MPCs for Hex-Tet Interface 2

[feajob]

Hi,

In Thread727-152330, hex mesh versus tet mesh was well discussed. Recently, I thought to take advantage of both them by interfacing tet10 with hex20 elements (parabolic elements).

So far, I am happy with the obtained results of my first model. I should mention that I am using MSC.Nastran.

You can find more details at the following link:

http://members.tripod.com/~NilanjanM/meshing_work/HTMPC.html

I am wondering if someone else has any experience about this kind of interfacing.

Thanks,
A.A.Y.

 

[gwolf2]

I find it easiest to align 4 linear HEX elements with two parabolic TET elements as shown in the attached picture. Just merge the nodes to make the connection. Yes I do mean merging mid-side nodes with corner nodes!!

It works surprisingly well and is much quicker and less error prone than MPC's for large interfaces. In bending test models a few years ago I got less than 5% stress discontinuity across the boundary and good stiffness characteristics - comparable with or better than MPC's or the tied contact available in packages more sophisticated than NASTRAN. Just don't use it anywhere near where you want really accurate stresses.

Because of the relative merits of linear/parabolic HEX/TET elements across many FE packages and Meshing programs, the linear HEX/Parabolic TET permutation is very common.

gwolf

 

[feajob]

Hi gwolf2,

Thanks for you response. I would like to provide more information about my models. Well, I usually have complex 3D geometry with many lugs and sockets interfaces. So, meshing my model with only hex elements is impossible. I mesh them with tet10 (parabolic) elements. But, I am unhappy about the tet10 elements at interface (contact) regions (such as lugs inner surfaces and sockets inner surfaces).

Recently, I used hex20 (parabolic) elements at contact regions with appropriate MPCs. As you mentioned, I believe that interfacing hex8 (linear) elements with tet10 (parabolic) elements is easier and more practical approach. By subdividing each hex20 elements, we can get 8 hex8 (linear) elements. In this way, total number of DOFs are similar. As you know, tet4 (linear) is much stiffer than tet10 (parabolic) elements and that's why we don't use them for detail stress analysis.

Now, if we have two approaches as follows:

1) N1 x Tet10 with N2 x Hex20 elements
2) N1 x Tet10 with N2 x 8 x Hex8 elements


In other words, if we replace each hex20 element with 8 hex8 elements then we can keep the same DOFs. I have only one question, what do you think about the quality of the outcome of these approaches? (from stress viewpoint)

I personally think that the difference should not be significant.

Thanks,
A.A.Y.

 

[gwolf2]

For models with contact interfaces like lugs and sockets which you describe I never use HEX20's at the interfaces - the contact stresses become far too 'spotty' and the models don't converge well.I only use HEX8 elements at contact areas regardless of analysis package.

I have no tests but 8 HEX8's for one HEX20 sounds like a reasonably fair swap, perhaps slightly less accurate at a free surface fillet radius. Certainly better for contact.

I have used the method of mixed element types for complex models with contact with great success for about 5 years - it's the best way. I have never tried this in conjunction with contact in NASTRAN, but that's another question really. I tried HEX20's alone with NASTRAN contact once and was disappointed.

My personal favorite is using ABAQUS with a mixture of C3D10 Tets and C3D8I Hex8 incompatible mode elements at the contact areas - The stress quality at the contact is superb and you don't need to have identical meshes either side of the gap (but it helps). Just make sure that you carry the HEX mesh around the holes out to about 3x hole diameter before merging with Tet's

gwolf