CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Blocking difficulties (http://www.cfd-online.com/Forums/ansys-meshing/108311-blocking-difficulties.html)

CFD_SIM October 19, 2012 05:38

Blocking difficulties
 
1 Attachment(s)
Hello!

I hope that i can find some help here, because i just can't get my blocking right. I have worked for 1 year with icem, but i mostly did unstructerd meshing and some easy structured meshs.

I have to mesh a pipe with 2 Ribs (at the Outlet) in it. I cut the geometry, so that i have just a quater of it. I thought that this would make things easier, because i can mirror the blocking when i have blocked and meshed it.

I made a hole Block around my pipe and after that i started cutting so that i would get an L-Block (after the mirroring i should get as an result my o-grid). Well, after that i did the necessary associations and well after all that i got a mesh that looks just terrible!

The Mesh around my half-rib is all right, but the mesh around the other surfaces (Top, Down an the quater boundary surface) are just not fitting right. Am i right that i just have to get a mesh around those surfaces? Because when i mirror it there will be a closed volume in the end. (At least so i hope^^)


I hope that someone of you can look at my blocking and give me some hints.

Best regards
John

BrolY October 19, 2012 10:23

- your geometry is not closed, so the premesh won't work propelly because the volume is "open".
- you have to associate all the edges at the top and the bottom of your geometry to improve the mesh.

You could rotate the blocking also, but I really don't like this way because it messes up the association (with ICEM 12.1).
So here is another method :
you should first closed your geometry with interfaces, do the association, generate your premesh, and convert the premesh into unstructured mesh.
Then you can rotate your mesh, merge nodes at the interface and delete those interfaces to have your full volume mesh.

EDIT : I took a lot at your blocking, and if you want to keep the geometry of the RIB, you should redo your blocking because of the angles of the geometry.
If you could simplify your geometry by changing the circular shpa eof the RIB to a rectangular shape, it would help a lot ;)

energy382 October 19, 2012 11:41

Quote:

Originally Posted by BrolY (Post 387518)
- your geometry is not closed, so the premesh won't work propelly because the volume is "open".
- you have to associate all the edges at the top and the bottom of your geometry to improve the mesh.

You could rotate the blocking also, but I really don't like this way because it messes up the association (with ICEM 12.1).
So here is another method :
you should first closed your geometry with interfaces, do the association, generate your premesh, and convert the premesh into unstructured mesh.
Then you can rotate your mesh, merge nodes at the interface and delete those interfaces to have your full volume mesh.

EDIT : I took a lot at your blocking, and if you want to keep the geometry of the RIB, you should redo your blocking because of the angles of the geometry.
If you could simplify your geometry by changing the circular shpa eof the RIB to a rectangular shape, it would help a lot ;)


yeah, shape of rib is really tough. you need several o-grids to capture the geometry.

be careful....your model has no rotational periodicity, only symmetry. so you've to mesh half pipe instead of quarter pipe and create a surface (symmetry plane).

then use a c-grid, do at least two splits in front and behind rib, insert o-grid (around rib) and do another o-grid to capture the edge fillet.

as alexander said, things would be much easier without that edge fillet!

CFD_SIM October 19, 2012 11:45

Hi BroIY,

thanks for your answer.

I tried to block the hole pipe, but the result was not better! :(
I have seen a lot of meshs that were made like i tried to do, and they did not have a closed volume. Maybe this is with ICEM 14.0 something different (don't know, because i only worked with 13 and 14)

I can post my blocking with the hole geometry on monday...but it actually looked much worse than this. Maybe because iam not that good with the hole blocking. When I try to build a smaller block on the bottom and then translate it up to the top the result is a similar mesh like uploaded. If i make a hole 3D block and split it afterwards the result is not good either.

And iam very sorry, but there is no possibility to change my geometrie. I have to mesh it like this :( (nothing that i like, but something that i have to live with :-) )

CFD_SIM October 19, 2012 12:01

Quote:

Originally Posted by energy382 (Post 387528)
yeah, shape of rib is really tough. you need several o-grids to capture the geometry.

be careful....your model has no rotational periodicity, only symmetry. so you've to mesh half pipe instead of quarter pipe and create a surface (symmetry plane).

then use a c-grid, do at least two splits in front and behind rib, insert o-grid (around rib) and do another o-grid to capture the edge fillet.

as alexander said, things would be much easier without that edge fillet!

That sounds really comforting :-D. But i will try the idea with the half pipe and try to insert some c- and o-grids. Hopefully i will have an result in the next week. This part should be the easiest of all :-D...but i guess i was wrong.

I will talk with my adviser about the edge fillet but i don't think that there are gonna be changes.
When it do not have any result by end of next week i think i will switch to unstructered mesh and hope that my quality will be all right.

diamondx October 19, 2012 13:53

hey there,
as everybody says, those edges are difficult to tackle, i had some free time this morning to try something:

https://dl.dropbox.com/u/35161486/cfdsim.png

black arrow indicates change that has to be done to get a good quality:

https://dl.dropbox.com/u/35161486/cfdsim2.png

i have attached the blocking file, so you can have an idea, i didn't take a look at your blocking, may be that what you did at first sight, sorry if that's the case... When i have a large geometry like yours, so i can focus on the rib only i erase everything else, nothing that the rest is easy and extrude can expand my blocking. it's not always the case

https://dl.dropbox.com/u/35161486/Quaterpipe.zip

CFD_SIM October 19, 2012 14:24

Thank you very much Diamondx!

Iam not sure, but i tried to get a blocking like yours. Unfortunately i had al lot of problems with the mesh :(.

I looked at your blocking and it seems pretty good...sad that i could not get to that point. I hope that i can transform it down to the bottom, but this should not be that big of a problem.

Thanks again and i hope that thats it with this part :-).

greetings
John

Far October 19, 2012 14:39

Here is my first try. Mim angle is 9 deg and I must think another smart topology:. Thinking........;)

http://imageshack.us/a/img833/435/quarterpipe1.png

http://imageshack.us/a/img607/5184/quarterpipe2.png

http://imageshack.us/a/img197/4949/quarterpipe3.png

PS: I am going to work on topologies/geometries to whom I have promised.

CFD_SIM October 21, 2012 03:20

Hey Far!

Your Blocking looks great too. Would you mind uploading your Blocking so that i can have a better look at it.

Thanks

John

Far October 21, 2012 03:31

I tried to attach blocking in previous post, but didn't finish because the file size 133 K exceeds the limit of 97K. Now files are shared through dropbox.


https://dl.dropbox.com/u/68746918/Qu...initialtry.zip

CFD_SIM October 21, 2012 05:10

Great. Thank you!

Far October 21, 2012 05:50

This post may be helpful to you. Simon is mentioning the that min angle 9 may be OK for Fluent. But you should confirm it. http://www.cfd-online.com/Forums/ans...tml#post262543


Quote:

Originally Posted by PSYMN (Post 261943)
I can't really see these elements in this pic, but I can see that they are the trailing edge wedges, both within the solid and the fluid.

First off, you can ignore the poor quality solid elements unless you are doing conjugate heat transfer. If you do need to keep them, the rest below still applies.

You can improve the quality a little on the far side of the fluid by opening up the angle there. The geometry doesn't go all the way, so the mesh doesn't need to be perfectly conformed to that shape all the way either. Open it up to 30 or 60 degrees at the FF using edge splits (not block splits). But this still won't help the elements right at the trailing edge.

Zoom in and take a look at those. The angle is constrained by the geometry, so you can't do anything about that. But if they are really long and skinny (long in the chord direction short across) then perhaps reducing the side 2 mesh size is the best solution to improve aspect ratio. Also look and make sure they don't appear warped or twisted (usually a mis-projection issue or an issue with misaligned edge params).

If your only concern is angle (which you can't possibly fix due to geometry constraints), then I suggest you just send it to the solver and see if the solver is as concerned about it as you are.

Keep in mind that these are just metrics, and some may not align with the needs of your particular solver. The ICEM CFD Quality metric is very "conservative" for prism quality. To calculate the ICEM CFD Quality metric, the software actually divides the prism (Penta-6) into 3 tetras (numerically speaking) and then gives the quality of the worst one. This very conservative metric is needed for some solvers, but not for others.

If you were checking based on "min angle", you would also get a low number, but that would be because it was a prism... The ideal angle for a Hexa is 90 and you really want to stay above 18 or at least 9 degrees for Fluent, but the ideal angle for a prism is 60, and the min angle tolerated by Fluent is much lower.

At 13.0, we are introducing a new "Orthogonal Quality" metric designed by a team of Fluent and CFX developers as the best measure of quality for those solvers.


CFD_SIM October 21, 2012 06:49

Thanks for the information and the link. I will look into it as soon as i can.

I think at this place the best thing to do is to look what the solver might say :-).

Iam not that familiar with the solver in Fluent, is he more prone to a "bad mesh" (min angle less then 9) or is the solver in ANSYS CFX more problematic?
For my simulation i will use ANSYS CFX so it would be good to know.

greetings

john

CFD_SIM October 22, 2012 04:03

Hey Far,

i have another question for you :-). I took a closer look at your mesh and iam not getting the same result as seen on the pictures that you ugploaded.

Is it still the same blocking? Because while i tried to recreate your blocking my quality wasn't that good. So i looked again in your file and there is, for example, the angle much worse.
Maybe iam just forgetting something.

Far October 22, 2012 04:22

Please turn-off the solid and VORFN

CFD_SIM October 22, 2012 04:33

Thanks! Stupid mistake :-D.

I think its time to look at what the solver might say to this mesh then :-).

energy382 October 22, 2012 13:26

I've attached blocking of the rib (note, that it's just a draft. you could of course do some additional splits and/or associations). Just to show you, how to get reasonable cell angles.

next steps to be done:

- extend solid blocking (use extend faces with a fixed distance....let's say with a value of 3 or 4 to create o-grid around your rib), create new part (FLUID) and assign these new blocks to fluid part.
- uncheck all geometry except pipe_inlet, do another 3-D blocking ("merge" to existing blocking), create C-grid
- create two vertical splits (one left and one right side of rib)
- extend all blocks except the 3 inner to your outlet
- use "create blocking from faces" to connect the c-grid to blocking round your rib (it's possible, that you've to do 2-3 additional splits)
- associate edges to curves

It's not that difficult. Try it on your own. As I'm busy with my own project, I couldn't do this too. If you've any queries, I'll help you out.

download link:

Quaterpipe.zip

CFD_SIM October 22, 2012 13:38

I have done the blocking today, as Far showed me. Not exactly like he did, but pretty close. I think with all the practice iam starting to get better :-).

I will try your way tomorrow and will check if my quality does improve, because the solver did not like my mesh much :-D.

Thank you for so much advise! I will need it, because the next thing to mesh is a nice little Blade^^.

If there are any further problems i will report them, but i hope it will work properly.

Far October 22, 2012 13:45

Quote:

Originally Posted by energy382 (Post 387941)
I've attached blocking of the rib (note, that it's just a draft. you could of course do some additional splits and/or associations). Just to show you, how to get reasonable cell angles.

next steps to be done:

- extend solid blocking (use extend faces with a fixed distance....let's say with a value of 3 or 4 to create o-grid around your rib), create new part (FLUID) and assign these new blocks to fluid part.
- uncheck all geometry except pipe_inlet, do another 3-D blocking ("merge" to existing blocking), create C-grid
- create two vertical splits (one left and one right side of rib)
- extend all blocks except the 3 inner to your outlet
- use "create blocking from faces" to connect the c-grid to blocking round your rib (it's possible, that you've to do 2-3 additional splits)
- associate edges to curves

It's not that difficult. Try it on your own. As I'm busy with my own project, I couldn't do this too. If you've any queries, I'll help you out.

download link:

Quaterpipe.zip

Hey energy382

Your method is awesome and new. But I need some practic to do like this, but hope to get help from you in other projects as well as you are way better than me.

Far October 22, 2012 13:52

Quote:

Originally Posted by CFD_SIM (Post 387946)
I have done the blocking today, as Far showed me. Not exactly like he did, but pretty close. I think with all the practice iam starting to get better :-).

I will try your way tomorrow and will check if my quality does improve, because the solver did not like my mesh much :-D.

Thank you for so much advise! I will need it, because the next thing to mesh is a nice little Blade^^.

If there are any further problems i will report them, but i hope it will work properly.

Any convergence issues or just starting warning~? If there is any warning then avoid it and continue running simulation and see what happens.


All times are GMT -4. The time now is 14:51.