Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Stress concentration inspection

AM_20700

I have a shaft with a sleeve welded to it:

The shaft is fixed at the top. A torque is applied to the sleeve via an RBE3 element with the face of the sleeve as the independent nodes.

The shaft elements are solid. The sleeve and weld elements are shell.

The contact between t he sleeve and shaft is set to "Slide".

The stress results of a linear analysis show a ring of stress concentration at the interface between the shaft and weld:

The stress values are discontinuous along both the length and the thickness of the shaft (jump from 114 MPa to 73 MPa along the length, and 63 MPa along the thickness).

Length of shaft (weld removed for clarity):

Thickness of shaft:

How can I verify (and convince myself) that this stress concentration is an artifact, and not likely to be present in the physical machine?

Find more posts tagged with

English

OptiStruct

Accepted answers

All comments

Adriano_Koga

A few comments:

- your weld in real life is not a sharp corner, so the stress will be a finite value.

- in your case, what happens when you refine your model? does the stress converge? or does it diverge? if it is a singularity it would diverge, right?

- representing this with a mixed of shell and solid might not be the best approach, maybe. Probably it would be better to represent the connection using solids only.

- another point on welded joints is that FE usually cannot capture so well the real toe stresses. Many studies use toe weld extrapolation in order to calculate stresses (such as Volvo method, or hot spot stress)

AM_20700

A few comments:

- your weld in real life is not a sharp corner, so the stress will be a finite value.

- in your case, what happens when you refine your model? does the stress converge? or does it diverge? if it is a singularity it would diverge, right?

- representing this with a mixed of shell and solid might not be the best approach, maybe. Probably it would be better to represent the connection using solids only.

- another point on welded joints is that FE usually cannot capture so well the real toe stresses. Many studies use toe weld extrapolation in order to calculate stresses (such as Volvo method, or hot spot stress)

Thanks (and for your reply to my other post). I didn't try the 'Split" panel yet.

I decided to delete a strip of 3D elements adjacent to my area of interest. Then I split the solid in that region. Then extracted faces from the 3D elements. Then I associated the nodes of the extracted faces with the faces of the split solid. Then I created a Hex mesh between the faces:

The change in stress values along the length of the shaft is less abrupt, and the max value has increased. I couldn't locally refine the mesh along the thickness so the jump in values along the thickness is large (172 MPa → 44 MPa).
I can't refine the mesh any further without essentially turning the 3D elements into shells, so I guess I'll have to remesh the entire shaft.

Why is representing this with a mix of shells and solids not a good approach?

Adriano_Koga

Thanks (and for your reply to my other post). I didn't try the 'Split" panel yet.

I decided to delete a strip of 3D elements adjacent to my area of interest. Then I split the solid in that region. Then extracted faces from the 3D elements. Then I associated the nodes of the extracted faces with the faces of the split solid. Then I created a Hex mesh between the faces:

The change in stress values along the length of the shaft is less abrupt, and the max value has increased. I couldn't locally refine the mesh along the thickness so the jump in values along the thickness is large (172 MPa → 44 MPa).
I can't refine the mesh any further without essentially turning the 3D elements into shells, so I guess I'll have to remesh the entire shaft.

Why is representing this with a mix of shells and solids not a good approach?

In my opinion, usually when you need to get a detailed stress representation in these interface areas, using 3d mesh is better to capture these geometry transitions. Usually with shells you'll need to simplify a little bit the connection.

Adriano_Koga

In my opinion, usually when you need to get a detailed stress representation in these interface areas, using 3d mesh is better to capture these geometry transitions. Usually with shells you'll need to simplify a little bit the connection.

Just to be clear, using shells far from the interface area is ok. Just in this welded area, i believe a solid mesh performs better.

But of course, you need to take care with singularities, sharp corners,