[hamidciv]

hi all
i mehed my model with tet mesh and it refined as well, but unfortunately number of cells is very high( number of node is 5 million), now i want used hex mesh , whether exist way for refining hex mesh using of body of influence or sphere of influence ?, i using multizone for hex mesh as shown figure, please help me. how i refined mesh in arbitrary area like tet mesh as shown follow, i want refined mesh in portion that given as red color in figure and remain of figure not useful for me.
thanks in advance

[Kapi]

Hi hamidciv,

Divide your geometry in some parts and pick the part where you need fine mesh and then give Body Sizing on that part.

Sphere of Influence is good when you are not able to pick particular edge/face/body for sizing.

Hope It helps

Cheers
KAPI

[hamidciv]

hi dear kapi, your answer is very clear and direct , very thanks for answer my question
dear kapi , if your possible i have 2 question for you
1-whether divided geometry to the various parts dont create problem in mesh? my mean is Lack of uniformity in mesh(also i apply as from part in geometry)
2- wheteher Despite using hex mesh, we can used of sphere of influence, when i selected sphere of influence (also body of influence is diactive) displayed x sign in beside body sizing and finally dont generated mesh.
thanks in advance
best wishes

[Kapi]

Hi Hamidciv,

whether divided geometry to the various parts dont create problem in mesh?

It dosent create any problem.
Make sure you give interface between the bodies connected.

wheteher Despite using hex mesh, we can used of sphere of influence, when i selected sphere of influence (also body of influence is diactive) displayed x sign in beside body sizing and finally dont generated mesh.

Please create new coordinate center for sphere of influence if thats the problem.
What errors is it displaying?
can you post picture of error?


Cheers
KAPI

[hamidciv]

hi dear kapi , thanks for response
i divide geometry in two parts and do freeze it and finally apply from new part, whether interface in geometry have a problem?
about sphere of influence, i used multizone for hex mesh,As soon as i selected sphere of influence in body sizing , appear x sign in side it and finally Blue box is filled but body sizing not worked.
best wishes
hamidciv

[Kapi]

Hi hamidciv,

i divide geometry in two parts and do freeze it and finally apply from new part, whether interface in geometry have a problem?

Please make sure in detailed view of your geometry, "Shared Topology Method is on Imprints. This will make sure you have imprint of 1 surface on other. To check click on the interface or select the interface, it should show 2 faces rather than 1. If its showing 2 faces then there is no problem.

about sphere of influence, i used multizone for hex mesh,As soon as i selected sphere of influence in body sizing , appear x sign in side it and finally Blue box is filled but body sizing not worked.

I think Your Advance function is active which You need to switch off.
Tools>Options>Meshing>>Sizing> Use Advance Size Function - > Off

the trick is that you need to turn off the Advanced Size Function if you are trying to scope sphere of influence to edges and faces.
For body sizing, make sure your Sphere of influence is close to edge or includes edge. Somehow it doesn't do sizing if it doesn't have any edges or faces associated with it.


Hope it helps

Cheers
KAPI

[hamidciv]

hi dear kapi, very thanks for spending time for me

dear kapi unfortunately Everything I do, exist x sign in side of body sizing, my advance size function was Pre-Off, i also checked interface in geometry that is consist of two face, when type is on element size in body sizing, checkmark appeared and when it is on sphere of influence again x sign appeared, i really dont know Where is the problem? i very confused.
thanks a lot
best regards
hamidciv

[hamidciv]

hi every body
As shown above unfortunately my problem still dont solved, i slice geometry in two part,
At first I used body of influence with tet mesh, but number of cells was very high, now i decided used of body of influence that i facing error (display x sign in side body sizing and Not working it ), i attached geometry in zip format.
please guide me and express Any comments about my model for selected better mesh method.
thanks a lot
best regards

[Kapi]

hi dear kapi
my goal is comparing result of numerical modeling with experimental results, i dont exactly What mesh size is good enough for my model, i when used vertical lines for edge and I doingy analysis with this mesh, i stopped my run after of multiple time steps and with regarding define plane of water.volume fraction , my graphical shape was unclear that in my opinion induced of coarse mesh.
dear kapi i used horizontal line in addition vertical lines my number of nodes Was obtained about 6 million, that really my system Do not respond with this value, the problem is when i used edge sizing
The lower part the model that I do not need it also doing mesh.
i dont know really reached one optimum mesh for my model, please advise me.
i attached one image of runing after multiple time steps, in my opinion movement of water is unclear, whether this is induced of coarse mesh?
https://drive.google.com/file/d/0B1T...ew?usp=sharing
thanks a lot for spending time for me
best regards
hamid

Hi Hamidciv,

You have to run your simulation till it reaches steady state then only your solution will give picture of what you have done. Atleast run your simulation till the time you tend to see that its going to converge.
The Picture your shared is of no use cuz you have done very few timestep.
Anyways by the looks of it, mesh isnt as good.
You have to decide if you are happy with the mesh or not.
After meshing you can click on mesh and go to mesh>Statistics>Mesh Metric and see whats your element quality, skewness, aspect ration.... are! this will help you decide if you have obtain a good mesh.
You have to find sensitive areas in your geometry and get good mesh at those locations.
Also have you fixed your geometry yet or not? I showed you that your edges are divided at several places.
Can I suggest you to read about getting good mesh as well, it will help you now and in future.

Cheers
KAPI

[hamidciv]

hi dear kapi
yes i fixed geometry in places divided to several edges and i connected to one edge, i used edge sizing with vertical line and horizontal line, but unfortunately element quality and aspect ratio is not good, how do improve this? as your said and clear with look previous image in runing induced bad mesh in my model, as i previous said when i used tet meshing all mesh metric was good only alone problem i have number of elemets was about 28 million in model and finally Was accompanied by an increase in computation time therefore i used hex mesh instead.
please advise me
thanks a lot

[Kapi]

Hi Hamidciv,

Reduce your elements size in Vertical edges and Increase in your Horizontal edges. Check your mesh, see where you are getting bad aspect ratio and post the picture of the location here.

Cheers
KAPI

[hamidciv]

hi dear kapi
as your mentioned i do increase element size in horizontal lines and decrease its in vertical lines, with do this high affected on aspect ratio improvement and other metrics also is good, but element quality is not good still, i attached image of element quality in model.
thanks a lot

[Kapi]

Hi Hamidciv,

Under Mesh, change Smoothing to High and Span Angle center to Fine.
You can find out if your mesh is good or not by this:

Skewness: 0-0.25 (excellent), 0.25-0.50 (very good), 0.50-0.80 (good), 0.80-0.94 (acceptable), 0.95-0.97 (bad), 0.98-1.00 (unacceptable).

Orthogonal quality: 0-0.001 (unacceptable), 0.001-0.14 (bad), 0.15-0.20 (acceptable), 0.20-0.69 (good), 0.70-0.95 (very good), 0.95-1.00 (excellent)

Element Quality: >0.30(good)

Cheers
KAPI

[hamidciv]

hi dear kapi
with your helps my problem is solved.
thanks very much for all.

[Kapi]

No worries!

Good luck with your project

[hamidciv]

dear kapi

I’m grateful to you for all the things you have done for me.
best regards
hamid