# Fluent dynamic mesh 'remeshing' method for pyramid elements

 Register Blogs Members List Search Today's Posts Mark Forums Read

 March 9, 2010, 03:48 Fluent dynamic mesh 'remeshing' method for pyramid elements #1 Member   Join Date: Sep 2009 Posts: 69 Rep Power: 9 Hi everyone I am working on a hybrid structured/unstructured mesh simulation at the moment with pyramid elements at the interface of both the meshs. My problem is the structured part of the mesh is moving dynamically as a solid body and it is causing the pyramid elements of the unstructured mesh to collapse. I am using both smoothing and remeshing methods. I am only able to preview it up to a certain point and then negative volume was detected. And when I tagged the negative volume for checking, it is always a pyramid element. Is it true that Fluent Dynamic Mesh does not remesh pyramid elements? If so how can I go about it as a pyramid element is the only element that can connect a hexahedral and tri/tetra region together. I am simulating a pitching airfoil by the way and the structured mesh is the boundary layer mesh while the unstructured is the farfield. Thanks for your help Regards, Darren

 March 9, 2010, 04:33 #2 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,149 Rep Power: 32 Remeshing and Smoothing was only available with tetra (on Fluent 6.3) Now I don't know anymore. Your problem, as you described, is that you are moving a hexa-zone (rigid-body) into a tetra zone. But the transition between hexa and tetra is a pyramid. What you ca do: Create a surface surrounding your hexa-volume and split your fairfield volume with this surface. You will have 3 volumes: fairfield - hexa - the new one squeezed between the 2 others. Then delete fairfield mesh, and mesh this new volume with tetra, and the outer surface pointing in fairfield direction has to be meshed with tri. Now remesh the fairfield with tetra Then redefine your rigid body like: hexa + new volume The remeshing should work __________________ In memory of my friend Hervé: CFD engineer & freerider

 March 9, 2010, 06:24 #3 Member   Join Date: Sep 2009 Posts: 69 Rep Power: 9 Hi MAX Thanks for the reply! I will give it a try and see what happens Regards, Darren

 March 14, 2010, 20:26 #4 Member   Join Date: Sep 2009 Posts: 69 Rep Power: 9 Hello mAx, I have tried what you have mentioned. Below is a pic of my mesh as per your suggestion : This is a picture of the side of my extruded airfoil mesh. This is probably not a good picture but what I have done is to define a new unstructured mesh zone right after my structured one and keep this layer as a 'Rigid Body' together with my structured boundary layers so that they move together with my airfoil when it is pitching. While this method is successful in preventing the pyramids from being deformed and only remeshing the unstructured tetra elements on the farfield, my mesh is still collapsing. This time it is in between the interface between pyramid/tetra zone (new zone) and the tetra zone (farfield zone). From what I can see, somehow the tetras on the farfield side of this interface are collapsing (like the roof collapsing on the house) and they are not being remeshed. If this happens, what settings in my Remeshing 'mesh methods' should be tweaked? What I am using so far is just default settings with 'size remesh interval' changed from 5 to 1. I only use 'local cell method' for remeshing method. Also I am actually using smoothing with a '0' spring constant factor, '0.0001' convergence tolerance and 50 iterations. I apologize if the question is trivial as I am very new to dynamic mesh in 3D and I am not very experienced when it comes to tweaking these parameters. Thanks for your help once again Regards, Darren

 March 15, 2010, 02:13 #5 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,149 Rep Power: 32 You can also enforce fluent not remeshing your interface (just set it as internal-BC and affect it the rigid-body motion). I also have never used Remeshing-Smoothing tool, but you will have to handle with parameter's tuning. Check User's guide about remeshing-smoothing __________________ In memory of my friend Hervé: CFD engineer & freerider

April 23, 2010, 09:44
#6
Member

Join Date: Mar 2010
Posts: 65
Rep Power: 8
Quote:
 Originally Posted by -mAx- Remeshing and Smoothing was only available with tetra (on Fluent 6.3) Now I don't know anymore. Your problem, as you described, is that you are moving a hexa-zone (rigid-body) into a tetra zone. But the transition between hexa and tetra is a pyramid. What you ca do: Create a surface surrounding your hexa-volume and split your fairfield volume with this surface. You will have 3 volumes: fairfield - hexa - the new one squeezed between the 2 others. Then delete fairfield mesh, and mesh this new volume with tetra, and the outer surface pointing in fairfield direction has to be meshed with tri. Now remesh the fairfield with tetra Then redefine your rigid body like: hexa + new volume The remeshing should work
hi mAx:
I'm working on IC engine.I met the same problem while meshing the model.
I creat a cylinder and split it with a face,mesh both volume with tet/hybrid TGrid.and the face between red zone and yellow zone interior.then export .msh into fluent.as shown in picture 1.
I define the yellow zone rigid body,red zone and its side deforming,but after mesh motion,I got image as shown in picture 2.
you can see that the mesh between red and small zone doesn't remeshing.
do you have any ideal?thanks
Attached Images
 1.jpg (87.5 KB, 110 views) 2.jpg (104.3 KB, 94 views)

 April 26, 2010, 01:03 #7 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,149 Rep Power: 32 your geometry is quite simple. I would mesh the red domain with hexa, and then handle the dynamic motion with layering. Let the yellow domain as rigid body motion, the lateral side as deforming, and the other red extremity as stationnary. The interface between the 2 domains should also set as rigid body, but in the mesh option panel, you need to give some parameter to the right side (as the interface is common to both domains) __________________ In memory of my friend Hervé: CFD engineer & freerider

April 28, 2010, 20:56
#8
Member

Join Date: Mar 2010
Posts: 65
Rep Power: 8
Quote:
 Originally Posted by -mAx- your geometry is quite simple. I would mesh the red domain with hexa, and then handle the dynamic motion with layering. Let the yellow domain as rigid body motion, the lateral side as deforming, and the other red extremity as stationnary. The interface between the 2 domains should also set as rigid body, but in the mesh option panel, you need to give some parameter to the right side (as the interface is common to both domains)
hi mAx:
another question:in the in-cylinder model,I can mesh the cylinder as you say,in which one is hex while the other is tet.so why do I have to mesh a pyramid zone between then?

 April 29, 2010, 01:03 #9 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,149 Rep Power: 32 if one volume is meshed with tetra, then the interface is already meshed with tri. If you mesh the other AFTER with hexa, then there will be a pyramid layer (transition from tri element to quad element. But is should be meshed automatically. In you case I would mesh bothe volumes with hexa, or you mesh your hexa domain FIRST, and then the other with tetra. It means the pyramid layer will be in the stationnary domain __________________ In memory of my friend Hervé: CFD engineer & freerider

 April 29, 2010, 07:45 #10 Member   李逾 Join Date: Mar 2010 Posts: 65 Rep Power: 8 but I can mesh the two zones seperately,make interface between their adjacent.then import them into fluent to grid interface.so the mesh motion still can be done.... what are the difference between making three zones include transition zone with no transition zone?

 June 27, 2012, 10:41 #11 Member   Satish Gupta Join Date: Jun 2012 Posts: 30 Rep Power: 6 I am trying to model a 2d square cylinder using dynamic mesh.I have divided the mesh into two zones.A circular zone is rotating with the square and the left over mesh is given deforming condition.The problem is only the cells adjacent to rotating portion is deforming and not the other cells in domain which gives me -ve cell volume after some iterations.what should I do to deform the complete domain?

 June 28, 2012, 00:52 #12 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,149 Rep Power: 32 set rigid body motion to your domain __________________ In memory of my friend Hervé: CFD engineer & freerider

 December 16, 2012, 10:26 #13 Member   Vidit Sharma Join Date: Aug 2012 Location: Delhi, India Posts: 32 Rep Power: 6 Hi All.. Sir, I am trying to rotate a 2D box or a 2D cup structure in Fluent using smoothing and remeshing. I am using tri mesh and as mentioned in Fluent Manual I am using smoothing and remeshing and also set the remeshing parameters from mesh info tab given in the remeshing menu. But the problem is that when i start simulation and it goes to first time step Fluent display "Updating mesh at time level N..." and here it stops and it happened alot of time and even waiting after a whole day it didnt worked. I also tried time step size from 0.01 to 0.000001 but it still show this problem. Can you plz help in this case? Thank u in advance

December 11, 2015, 05:38
#14
New Member

Ajith Kumar A
Join Date: Dec 2015
Posts: 1
Rep Power: 0
Hi Max,
I am relatively new to fluent. Having difficulty in remeshing in moving zone for a dynamic mesh problem. The deforming zone is not getting remeshed. The mesh and pressure contours of steady simulation and transient simulations are attached herewith. Can you tell me what am I doing wrong here in the transient simulation?
I would appreciate your help on this.
Thanks and regards,
Ajith
Attached Images
 6DOF1.jpg (54.9 KB, 27 views) 6DOF2_transient.png (39.6 KB, 23 views)

 December 11, 2015, 05:58 #15 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,149 Rep Power: 32 what kind of remeshing are you using? layering/smoothing or layering? check this tutorial for layering __________________ In memory of my friend Hervé: CFD engineer & freerider

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20 Pei-Ying Hsieh (Hsieh) OpenFOAM Running, Solving & CFD 64 June 7, 2012 10:04 weiyang1980 Main CFD Forum 0 September 22, 2009 21:06 SSL FLUENT 2 January 26, 2008 12:55 Althea FLUENT 21 February 6, 2001 08:05

All times are GMT -4. The time now is 12:48.