December 1, 2017 at 3:52 pmwbmckinneySubscriber
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.
December 1, 2017 at 4:40 pmpeteroznewmanSubscriber
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?
December 1, 2017 at 6:44 pmwbmckinneySubscriber
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.
December 1, 2017 at 8:29 pmpeteroznewmanSubscriber
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.
December 1, 2017 at 8:41 pmRaef.KobeissiSubscriberHello 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
December 1, 2017 at 10:48 pmwbmckinneySubscriber
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.
December 3, 2017 at 10:58 amRaef.KobeissiSubscriberIf 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.
December 3, 2017 at 9:24 pmwbmckinneySubscriber
I want to study the effect of the moving tip on the fluid flow features (i.e. flow rate & velocity exiting the tube)
December 4, 2017 at 2:13 pmraul.raghavSubscriber
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:
Ansys Fluent tutorial: Fluent FSI tutorial
Ansys CFX tutorials: Ball check value using mesh deformation tutorial
December 5, 2017 at 4:46 amwbmckinneySubscriber
Thank you for the responses, I really appreciate it.
December 6, 2017 at 8:04 amVishal GanoreAnsys Employee
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.
December 6, 2017 at 5:38 pmwbmckinneySubscriber
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?
December 6, 2017 at 6:22 pmraul.raghavSubscriber
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.
December 6, 2017 at 7:35 pmVishal GanoreAnsys Employee
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!
December 6, 2017 at 7:47 pm
December 29, 2017 at 10:38 amVishal GanoreAnsys Employee
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.
#define pi 3.141592645
DEFINE_CG_MOTION(SHM, dt, cg_vel, cg_omega, time, dtime)
a= 30 * pi / 180;
T= 120; /*period of 120 sec*/
w= 2 * pi / T;
cg_vel = 0.0;
cg_vel = 0.0;
cg_vel = 0.0;
cg_omega = 0;
cg_omega = 0;
cg_omega = a * w * cos(w*time); /*Cosine function of oscillation*/
January 2, 2018 at 7:57 amVishal GanoreAnsys Employee
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.
January 8, 2018 at 6:00 pmwbmckinneySubscriber
Thank you Vishal. I believe this is what I will need to do. I appreciate the help.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- check element type
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- execution error inside the mesher. The process suffered an unhandled exception or ran out of memory
- Conformal vs Non-Conformal Mesh
- inflation created stairstep mesh at some location
- Error in meshing
- Meshing Error
- How to resolve Mesh Failure
- How to get three elements across the wall thickness of a thin part
- Meaning of the symbol crossed out tick mark on a body in the tree outline indicate in Meshing
© 2023 Copyright ANSYS, Inc. All rights reserved.