1st Order Hex to 2nd Order Tet Transition

Hello everyone,

I meshed a geometry with both tet and hex elements. I would like tet elements to be 2nd order. So the pyramid elements which are used for the transition should not have mid nodes at hex side.

However, using the 'order change' for both tet and pyramid elements creates midside nodes everywhere. Is there a way to eliminate midside nodes of pyramid elements at rectangular face (9 node pyramids).

Thank you in advance.

Regards,

Emre

Find more posts tagged with

English

HyperMesh

Accepted answers

All comments

QuyNguyenDai

Hi, Tell me which solver supports this 9-node pyramids?

seyilmaz

ansys

Altair Forum User

Hi,

which ET in ansys supports 9 node pyramid?

I remember only 5 node and 13 node.

<?xml version="1.0" encoding="UTF-8"?>

image.png.0cf154ae80ce07821a31b4651c0d12eb.png

QuyNguyenDai

Theoretically, I don't know it's possible to build 9-node pyramid element?

seyilmaz

Dear sathya,

SOLID95 (legacy ET) and SOLID186 supports 9 node pyramids.

When you mesh a volume with 1st order hex elements then the connected volume with 2nd order tet, Ansys automatically creates 9 node pyramids at transition region. There are examples for hex to tet transition in web.

Regards,

seyilmaz

Theoretically, I don't know it's possible to build 9-node pyramid element?

To be honest, I did not dig into the theory.

tinh

If ansys can generate that pyramids you have to use ansys because hypermesh don't have. It's a strange element

QuyNguyenDai

Not only 'strange' but also impossible, mathematically.

seyilmaz

Not only 'strange' but also impossible, mathematically.

Great scientific approach from you. Thanks!

Phillip_20275

Sorry for the reply 4 years after the OP, but I found the answer and figured to share it in case others have a similar question. The answer is that Hypermesh has a utility function to eliminate midside nodes at the interface between 1st order and 2nd order elements. Documentation of this utility is here: https://2021.help.altair.com/2021/hwdesktop/hm/topics/user_interface/utility_menu_ansys_convert_special_second_order_macro_t.htm. Because links have a habit of breaking, I'll copy the text here:

ANSYS Convert to Special 2nd Order Macro

When you run the Convert to Special 2nd Order macro, a mesh matching is used to remove the mid-side nodes at the shared edges between these first and second order elements.

Models created for the ANSYS solver often contain second-order pyramid and tetra elements in which most sides contain "mid-side nodes". These types of elements exist in a transition layer between the first-order hexa and second-order tetra elements, as shown below.

Beginning in HyperMesh 8.0, these types of elements are supported and preserved in the model. HyperMesh can import:

Pyramid-shaped SOLID95 and SOLID92 elements with side edges containing mid-side nodes and bottom (base) edges that do not contain mid-side nodes
Tetrahedron elements with one or more edges that do not contain mid-side nodes
SOLID95 (special type)
SOLID187 (special type)

These special elements will be imported as full second-order elements, including mid-side nodes.

Imported full second-order elements are exported as special elements, thereby restoring the original element configuration. Similarly, special second-order elements created in HyperMesh are also exported as special second-order elements.

Mesh the part for first-order with hexa or penta elements. Place these elements in a collector with the correct element type (SOLID45).
Mesh the mating volume with second-order tetra elements. Place this mesh in a separate component with the correct element type (SOLID95 or SOLID92).
Ensure that the two mesh patterns have a common layer with shared edges between.
From the ANSYS Tools page of the Utility menu, click the Convert to Special 2nd Order macro.
Select the first-order component from the drop-down menu that shares a common face with the second-order meshed component.
Select the second-order meshed component in the next drop-down menu and click Apply.
The special order elements are generated
Export the file. Read it in the solver and check the elements.
The following images show examples of proper meshing for the above practice.
Figure 4.