2.5D Remeshing with Biomedical Application

  • 373 Views
  • Last Post 17 January 2019
RD2016 posted this 14 September 2018

Hey guys,

I'm trying to simulate a contracting left ventricle with a working aortic valve (implemented using 2-way FSI). To cut down on complexity, the simulation is 2D at the moment. I can achieve accurate wall motion, but upon implementing the valve my mesh fails due to negative cell volume. I've implemented the 2.5D remeshing strategy, and hoped that it would maintain mesh quality as the leaflets open up as well as help with issues involving negative cell volume. No such luck, as the mesh does not appear to be actively remeshing.

Here is a list of the parameters I've set/are working with:

  • In the Dynamic Mesh options, Smoothing and Remeshing are enabled.
    •    Under Smoothing, I'm using the Spring/Laplace/Boundary Layer method, as this is what works with 2.5D remeshing (Note for other students: According to the manual, face region remeshing will only work with the Spring/Laplace/Boundary Layer method).
    • The Spring Constant Factor is set to 0.1 (Although this apparently is negligible with iterations>100).
    • The Convergence Tolerance is set to 0.001.
    • The Number of Iterations is set to 100 (I've attempted changing this number, but have not noticed a significant change.
    • The Laplace Node Relaxation is set to 0.5.
    •    Under Remeshing, the only method enabled is 2.5D. The Minimum Length Scale is set to 0.04 mm and the Maximum Length Scale is 0.71 mm (in the Mesh Scale Info, the min and max are 0.044 mm and 0.71 mm, respectively). I know ANSYS recommends setting the min and max scale at 0.4 and 1.4 of their Mesh Scale Info values, respectively, but even after I did that I was not getting good remeshing.
    • The Maximum Skewness is 0.5 (0.53 in the Mesh Scale Info)
  • As this is a 2D case, the "top" and "bottom" of the domain have been set to Symmetry in the Boundary Conditions
  • In the Dynamic Mesh Zones, both leaflets are set to System Coupling, and have Solution Stabilization enabled.
  • The symmetry regions are set to deforming
    •    Under Geometry Definition, the plane definition is used, with appropriate points on each plane set
    • Under the Meshing Options, both have Smoothing enabled, but only one has remeshing enabled (as per instructed by the manual)
    • The Min and Max length scale, and Maximum Skewness are the same as previously described
  • The time step size is 0.0005 s.

The only thing that I can think of at this point is that the issues I'm having is a direct result of the meshing strategy I implemented (Adaptive Sizing used, element size of 0.5 mm, and a Linear Element Order). I can provide more info if need be.

If anyone has any suggestions, I'd love to hear it.

Order By: Standard | Newest | Votes
rwoolhou posted this 17 September 2018

Pictures will help. Common issues are moving the mesh too quickly in one time step and topology clashes. As ANSYS staff we're not able to open solver files so may need the wider community to trouble shoot this. 

RD2016 posted this 18 September 2018

Sure, I can post some pictures.

So this is my fluid domain. As I said before, it is a 2D left ventricle with prescribed motion on the walls. Adaptive meshing was used, and I'm not too sure about the quality of the elements near the leaflets. Here is a close-up of the leaflets (where the negative cell volumes occur). Although ANSYS does not allow for 2D FSI, I'm able to perform this by having my entire domain be only 1 element thick. I've accomplished this by using the sweep method (I'm going into detail here in case any others in the community are curious).So, after a few time steps (that take a very large amount of iterations to converge, possibly due to mesh quality?), the simulation reports that negative cell volumes have been detected. Shown in this image (the green portions along the tips), it does not appear as though the mesh is remeshing...Close-up of the negative cell element.

I have experience with FSI, and I understand that if the mesh moves too quickly, negative cell volumes may occur. My time step, as previously mentioned, is small enough that there really aren't any large deformations within one step, so I don't think that's the issue. Any comments would be appreciated!

RD2016 posted this 18 September 2018

 I apologize for not posting sooner, but the website would not allow me to post these images. I included an image description for each, but it does not look like it is displaying properly. I have added them here.

First image: So, this is my fluid domain. As I said before, it is a 2D left ventricle with prescribed motion on the walls. Adaptive meshign was used, and I'm not too sure about the quality of the elements near the leaflets. 

Second image: Here is a close-up of the leaflets (where the negative cell volumes occur).

Third image (left): Although ANSYS does not allow for 2D FSI, I'm able to perform this by having my entire domain be only 1 element thick. I've accomplished this by using the sweep method (I'm going into detail here in case any others in the community are curious).

Fourth image (right): So, after a few time steps (that take a very large amount of iterations to converge, possibly due to mesh quality?), the simulation reports that negative cell volumes have been detected. Shown in this image (the green portions along the tips), it does not appear as though the mesh is remeshing...

Fifth image: Close-up of the negative cell element.

RD2016 posted this 18 September 2018

So, quick update; I split my fluid domain into two different regions encompassing the ventricle and leaflets, respectively. The region around the leaflets was meshed using a uniform mesh and a really fine resolution. I had read elsewhere that doing this allowed me to control the remeshing properties directly in the region of interest. However, this did not initiate remeshing, and negative cell volumes still occurred at the same regions shown in the photos above. If anyone has anything else for me to try, I’d be eager to do it.

Kremella posted this 19 September 2018

Hello,

When you first started, what was your mesh quality like? Skewness and orthogonal quality?

Best Regards,

Karthik

RD2016 posted this 19 September 2018

Hi,

When I first started, the mesh quality was pretty good. The skewness in the leaflet region was 0.3975859, and the minimum orthogonal quality was 5.35187e-01.Unfortunately, I decided to run another test case, and did not save my previous case files when the failures occurred. I'll try to see if I have them in another location, but the skewness values were close to what I just described.

In the manual, it says that 2.5D remeshing will assume rigid body motion is applied to the moving face zone. As this is an FSI study, could that be a potential reason for failure?

RD.

anmehta posted this 20 September 2018

Hello ,

 You can follow some steps of oscillating plate tutorial of fluent two way FSI where we use 2.5 D remeshing concept and also smoothing .Initial few deformation of structure will be mostly handled by smoothing operation as deformation values will be small . 

1)I hope you have set the remeshing criterias (a good starting point for length scales are 0.4Lmin and 1.4 Lmax values  and max skewness can be kept at 0.7 if initial value is 0.397 ) .

2) Care must be taken on symmetry planes for defining the dynamic mesh so that we will not have any warpage (out of plane deformation of tet ) . These could be the cause of failure if no constrain has been specified . All nodes must move in planar direction 

Planar deforming on sym 1 Remeshing and smoothing operation setting on sym 2 . Only one face needs to set with remeshing other surface will follow same in 2.5D remeshing

Planar deforming needs to set on one sym surface (kindly set values for plane as per your case) and remeshing settings needs to be set on another sym surface (2.5 D remeshing concept)

 

Regards

RD2016 posted this 20 September 2018

Thanks for the info. It seemed like a lot of that was from various tutorials (such as the 2.5D remeshing tutorial found in the Fluent Dynamic Mesh workshop, and oscillating plate FSI tutorial), which did assist in the initial setup of the simulation. However, as previously stated in my original post, I have already done what you suggested and the fluid domain did not remesh.

There is no out of plane deformation of the elements (which, according to the manual, can only be wedge cells when using 2.5D remeshing, not tetrahedral). The current issue is that Fluent does not seem to be remeshing the elements according to the specified min and max length scale I set.

I am wondering if this could be due to the settings I set for the Spring Diffusion method. Perhaps with the number of iterations set so high, and Laplacian smoothing set so low, Fluent is capable of generating a mesh that still satisfies the desired equations (located in 10.6.2 of the manual). It's worth a shot, I guess. If anyone has any other ideas, let me know. I'll provide updates as I get them.

Tayyaba posted this 10 October 2018

hi, did you solve your problem? as I am also solving a 2.5D problem using 2-way-FSI. I am solving a laminar test for an elastic flap but unfortunately I am unable to get into simulation because  I encounter the following error even at start of simulation:

"(DP 0) Element 195 located in Body "fea" (and maybe other elements) has become highly distorted.  You may select the offending object and/or geometry via RMB on this warning in the Messages window.  Excessive distortion of elements is usually a symptom indicating the need for corrective action elsewhere.  Try incrementing the load more slowly (increase the number of substeps or decrease the time step size).  You may need to improve your mesh to obtain elements with better aspect ratios.  Also consider the behavior of materials, contact pairs, and/or constraint equations.  If this message appears in the first iteration of first substep, be sure to perform element shape checking. Named Selections for the offending element can be created via the Identify Element Violations property on the Solution Information Object."

could you please suggest me anything regarding this? my transient structural case runs well separately  but when I couple it with Fluent this error comes.Some times I also get an error regarding 'Neg. cell volume detected'

Moreover I am also confused about the Min and Max length scale under remeshing setting, is it exactly the same as the mesh scale info?because the tutorial I have seen, it is different and I do not know the reason behind that. Also do you know how to set 'Point to plane, and Plane normal' in 'Geometry' setting when a 'Deforming' zone is selected?

Waiting..

RD2016 posted this 22 October 2018

Well, I kind of solved my problem. I basically had a misunderstanding of what the "Minimum" and "Maximum" length scales physically represented in the simulation. For reference, I believe they refer to the minimum and maximum size the "leg" of the triangular surface can actually be before it starts to remesh. I can try and elaborate, if need be.

As to your problem, oh boy. It's a simple fix, but requires a very in-depth answer, and the understanding that FSI is not simple. So, the reason you are getting the mechanical error is essentially due to your mesh moving too quickly, or oscillating too much in a particular time step. This could be due to a variety of things, ranging from how you set the simulation up (if you have no force one time step, and then max force another time step), to the basics of your simulation (how large your time step is, mesh size, etc.). Unfortunately, I'm pretty confident that it is neither of those things.

This is going to be very difficult to explain, but try to keep with me. So Fluent will run through its calculations, and then send over force information to Mechanical. Mechanical will then take these force calculations, and then move the geometry accordingly. This is the basis of system coupling, and we all know this. What happens next, however, is where it gets tricky. Mechanical will then send this displacement data back to Fluent, and Fluent will respond by moving the mesh. The problem comes into play when Fluent begins to run its calculations again. As the surface has moved, this will create either a higher pressure or lower pressure area in the location that the object was once in. Not to worry, Fluent can handle this, and it will finish its calculations and solve accordingly. This loop will continue on until 1.) Fluent has converged, 2.) Mechanical has converged and 3.) system coupler has converged.

So, think about this for a minute: what happens if the movement of the mesh is just a bit too much? Easy. Fluent overcompensates and sends over a pressure that is slightly larger than last time. This causes Mechanical to move the geometry more than last time, which causes Fluent to overcompensate, and on and on and on...Starting to see the problem yet? Good.

This is what's causing your crashes. The movement of your mesh is oscillating out of control, and your simulation is failing. To fix this, you need to implement "Solution Stabilization" in the dynamic meshing tab. Download the dynamic mesh tutorial from ANSYS, as well as the system coupling tutorials and materials to get you started. Also, check out CFD-online for any info related to "Solution Stabilization". Only use this for regions that are linked to system coupling. But, you also need to see how your surfaces are failing. I recommend adding in a Surface Monitor under Report Definitions. Take the integral of static pressure over one surface you are interested in (what you have your system coupling set to).

I think this is the most I can answer at the moment. Good luck, and I hope it works out!

  • Liked by
  • Kremella
Tayyaba posted this 25 October 2018

Thank you very much for your detailed reply, Any how I have tried this too but still getting the same error. should i also have to set the 'Stabilization' in 'Analysis settings' of the transient structure?

Regards

Tayyaba

Tayyaba posted this 25 October 2018

Thank you very much for your detailed reply, Any how I have tried this too but still getting the same error. should i also have to set the 'Stabilization' in 'Analysis settings' of the transient structure?

Regards

Tayyaba

RD2016 posted this 25 October 2018

Without an intimate knowledge of your setup, I don't think anyone could really tell you specifics on what to do. That's not meant as a discouragement, just that could tell you to do something that is potentially very wrong for your situation. As far as your errors are concerned, check your solution monitor plots and see if your integral of pressure (surface monitor) on your system coupling surface is converged (if it looks like its oscillating out of control, try increasing your solution stabilization). Using stabilization in Mechanical is an option, but have you read what it does on the manual? More importantly, do you know how it will affect your simulation, and if the output is close to what is "right" in real life? We can change things, and poke and prod them to make it work, but if it doesn't resemble the case you are trying to model, then it's wrong.

I hope this helps.

destroy posted this 26 December 2018

Hey RD2016,

 

I am trying to simulate 2.5D FSI of aortic valve blood flow.

The structural results depends among others on the Young modulus, Poisson ratio the mass of the valve

the mass of the valve is dependent on the material density and the thickness extruded in the normal direction

So, how did you choose this thickness? Should I create as thick extrude, as the mass will be equal as the 3D model?

 

Regards

Destroy

 

RD2016 posted this 29 December 2018

Hey destroy,

Good question. For future reference, however, please don't tack on another question that has little to do with the original one. It creates a long chain that can become very confusing and full of differing topics (if you need an example of this, check out cfd-online). A much better alternative would either be to email the person directly. If they don't have an acceptable answer, or there is no person who originally asked a question, you can post your question to the forum and see if there's anyone that can help. I'll answer this one here, but please try and continue the conversation with me directly.

Unfortunately, I don't have a good answer for you. Beyond ensuring that you are using the "symmetry" option in Mechanical and keeping only one element in the normal direction, I'm not sure what a "good" thickness would be. The main reason for this is that since you and I are both using a 2D model to simulate a complex 3D phenomenon, there will undoubtedly be incorrect results in our simulations that are present due to the simplifications we had to make. Think of it this way; if you make your thickness such that the mass of your 2D leaflets will be equal to the mass of your 3D leaflets, you will be representing a case that does not exist. You take your 2D geometry from the mid-section of your 3D geometry (a slice, if you will). This means that the mass of your 2D geometry will actually be less than your 3D geometry. How much less? Well, that depends on the thickness of the slice you decide to take. I'd recommend the thickness to be one element (whatever you define as your element) thick. That way, it more-closely resembles the slice you took. Beyond that, you're going to need to defend whatever decision you make based on the physical properties, and how the solvers will interpret them.

I'd love to talk about your setup and compare notes, however.

  • Liked by
  • destroy
destroy posted this 29 December 2018

Hey RD2016,

Thank you very much for the answer. Unfortunately I can't find your email adress or another opportunity to write a private message, so I will contunue discussion here.

Im writing to continue discussion started here: https://studentcommunity.ansys.com/thread/2-5d-remeshing-with-biomedical-application/

 

Im not sure if I understood you well, so I will try to describe my problem more precisely;

 

 

I inserted a picture of the 3D geometry.

I want to create 2D FSI analysis of the blood flow, where the valve leaflets only rotate (they are rigid). So the motion of the fluid create forces that make the valve move (rotate). This could be done using 6DOF solver in Fluent, but I want to compare results with the coupling Fluent+Mechanical.

 

To create the 2D analysis, I draw the longitudinal section of the valve, sth like that

(please dont consider here the mesh, only geometry).

For the FSI (coupling) analysis, as I understood from the Hyperelastic flap tutorial, I have to create 2.5D analysis so I simply extrude this geometry in the "z" direction (normal direction). Of course the mesh will be one element thick.

The only question is: does the thickness of the extrusion influence on the results? If yes, how to choose the appropriate thickness? Furthermore, I don't clearly understand the 2.5D ideology, but I know that if the mechanical will be 2D, you have to choose 1 of 3 options (plane stress-zero stress in the 3rd direction, plane strain - zero strain in 3rd direction, or axisymmetric). If you have 2.5D it is not required.

 

Thank you in advance for the answer

 

Regards

Destroy

RD2016 posted this 02 January 2019

I apologize for telling you to reply via private method. I honestly did not know that function was nonexistent on this forum, and am actually pretty shocked that the developers decided not to include it. I usually write on https://www.cfd-online.com/, so anything outside that is a little new for me. But hey, this site has badges, apparently, so at least you can get rewarded.

Okay, now I'm going to begin tackling your questions. Thank you very much for the detailed description, you seriously have no idea how crucial that is. Now that I have a better understanding of your problem, the solution isn't going to be satisfying. Does the thickness influence the results? Sure it does. By how much? I have no clue. As you increase the thickness, your fluid solution should essentially remain unchanged, provided it is only one cell thick. However, this increased thickness will increase the mass within Mechanical, altering your calculations. You asked if you should extrude the thickness in such a way as to mimic the overall mass of the leaflet, and I don't think that is a good idea. You are looking at a cross-sectional area of the leaflet that has near-zero thickness and mass. Obviously, to use FSI, it has to be 3D, so some extrusion must occur. If you were to extrude such that the thickness is representative of the mass of the leaflet, you would end up with something similar to this:

where the red arrow is the 2D flow field, the grey semi-circle is your actual mechanical leaflet, and the blue box is the 2D cross-sectional equivalent extruded out to match the mass. Remember that Fluent will calculate all quantities with respect to the cell center, so it doesn't matter how large the cell is there. While this might not seem like a big deal, think of it this way:

your flow field is now acting on a portion of the leaflet that is exponentially larger than what it actually should be. This will produce incorrect results that I will not model the actual behavior, in my opinion (Note: I am only using my best judgement at this point).

I believe a much better approach would be to make the extruded thickness such that it is representative of the mass in that given location, while still maintaining correct spatial relations. Observe the following image.

In this image, the extrusion is large compared to the 2D flow field, but small enough to mitigate any errors associated with it.

Now, this is where trial-and-error comes into play; how large should this extrusion be? The answer to that question is simply; large enough that the 2D simulation matches the 3D behavior. Matching certain quantities (such as opening angle w.r.t., or maybe even peak velocity at varying time points) with either experimental data (particle image velocimetry (PIV) is really respected) or in vivo data (PC-MRI, echo if you have high-enough resolution, etc.) will help validate your setup, and allow you to prove that the more complicated results taken from your simulation (vortices, wall shear stress, etc.) are correct. There really isn't a black-and-white answer to your question. You simply have to prove that what you chose to do is good enough based off of other sources.

On to your second question, I'm afraid I don't quite understand what you are asking. But, more to the point, the setting you should use in Mechanical is simply "symmetry". To do this, start in Mechanical. Right click on the Model header in the tree, and select "Symmetry". This will add "Symmetry" to the tree. Then, it's as easy as adding a new symmetric region (the top and bottom of your leaflet cross-section), and specifying where the normal direction is. The model should now only being able to move and flex in two directions.

 

  • Liked by
  • destroy
destroy posted this 08 January 2019

Thank you @RD2016 for the answer

 

However, I am pretty sure now that the thickness extruded in the normal direction does not influence on the result, both on the fluid and solid side.

I performed a simulation of the hyperelastic flap (ANSYS tutorial), where I used 4 thicknesses: original, 2x original, 10x original and 20x original.

I was tracking and comparing the average pressure on the flap and it doesn't differ. Furthermore, the course of the flap deformation is equal every time.

 

I was thinking about it a lot. And I have the conclusion:

- Fluent transmits the force based, among others (mainly) on the pressure, it is equal let's say F=p*S (F-force, p-pressure, S-area)

So if you magnify the area twice (by extruding twice greater thickness) the force is two times higher. BUT - this force works on the flap area that is two times greater too. So thus it does not matter.

 

However - I have the new problem.

This is the problem that you were asking in this topic - remeshing 2.5D.

Im not sure what means the minimum and maximum size.

In the hyperelastic flap tutorial (and another one case, not aortic valve, that I succesfully performed) the minimum defined size is greater than min size in the mesh info; and the maximum defined size is lower than the one in the mesh info dialog box.

I dont know how to choose the min and max size for any case, what are the rules
In the current case that im working I cant find the appropriate values

Could you give me some advices on that point?

 

Regards

Destroy

RD2016 posted this 10 January 2019

I'll try to do my best.

So, let's say that you have a surface mesh that are full of triangular cells. In 2.5D, these cells would actually be "wedge cells", but I'm only concerned with the face remeshing (read through what anmehta wrote on how to set up remeshing). The typical triangular cell looks something like this:

When you look at your mesh info under the dynamic meshing tab, you'll notice that the max and min length scales are reported as being 3 mm and 1 mm, respectively. This isn't a lot to go off of, but if you actually take the time to measure your cells, you'll see that these values area actually reporting the max and min size of the legs of the triangle, like so:

So, this gives us some much-needed info! Now we can relate what the quantity is referring to with something more visual. Now, what about the length scales in the remeshing tab? It's actually pretty straightforward, and horribly confusing all at the same time. Let's say that, in remeshing, you have your min and max length scales set to 1 mm and 3 mm, respectively. What this means is that Fluent will not remesh your domain unless the legs of the triangle fall out of this range. Visually, imagine that your mesh is being compressed in a certain area. The legs of the triangle, as shown below, are slowly being compressed. Remeshing, however, does not occur until the length of one of the legs is below the specified min scale.

Once it is, Fluent will then merge this cell with an adjacent one, smooth the grid a little, and interpolate the results from the two smaller cells into the newly-created larger one. The process by which the max length scale is reached is similar as well. Let's say that your mesh is being stretched. The cell will not remesh until the max length is exceeded.

When this happens, it will divide one cell into two, and interpolate the results. I strongly recommend you read through the manual on dynamic meshing to have a better understanding of what's occurring here.

If you remember, I said that this was simple, and difficult at that same time. The way I've described it seems easy enough, but you need to remember that your mesh is nothing like this. If it is non-uniform, if you have inflation, if you adjusted for curvature, if your cells are not all exactly the same, this is really difficult. In most instances, the min and max length scales will refer to the smallest and largest legs, respectively. If you set your remeshing parameters up based on this, you will get negative cell volumes from cells that are nowhere near close to these minute values. This is why the tutorial actually set values lower than the max, and higher than the min; it was mitigating these potential issues.

Fluent recommends setting the max and min length scales to 1.4 and 0.4 of the reported max and min, respectively. This, however, is contrary to what I just described. Unfortunately, you have to just play around with the values a bit, and determine what the correct parameters are based off of your individual mesh. Let me say this again, FSI is not simple. You cannot perform simulations by simply being "good" at Fluent. You must have a deep understanding of Fluent, Dynamic Meshing, System Coupling, and Mechanical as well as an intimate knowledge of your setup. Even then, you will get errors. Your simulation will fail. You will have a bad time. But stay with it, read whatever you can, and really try to understand what the program is doing, and you'll come out with a truly awesome model.

On a side note, could you post the hyperelastic flap tutorial here? I'd like to play around with it.

destroy posted this 13 January 2019

Thank you @RD2016, your post seems to me to be very useful, you described this question very detailed, I will read the manual and presentations too.

 

As I checked, the dynamic mesh operation depends very much on the set min and max size, the cell size range and the time step size

My conclusions are, the better dyn mesh work, and the smaller probability of the negative cell volume, if you have quite uniform mesh (as you already wrote), and the small time step size

My next exploring will be to check, if the zone remeshing is possible, using 2.5D remeshing. If so, the mesh generated by remeshing and smoothing will be more uniform - the effect of much compression and stretching will be diminished. Furhermore, it will be useful to set the dynamic time step size - there is UDF for it, but im pretty sure that it won't work with system coupling, because the time step size is being set in System Coupling Application. So, I think that the only way to do it will be stopping the calculations, changing the time step size and reactivating the calculation (this is possible as I checked, but very cumbersome). 
I have to read about (and do some tests) on the sizing function in the remeshing tab - maybe it works as ANSYS Meshing curvarture (or proximity and curvarture) mode, and maybe will help with the non-uniform cell sizes.

 

One of the very important reasons of my problems, are the non-uniform speed of detofmation (i.e., the speed of mesh working). This is the reason why I would like to use dynamic time step size.

 

 

According to your question, of course I can send you the data for the hyperelastic flap tutorial, but please tell me how to do it (give some email adress or tell me how to insert files in post)

 

 

RD2016 posted this 13 January 2019

I'd try to add it to like a dropbox or google drive, and then share the link here.

destroy posted this 14 January 2019

Well, Im a little confused, because Im not sure if it is allowable to share these files

They are accessible in the Customer Portal, so - it is for the customers and not available on the Internet, and if you buy the ansys license (or you are the PhD student and your University has it done) you can register and download them on your own

 

The ANSYS Staff should tell if it could be shared here

rwoolhou posted this 14 January 2019

By all means share the link to the ANSYS Portal: this then assumes that destroy or supervisor can access the Portal due to having software. If the material is accessed via the Help then that is available to anyone with a valid install of R19.x and beyond, including the student version. 

We are looking at expanding what can be shared on here but at present staff are restricted to "public domain" information due to export laws and restrictions. 

destroy posted this 14 January 2019

@RD2016 as @rwoolhou said, it is now allowed to upload these kind of files (if I understood)

But you can download them, as I did, from the Customer Portal (search for the hyperelastic flap)

RD2016 posted this 14 January 2019

Totally fine, I wouldn't want anyone to get in trouble over something I suggested. However, whenever I tried to look up the hyperelastic flap tutorial you referenced on the customer portal, all I could find was this (2-way FSI with overset example (hyperelastic flap)) which, at this point, I'm assuming is what you are referencing.



yk2359 posted this 15 January 2019

Hello RD2016,

Sorry about the irrelevant post I couldn't find another way to contact you. I am working on a two-way fsi problem of blood flow in arterial vessels. I have a few questions to discuss. It would help me a lot if you could share your CFD Online user contact info so that I can reach you over a private message. Please let me know if you are comfortable with that or want me to post questions here. 

Thank you,

YK

 

RD2016 posted this 15 January 2019

Sure dude,

My CFD Online account is RaiderDoctor. Hit me up!

  • Liked by
  • yk2359
yk2359 posted this 17 January 2019

Sent!

Close