Good morning. You can enable de user-defined option in de Dynamic Mesh Zones pane. Doing so, in the Motion Attributes tab you will be able to select a user defined function to define the geometry of the deformable zone in each time step. Actually, the macro DEFINE_GEOM allows you to do that. However, in my experience you probably don't really need to do that, since the available options in the Dynamic Mesh Zones pane should be able to overcome with any further problem (although of course the in-time mesh generation is not under your control).

Thank you Antonio for your comprehensive respond, I really appreciate you.  It is good idea to load the geometry as you said and then automatically mesh the geometry by using the dynamic mesh feature. My problem is that because my geometry deformation is not harmonic, in the other hand I cannot define a function to change the geometry accordingly, so can I construct geometry for different time steps and then load here by using the DEFINE_GEOM? For your information, I construct the geometry by using the medical images (CT scan).

Thank for your explanation. DEFINE_GEOM allows you to set the new position of the nodes according to what you define. That definition can be brought up by a embedded formula in your UDF code, but I think it might come form a reading out from an external file containing your desired node locations at each time step. I guess the time to program it would not be short, neither the real time for solving each time step. Let me know what do you think.

But thinking in other different option, what you really could do is define a motion routine for your boundaries, no matter how complicated or not harmonic would be. Say, you can use the UDF to read out a file containing a time serie of boundary positions, and let FLUENT do its best. Of course we are using a UDF, but it is easier to define the motion of a set of boundaries individually, that define the motion of a whole set of nodes. Let me know what you think about that.

Good morning , I’m interested by deformed geometry in Fluent i'm Phd student and i'm working about Blood Flow in arteries ( dilated arteries ) i think that in this case we have to use unsteady boundary conditions and the deformation of the geometry depend on the change of pressure condition ( i used in my work unsteady boundary condition with UDF ) .  I think that you can use Fluid Structure Interaction FSI by coupling fluent with Ansys Mechanical or Ansys CFX .

Hi Belkacemi, I am grateful for your response. As you mentioned, one approach to solve the boundary deforming problems (or FSI problems) is the coupled FSI (couple the CFD and structural solver by using the ANSYS Workbench), but it is very difficult to employ in high deforming problems such as the heart or heart valve (The solution is very unstable due to the low elasticity of the solid part). FYI, I am familiar with this approach and I simulated graft and stenosis artery by using the coupled FSI before. However, the alternative approach is the geometry prescribed method that only the fluid domain is solving by defining the deformation of the fluid-solid interface as the moving boundary (By using the ALE formulation). I am trying to use this approach, so I need to prescribe the motion of the wall to the solver. Antonio proposed a good suggestion but it needs to develop a complex UDF (reading the boundary from external file), however I will try to do it.

Morning all. Yes, a complete UDF is totally required of course. For harmonic motion it is really easy and I would suggest you to set a simplified case to check how it goes. For not-so-harmonic motion you can however take advantage from System Identification tools, for example ARX, ARMAX or Hammerstein-Wienner models, I mean, models that provide you with a fairly good analytically description a non harmonic system. I have used those kind of models to predict transient states in wave energy systems with reasonable good agreement with theoretical predictions. Let me know if you want further information.

Good morning all. Yes, DEFINE_GEOM proposed by Antonio is a good suggestion and DEFINE_ GRID_MOTION can be used .But i think that by using it we assume that the deformation is prescribed but i'm not sure if in reality the deformation is known (for example heart or aortic aneurysm in my case) except if you have a medical image at different time step? 

Hi Siamak,

Take a look at the flowing paper. I thing they did similar simulation as the one you are intending to do (CFX was used, but the concept is similar). you might be able to contact the author and ask for details. 

http://link.springer.com/article/10.1007%2Fs13239-014-0187-5

As another approach, if you have all of your geometries meshed separately (you should have say 1500 .msh files), and if all of them have the same topology (same BC, ...) you can create an event file that loads the new mesh at the end of each time step  and map the data from the previous time step on the new mesh. You can try to do it manually for a couple of time steps and if it works, writing the event (journal) file is not hard. (You need to find a way to automatically generate your mesh files!)   

And, out of curiosity, how come that your geometry deformation is not harmonic? I am asking this because all biomedical applications that I've encountered with were inherently harmonic (they were somehow linked to cardiac pulsations).

Hi Soroush,

Thank you for your clear and helpful explanation, I will read abovementioned paper.

I think the word “harmonic deformation” leads confusion in above comments; maybe I could not convey my meaning or maybe I used incorrect word to describe it. As you said, the biomedical motions are almost harmonic but I didn’t mean it in previous comments. Let me describe my problem first and then explain it. My model is the simulation of the heart and I am using MRI images. As you know, each medical image includes about 20-30 images for one cardiac cycle (it depends on the heartbeat), but because the extracted geometries from medical images don’t have enough temporal resolution, so need to generate intermediate images between main images to reach desired time steps. The intermediate geometries must be reconstructed by using the interpolation of the each grid position. Because the motion of the grid is not “harmonic” during these 20-30 images (they moves in different directions during the whole cardiac cycle), so a function cannot be defined (or is not easy) to fit the trajectory of the nodes’ positions. So, the DEFINE_GEOM macro (prescribes the node position in each time steps by a given function) cannot be used to update each node position but the DEFINE_GRID _MOTION (loading each node position from external file and update the new position) is applicable to update the node positions in each time steps. See the following paper:

http://link.springer.com/article/10.1007/s10439-008-9627-4#page-1 

So, do you have a way to generate all your intermediate geometries?  (I think that is what they did in the paper, right?) If yes, you might be able to use a single "block representation" in ICEM CFD and generate mesh for all of your geometries at least semi-automatically. And then you can try what I suggested in my last post.

>Soroush

Attached is a figure that shows where you can define events for reading the new mesh and interpolating the results from the previous time step: If you can find a way to generate your meshes for all time-steps, the problem is more or less solved.

Yes I know that, but because I have about 1800 different time steps and geometries (30 MRI images and 60 intermediate images) It is very time-consuming and cumbersome to define it one by one. At first I will try to do it by using the UDF and then if I notice that it is difficult, I will try it manually as you are saying. Anyway, I will keep you in posted. Thank you very much my old classmate for your help and consulting.

You're welcome!

Just to make my point more clear, if you have 1800 .msh file, you don't need to define events one by one. You can write a journal file for that. But you probably meant creating and meshing geometries one by one is time consuming, right?

Yes Soroush. Reconstructing the geometries one by one and then meshing is time consuming. I have not reconstructed geometries/meshes yet. I just generate points in each time steps and looking do that automatically (reconstructing the geometry by loading the node position each time-steps and then using the remeshing features of the FLUENT).

Hi Siamak, I'm trying to do exactly what you wanted to do here. I've reconstructed my meshes and generated the node positions for each time-step, I'm stuck at writing the UDF to update the mesh at each timestep. Just wondering if you've made any progress since your last post and if you're happy to point me in the right direction? thanks!

Hi Jason, the overall idea is exporting the X, Y, and Z position of each node located on the deforming boundaries in separate files each time step, and then, recalling them and updating the new position by DEFINE_GRID_MOTION micro. All procedure, including the UDF, exporting the mesh position, and ... highly depend on your case. You maybe need to develop a separate subroutine to define/export the mesh positions each time step before simulation.

Regards, Siamak

Hi Siamak,

the method you describe would be very useful for me. My problem would even be more easy. I have a harmonic changing geometry but I don’t have a approach to automatically write the mesh files for each time step. Is there a python library available for meshing purposes and mesh translation to the fluent format? Or do you have another suggestion for creating the mesh (Fortran, C).

Thanks Stefan

Hello Siamak N Doost and Soroush Heidari Pahlavian

Is there a way to delete certain part of the computational domain by an iso-surface in Fluent?

Thanks & Regards,

Vidyadhar

Sir, I have met some questions just like you, now I have 20 vascular models at different time points in one heart cycle. And I want to use udf to solve the moving boundary condition. May I have your suggestions?

Dear Siamak N Doost , Sir, I'm really interested in what you have done, and now I can get coordinates at different time steps by using MATLAB to interpolate points.

But I'm confused when I want to update mesh in fluent at differents time steps, there are some points move but others not. As shown in my .gif file, I use the macro "DEFINE_GRID_MOTION" to update coordinates, and the main code I use is shown as below:

SET_DEFORMING_THREAD_FLAG(THREAD_T0(tf));

begin_f_loop(f,tf)

{

f_node_loop(f,tf,n)

{

v = F_NODE(f,tf,n);

if(NODE_POS_NEED_UPDATE(v))

{

for(ti=0;ti