2D selective mesh generation
I have modelled a 2D circuit breaker in CFD ACE and imported the IGES file into the design modeler. I had to repair some parts that have been curvy in CFD. I had to make some assumptions and approximations in design modeler.
Now that I am done with the modeling, I want to mesh it. The breaker has 63 faces and I intend to mesh each face selectively. When I select a face and define the size of the element as 0.1 or 0.5, the mesh generator shows the following error or warning - 'A size control has a size defined which is smaller than the global min size. This may cause conflicts during assembly meshing and the global minimum size may be used rather than the size defined on the mesh control. In addition the tessellation tolerance might need to be adjusted based on the small scoped min size.' I was working on CFD ACE where I didn't come across such a problem while meshing each face.
It would be great if someone could help me out on this.
I can only reply with my experience in Gambit and Fluent.
Basically you don't need to set interior edges or "outside" edges. They should be set automatically as interior or wall.
For better understanding please display a sketch of your model
Please find the attachements.
I started it this way--
I have created 3 parts:
1. Static fluid
2. Static solids
3. Moving fluid - the main elements are moving fluid and deforming fluid.
This was done with an intention of getting a conformal meshing.
(Especially between the moving fluid section and the deforming fluid section. initially I included the deforming fluid section in static fluid part, but I got pretty weird results where the moving fluid moved irrespective of the othe parts. I could not get deformation / dynamic meshing.) this is depicted in the picture 'mesh movement - no reconstruction or remeshing'
After I have included the deforming fluid part in the moving fluid part in the geometry, I could get a conformal meshing.
Creating named selections seemed to be the toughest and I had to revisit this section for a minimum of 20 times. I named the out line as walls; fluent was intelligent enough to accept them as walls. I named the outline of the moving part as ' moving walls'.
Those zones that had to act as interiors as interiors instead of intefaces. Those walls that had to deform as 'Walls deforming' and some as stationary walls.
Ansys meshing generated some contact regions. I proceeded to fluent.
The following are my course of action till date. I have been stuck with this for the past 5 days.
1. I initially though deforming the walls and reconstruction of the mesh would happen by moving the fluid in the cell zone ' moving fluid' -- the result has been attached. The part moved but it didn't lead to compression or relayering. Fluent created some void space instead. I had to compress the mesh near the cylinder but the result in this case was mesh moving over another mesh without disturbing the mesh it was to distrub (Cylinder)
2. I removed the interfaces between the deforming zone and the moving zone and remeshed (conformal) to see if there is any disturbance near the cylinder section. No more interfaces between the deforming part and the moving part. Initially I didn't move the fluid zone in the cell zone section. Instead, I passed once a velocity profile and once constant velocity to the moving walls around the moving fluid section. The walls didn't move at all.
3. This time I prescribed a constant velocity to both the moving fluid and the moving walls. I got a negative cell volume message. Before 'previewing the mesh', I set the dynamic zones as well. The walls around the moving fluid as rigid body and the walls around the deforming fluid as deforming.
I am ignorant about dynamic meshing and I couldn't find tutorials suitable for the utility. Please contact me in case of any clarifications on the model geometry or the physics of this. My main aim is to move the 'moving part with out any desjoining of the mesh and calculate the pressure output'
How many moving parts do you have?
Post a sketch with different colors for seing what will move, etc...
If you have more than one moving parts, I will start and focus on just one untill it works, then add another moving part.
Layering is tricky, here is a tutorial: https://www.sharcnet.ca/Software/Flu...tg/node178.htm
I have two moving parts. One part is the moving fluid, that moves immediately the command 'preview meshmotion' is activated (please find the moving liquid attachement); the other one is the movement with delay part- this moves after sometime.
I have one doubt max - While dealing with dynamic meshing, do I need to specify a velocity profile or constand velocity just in the dynamic meshing window or DM window as well as in the cell zone conditions window -where I have a moving liquid surface body.
one more doubt - In dynamic meshing zones, it is sufficient to specify the walls deforming and the walls rigid body or should I include the surface body objects like fluid moving - rigid body, fluid deforming - deforming?
I hope you understood what I meant.
regarding velocity of motion, you can set it as constant or you can treat it with a profile or with a udf
You can set a surface as rigid body.
But I still not understand your motion. In your picture (First movement.jpg ) do you have a massfllow entering from the right or are you trying to modelize a piston which moves and therefore creates a massflow?
Thank you max for the reply.
please watch this youtube video.
The left part of the video is the right part of my model. The fluid zone in my model is mainly due to the cylinder movement. We can say that this the dynamic zone is due to the mass flow.
Move walls and deform walls
What I understand is that I need to set the moving walls as rigid body and stationary walls as deforming. I am getting negative cell volume problem also.
Anyway u could find the attachment and conclude. please contact me in case of any rectifications..
I f I see your video, then I would treat it in another way.
Check my picture:Attachment 27823
The orange zone will be the layering domain (where mesh topology will change.
The blue zone on the right will be the moving zone, I set it as rigid body, so the whole surface will move (with rigid body: understand no mesh modification).
The edge which separates orange to blue surface has to be set as wall else I don't know how you could generate a flow field due to motion.
Set also this edge as rigid body.
Now you have 2 possibilities:
*you don't set the orange zone as rigid body and the add/suppress layer's process will occure on the left side from "separation line" (you have to set the cell height limit in meshing options)
*you set the orange zone also as rigid body, and the add/suppress layer's process will occure on the right side of the stationnary edge (you have to set the cell height limit in meshing options)
If I talk about right and left side of the edge, it means you have 2 adjacent zones . Both zones have to be separated (call the blue zone moving domain, the orange layering for instance)
So you need to do some splits for setting the layering zone.
PS: I am basing of my memories with fluent 6.3 (I am not usinf fluent anymore); maybe it has changed with new versions, but I think the idea should remain the same
Thank you very much for giving me time on this. Yeah, what you say about the flow field is perfect but kindly have a look at the attached picture. You might understand the full picture. The whole section mentioned above moves to the right and the rectangular solid which has been named a wall should create the flow field. Please correct me if I am wrong.
1. As mentioned by you, if I include a wall between the blue zone and the orange zone, wouldn't I block the flow from right to left?
My try with dynamic zones:
1. I tried to set the walls and the surface body in the blue as rigid body and the walls and the surface on the right as deforming body!! is there something wrong?
I ll try doing what you told by inserting a small wall in between the blue zone and the orange zone and 1 oriface on top and bottom. This is a modification I might need to include and is not there in the real circuit breaker.
my picture has been cutted in some way and you don't see my blue zone I was talking about.
Do you have a cad cross section or whatever?
Thank you very much for the idea of moving the wall from behind. Though it doesn't comöply with the real model, it opened up my mind and I encountered my walls deforming. This has given me some leads to the present status.
I am sorry for I couldn't get back to u on with a model. I have partially solved the problem by choosing the wall that had to be rigid as 'rigid body' and the walls that are to deform as 'deforming'. I have set a time step of 1e-09 and tried to run 100000 timesteps by viewing the mesh motion. The orthogonal quality started reducing from the 81000th step. I have attached some pictures. Can you help me with the dynamic layering settings.
Orthogonal quality before starting the mesh preview motion:
Min OQ - 0.58
Max skewness - 0.688
At 80000th step -
Min OQ - 0.282
if your mesh motion is piloted by layering, I don't understand why you are showing tri elements, since layering is only for quads
I came across a thread which told that spring based smoothing goes better with triangles rather than quads. Anyway I ll change the tris to quads. No where in fluent manual have they written that layering would just go well with quads not with tris. I have 2 more days.
Layering enables the layering mesh update method (valid for a prismatic cell zone only). This item will appear only if the zone you are defining is a cell (fluid) zone.
I remeshed with quads. I can see the orthogonal quality improving with time steps. I hope this is leading me to what I want. Thank u max for helping me. I couldn't have realised if you didn't talk about the prismatic cells.
multiple subdivisions on zone --- and Zone --
Sorry for the inconvinience.
how r you. I am finally through the dynamic meshing.
I have a new problem. When I try to run the calculation, it flags multiple subdivisions on zone --- and Zone -- and AMG solver diverges. These happen to be the stationary walls in the dynamic zone.
I checked on the forum but I could not get the reason for that. What do you think might be the reasons.
I am very close to the solution but the solver should start calculating.
check some fields (velocity / pressure) and see if your stationnary or whatever are well defined
you can also post a picture of your mesh at t=0 , and one when it diverges
|All times are GMT -4. The time now is 08:20.|