Matching mesh

Rahul_P1

Hello,

I actually encounter problem for meshing two tubes forming a T shape with two shell tubes (which will have different thickness and so belong to two different components), the pictures below describes the general idea:

However the mesh (created using 2D Automesh) for the blue tube and the red tube don't match:

My question is how can I make them match without using equivalence because it creates bad quality mesh and result in failing the simulation?

Thank you very much for your help

Rahul_P1

Hi Albain,

If the mesh size (element size) can be same in both the tubes, you should merge the tubes together (for instance, you could just translate the tubes until they intersect, then you can trim the tubes so that they are now connected,) and then mesh both the tubes at once using automesh, keep connectivity option.

However, you could perhaps try the mesh imprint option, see - HyperWorks Desktop Applications > HyperMesh > User's Guide > HyperMesh Panels > HyperMesh Panels Listed Alphabetically: > Mesh Edit Panel

Rahul_P1

Hi Rahul,

Unfortunatelly, I can't mesh both tubes at the time as they have different thickness (and so different properties applied to two different components, one for each tube). They also are connected, thanks to the CAD. So there is nothing to trim and the mesh imprint option fails...

Thank you for your time and your answer

Rahul_P1

Albain,

The fact that they have different thicknesses should not affect our shell mesh,

We can still mesh them together, then reorganize to different components and then assign different properties/thicknesses (you can assign different thicknesses to different elements even if you do not organize them into different components.

Please send me the model using the dropbox below and then I can guide you better.

Rahul_P1

Albain,

Step 1 - go to defeature > duplicates > find > delete all duplicate surfaces

Step 2 - go to quick edit > toggle the edges where they meet

Step 3 - go to surface edit > trim with lines > trim the surfaces > use the lines where the tubes intersect to trim
so that that the perpendicular tube and the vertical tube have trimmed surfaces where they meet.

Step 4 - mesh using automesh > keep connectivity

Step 5 - re organize the elements to desired collectors by selecting elements > by geoms > surfaces > select the relevant surfaces

Then you get the desired result !

Rahul_P1

Thank you very much for your help!

I also find another way to do it using connectors:

Step1
Connectors >Create> Seams
select the line between the two tubes
Connect what> comps select the whole model and switch elem to geom
Type= weld
Create>Return

Step 2
Mesh the whole model (/!\ you have to mesh the surface from the inside of the tube) 

Step 3
Reorganize the element to desired collectors ...

mirko088

Hi, i have the same problem with different component . Can you help me?

Altair Forum User

Which photo do you like best? I have many more photos (photos are clickable)*