How to modify the aspect ratio of an element 2

[Dan90]

Hi to everyone,

I have a problem with the aspect ratio of some elements within my meshed geometry.

Practically I need to mesh a geometry with a max aspect ratio equal to 5, but, after many operations on my mesh, some elements still have a too high value of the aspect ratio.

Can someone suggest me a way to improve the quality of the mesh from that point of view?

 

[rb1957]

reduce the length or increase the width ...

yes, i know that a pretty dumb reply but those are the only ways to answer your question.

why can't you reduce the length (clearly easier to add elements) ? increasing the width would mean merging elements together.

is this magic "5" written in a spec ? an aspect ratio of 5 could be unacceptable (is an area of high stress gradient).

another day in paradise, or is paradise one day closer ?

 

[Dan90]

Dear rb1957,

thanks for the very quick answer.

The magic value of the aspect ratio I need to obtain (5) comes from a specific for a FEM sound propagation problem.

I am using Femap to mesh my geometry which I will solve in another software (more specific for vibroacoustic problems).

Clearly, increasing the number of elements could be a solution but I already have more than 330000 nodes, which are enough for my model's dimensions.

I am not an expert in meshing, so I have attached my geometry.

Do you think there is a more efficient way to mesh it?

 

[rb1957]

i couldn't open your stp file (my computer issues, not your attachment) ... how about a pic/pdf ?

what's the problem with more nodes ? so the problem takes a little longer to solve ?

another day in paradise, or is paradise one day closer ?

 

[ThomasH]

Hi

I think a picture that shows the meshed area that causes the problems would be helpful. I managed to open the stp file and there are some surfaces with high aspect ratios. Those surfaces may be governing for the meshing. It depends on how you have made your mesh to beging with.

Regards

Thomas

 

[Dan90]

Hi ThomasH,

thank you too.

Yes rb1957, the more the nodes, the longer the solution time.

I have attached three images, with could show one of the problems. Treating very small elements, it is also difficult to find where the other elements causing error are located.

Thomash, what do you mean by "how I made my mesh beginning with"?

http://files.engineering.com/getfile.aspx?folder=3d1ff26b-b0b7-4c26-b8a6-d80bca5893f9&file=Mesh.png

http://files.engineering.com/getfil...809f-98b94c0d777c&file=Quality_colour_map.png

http://files.engineering.com/getfil...5c-9da9-56ee016b05a5&file=Problem_example.png

 

[rb1957]

my apologies ... i went to rectangular elements, not TETs.

i think you've found a "sliver" in your CAD model. i think you should be able to delete this by joining across the sliver ...

if you have a TET with N1 on one side of the sliver, and another, on the other side with N2 that's almost in the same place as N1 (on the other side of the sliver) then change N2 to N1 and the sliver should disappear.

another day in paradise, or is paradise one day closer ?

 

[BlasMolero]

Dear Thomas,
The base geometry is a little disaster, you need to clean-up yor geometry in order to get quality mesh, this is the "secret" to arrive to an excelent FE model, the geometry base.

The first thing I will do is to run "Geometry > Solid > CleanUp" and activate the four options. This command will check the solid, and remove any extraneous features which are not part of the actual solid, but may have developed during export from a CAD package or from Boolean operations on it. If a portion of your solid appears inaccurate, or drawn incorrectly, use this command to see if you can remove it. And in general is better to answer NO when FEMAP detect problems like SLIVER GEOMETRY, is better to control yourself the changes.

"Slivers" are small faces that are created because of numerical inaccuracies in Boolean or other solid modeling operations. Typically these faces are much smaller than the other faces that define your solid. While they are small, they can cause great difficulties in meshing. They will often completely prevent a part from being hex meshed. FEMAP will try to removes these surfaces and attempts to restitch your solid without them. This option is only available with Parasolid geometry.

It will give you error of "Sliver Removal", then click CANCEL (do not let FEMAP to do the job automatically).
Take a look to this video to learn how to use the MESHING TOOLBOX and search for small edges. Also you can try "Mesh > Geometry Preparation" command, and automatic way of cleaning a CAD model.

http://youtu.be/ZgkT2w66wu8

Yes, under MESHING TOOLBOX you have plenty of resources for more or less automatic fixing tools like "COMBINED/COMPOSITE CURVES" and "COMBINED/COMPOSITE SURFACES", also "FEATURE REMOVAL" and "FEATURE SUPPRESSION", but I am of those that like ful control of geometry changes and to perform myself all fixing and repairs, you can try and see the best approach to follow, all depends of the geometry complexity. Take a look to this excellent video from Mark Sherman about combination of surfaces:

http://youtu.be/nbQu7yLVQzk

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Dan90]

Dear Blasmolero,

Thank you very much for your precious suggestions.

I will let you know if I succeed in fixing the problem.

Greetings.

 

[assafwei]

Dan,

In the last image you attached - it seems as if you have some overlapping elements in addition to the high aspect ratio elemens, I would suggest doing as Blas offered - first take care of the base CAD geometry and have a clean CAD, then try to mesh.

 

[BlasMolero]

Dear Dan,
CleanUp the geometry base is critical: try to use first the basic commands found under "GEOMETRY > SOLID" menus, the REMOVE FACE command is great, first locate small edges & sliver surfaces using the MESHING TOOLBOX, one of the most powerful tool of FEMAP: the ENTITY LOCATOR in the MESHING TOOLBOX !!.This is really powerful, you can "scan" your FEMAP model and search for any entity (curves, surfaces or elements) like "Short Edges", or "Adjacent Edges", etc..

After performing the geometry solid CleanUp I trick I usually run to see is 3-D meshing will be successful is to perform a 2-D mesh using ALL the surfaces of the solid with 2-D PLOT-PLANAR elements using command "Mesh > Geometry > Surface > Method = On Solid", select the solid body, click OK and in the AUTOMESH SURFACES form do not select any property (let the field empty, in blank!), this way you will mesh with plot-only elements.

After performing the 2-D mesh look for FREE EDGES using command "View > Select" (o clicking the short-cut "F5" key), if not free edges exist then your 3-D solid mesh will be successful.

You can improve the 2-D mesh "interactively" using the MESHING TOOLBOX with "MESH SIZING", when you are happy with your 2-D mesh then issue command "Mesh > Geometry > Solids" and the 2-D PLOT PLANAR mesh will be a seed-mesh for the 3-D TET mesh, OK? -- Enjoy!, meshing with FEMAP should not be a pain, but a pleassure!!.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Dan90]

Thanks to your suggestions, I succeed in getting a better mesh, but some elements still cause me problems.

In particular, It seems that there are elements with an aspect ratio of about 179 but I cannot find them.

Does an automatic way to recognize these elements exist?

Greetings.

 

[Dan90]

Here below is the file attached..

 

[BlasMolero]

Dear Dan,
For plotting element quality checks in 3D solid elements forgot at the MESHING TOOLBOX, this is for 2-D mesh, for 3-D TET elements you need to use command "View > Advanced Post > Contour Model Data" and for TET elements forgot at all the ASPECT RATIO, the important distorsion factor to control TET-COLLAPSE & JACOBIAN RATIO. I have played a few minutes with your geometry and here you are a solid 3-D TET10 mesh with a TET COLLAPSE RATIO = 27.35 (the recommended level from NX NASTRAN is maximum 10.0). Is important to activate the option "ALLOW LABELS", this helps to locate the element with higher distortion.

And to know where the maximum distorted elements are located simply use command "Tools > Check > Element Quality", here you can find the recomendations of minimum element quality thresholds for 2-D and 3-D elements. Feel free to play with each check, if you click in SHOW then you will see "highlighted" the element with the high value, then you can locate its position. Also activate the option LIST QUALITY SUMMARY > OK and you will see a summary of quality in the message window, OK?.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Dan90]

Ok Blas,

thank you again.

I wonder, is it possible to merge adjacent elements?

I mean, If I found two adjacent element (one follows the other), one of which causing error, can I merge this element with "the following"?

 

[rb1957]

if the two elements have common nodes (3 for TETs) then there should be one node common to the two TETs and you can edit one element to swap nodes (so that one TET encompasses both elements).

check by window/show entities/elements select elements "using node" and only the two TETs should show up.

clear as mud ?

another day in paradise, or is paradise one day closer ?

 

[Dan90]

Hi rb1957,

what do you mean by "editing one element to swap nodes"?