effect of a rotational displacement of the tip. I think this is where you will end up building the model.

I can imagine a Transient Structural system that applies a sine wave rotational displacement on the tip with an amplitude of 30 degrees. The material properties of the tube (density and modulus) and its diameter and wall thickness as well as the density of the fluid will determine the dynamic response of the system, but if the period is long, the tube deformation will be close to the static solution.

I expect a member with some deep FSI knowledge will have a comment.

  • Liked by
  • wbmckinney
Raef.Kobeissi posted this 01 December 2017

Hello you will need to ise system coupling (transient structural + Fluent) which is defined as an FSI simulation. To let you know: Academic Student Version of ANSYS does not support system coupling Cheers

Raef Kobeissi

  • Liked by
  • wbmckinney
wbmckinney posted this 01 December 2017

Thank you for the responses. The tip will move 30 degrees up and back down to -30 degrees for one cycle. This will be the effect of an external device causing the tip deflection. The period of motion is unknown as of now but will be slow. For this case, will I need to do a one-way FSI or two-way FSI if I am wanting to look at a transient case?

Is this simulation practical for a grad student without any prior knowledge of FSI simulation?

Also, is there any previous research, tutorials, or information that y'all might recommend concerning FSI simulation and meshing. 

Thanks, 

Will McKinney 

Raef.Kobeissi posted this 03 December 2017

If you want to study the effect of fluid on the structure of an object it would a 2 way- coupling - FSI os always 2 way coupling. Cheers

Raef Kobeissi

wbmckinney posted this 03 December 2017

I want to study the effect of the moving tip on the fluid flow features (i.e. flow rate & velocity exiting the tube)

 

 

raul.raghav posted this 04 December 2017

As far as your case is concerned, it would be a 2-way FSI problem. It would be an iterative process where after every timestep,

1. the results from fluid model (pressure etc.) will be transferred back to the structural problem which will be solved, and

2. then the results from the structural model (deflection, deformation etc.) will be transferred to the fluid model which will be solved and this goes on and on.

Remember that this would require extensive computational effort and as Raef mentioned the student version of ansys has limitations on the 2-way FSI. A simpler way of approaching the problem would be considering it as a fluid dynamics problem with a dynamic mesh if you can somehow derive a time-varying deflection data.

Some tutorials that might be of help to you if you have the computational resources to perform a 2-way FSI:

Raef has an amazing tutorial for a 2-way FSI of a vibrating plate problem with Ansys Fluent on youtube:

A tutorial similar to what you want to model with Ansys CFX on youtube:

  • Part-1:
  • Part-2:
  • Part-3:

Ansys Fluent tutorial: Fluent FSI tutorial

Ansys CFX tutorials: Ball check value using mesh deformation tutorial

Oscillating plate 2-way FSI tutorial

Good luck !

Rahul

  • Liked by
  • wbmckinney
  • Raef.Kobeissi
wbmckinney posted this 05 December 2017

Thank you for the responses, I really appreciate it.

Regards,

Will McKinney

vganore posted this 06 December 2017

Raef has created a super tutorial but it is more relevant in understanding how fluid forces (pressure) will deflect the tube. I guess that is the reason why 2 way FSI is used. 

Will, I guess you have an external motor/device deflecting your later 10 mm tip. It has nothing to do with fluid forces causing deflection. It could be simply rotation of a tip with (+or-30 degree) or SHM by defined external mechanism. If so, could you tell me what rotational velocity (omega) are you using or is it SHM? I am guessing your solution to the problem has a different approach. 

Vishal Ganore, ansys.com/student

  • Liked by
  • wbmckinney
  • Raef.Kobeissi
wbmckinney posted this 06 December 2017

Yes, I will have an external device deflecting the 10 mm tip. That is correct, I am not looking at fluid forces to cause deflection. It will be SHM defined by the external mechanism. I am unsure of the period of motion at this time, but it will be slow. Do you have a suggestion for this approach?

Thanks,

Will McKinney

raul.raghav posted this 06 December 2017

Can you share some images of your analysis where the tip angle is fixed? I assume you ran cases with tip angles 30deg, 15deg, -15deg and -30deg.

Rahul

vganore posted this 06 December 2017

Hi Will, You need a simple UDF (User defined function) to define SHM motion and assign it to tip portion. I will create a short demo for you to help you get started. Stay tuned! 

Vishal Ganore, ansys.com/student

  • Liked by
  • wbmckinney
wbmckinney posted this 06 December 2017

10 degree - Velocity magnitude slide20 degree - Velocity magnitude slice30 degree - velocity magnitude slice

I have done analysis at 10, 20, and 30 degree tip angles as shown in the 3 pictures. It was run with a velocity inlet of 10 m/s and pressure outlet along the outer domain extents. I am looking at the flow velocity exiting the tip and up to 10 mm downstream of the exit.

vganore posted this 29 December 2017

I would neglect tube thickness for internal flows unless you have specific significance for it (heat transfer across wall etc.). Sample of the SHM UDF you need is given below (& attached). I assumed maximum 30 degrees of displacement (amplitude) and total period of 120 seconds (time to complete one oscillation).

Compile this UDF in fluent to assign SHM motion to relevant boundaries. 

/*********************************************************************/

#include "udf.h"

#include "math.h"

#define  pi 3.141592645

 

DEFINE_CG_MOTION(SHM, dt, cg_vel, cg_omega, time, dtime)

{

real a,w,T;

Thread *t;

 

  a= 30 * pi / 180;

  T= 120; /*period of 120 sec*/

  w= 2 * pi / T;

  cg_vel[0] = 0.0;

  cg_vel[1] = 0.0;

  cg_vel[2] = 0.0; 

  

  cg_omega[0] = 0;

  cg_omega[1] = 0;

  cg_omega[2] = a * w * cos(w*time); /*Cosine function of oscillation*/

}

Vishal Ganore, ansys.com/student

Attached Files

  • Liked by
  • wbmckinney
vganore posted this 02 January 2018

AND here is the quick animation of dynamic mesh showing how the mesh motion is diffused in the domain. Motion UDF is applied to moving walls flapping with SHM.

Vishal Ganore, ansys.com/student

  • Liked by
  • wbmckinney
wbmckinney posted this 08 January 2018

Thank you Vishal. I believe this is what I will need to do. I appreciate the help.

Regards,

Will McKinney

Close