Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- CAE Simulation - Simcenter 3D Forum
- Why difference in stress nodal with and without GA...

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

Highlighted

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-29-2018 10:04 AM - edited 08-30-2018 04:57 AM

Hello experts,

in order to get the elemental stress at integration points of elements (GAUSS) I switched the Stress output location in my property for CHEXA8 elements (selected deliberately) to GAUSS.

Now I get elemental and nodal stress values but no integration point values.

See here "Elemental stress" with GAUSS and DEFAULT=NODAL:

See here "Nodal stress" with GAUSS and DEFAULT=NODAL:

Elemental stresses are identical and nodal stresses are different.

What's the reason? Where I can find my integration point stresses? - I expect 2x2x2 values.

See in online documentation >>>

<<<

Test for one element (for example 184)>>>

<<<

In f06 file I've found for the element Measurement UNIT [mN/mm²]>>>

<<<

and Excel-Export is >>>

<<<

All looks identically. Where is my mistake? I'm not sure if I can get stress values at integration points (GAUSS). Is there a way?

Who can help. All suggestions are welcome. Best wishes, Michael

| *Production:* NX10; *Development:* VB, TCL/TK, FORTRAN; *Testing:* NX11 | *engelke engineering art GmbH, Germany *

| Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution".

Solved! Go to Solution.

Labels:

7 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-29-2018 10:44 AM

The elemental stresses are identical because they will be unchanged.

When you select GAUSS output, gauss point result values are output at the closest grid location. So, you are seeing the nodal output values changing, but they are no longer values at the corner node - they are values from the Gauss point closest to that corner node.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-30-2018 04:05 AM

JimB

My understanding has always been that nodal (stress) values are extrapolated values (using the element shape function) from the Gauss point. Is this wrong?

Production: NX.CAE 9.0.3.4, NX.CAE 10.0.2.6

Development: VB.NET (amateur level !)

Development: VB.NET (amateur level !)

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-30-2018 04:48 AM - edited 08-30-2018 04:57 AM

thank you for answering. That means that NX NASTRAN stores the stress tensor values of integration points of elements at the "place" of nodal stress tensor values of elements, ok.

But, does it mean that normally NX NASTRAN stores the nodal stress tensor for all nodes of element permanently and the post processor doesn't extrapolate it to nodal positions if needed? - I guess that's what @selex_ct also mean.

>>>

@selex_ct wrote:

JimB

My understanding has always been that nodal (stress) values are extrapolated values (using the element shape function) from the Gauss point. Is this wrong?

So if I need the stress values at integration points and I have integration scheme with 3 x 3 x 3 integration points (27 GAUSS points) I can't get all 27 results because the CHEXA20 has only 20 nodes, is it correct?

Or, If I understand the online documentation in the right manner, I must assume that GAUSS for CHEXA works only with linear element type in SOL101.

Is there a more general way to get the stress tensor at integration points (GAUSS point integration) in PCH or f06?

Maybe there is a PARAM to do so?

Can you or someone else explain it? - With regards, Michael

*Production:* NX10; *Development:* VB, TCL/TK, FORTRAN; *Testing:* NX11 | *engelke engineering art GmbH, Germany *

| Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution".

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-30-2018 10:27 AM

You need to consider the nature of "stress results" in a finite element analysis. In FEM - and that is not limited to NX Nastran but holds for all classical FEM solvers - we work with an "equilibrium in a weak sense". This means that the forces, that are intergated from the stresses over the elements, form an equilibrium in the nodes. "Stresses" are derived quantitities and that do not exhibit a stress equilibrium. Stresses are evaluated at the Gauss points for the residual force calculation. ** There is not a unique way to calculate stresses on element nodes **since the stresses are derived from the displacements and therefore discontinous over element borders. If the nodal and Gauss point stresses differs a lot, this can be an indication that the mesh is too coarse.

Martin

Global Simcenter 3D Portfolio Lead

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-30-2018 10:52 AM

@selex_ct, at a basic level, elemental results are interpolated from gauss point results and nodal results are extrapolated from the gauss point results. The exact sequence and methodology varies by solver.

The issue here is that post processors graphically display results and allow the user to interact (i.e. probe/identify) results. Traditionally, this interaction is done on an elemental level or a nodal level. Post processors typically do not have graphical "hit points" that correspond to the gauss points of an element. The post processor would have to understand element shape functions, integration orders, etc. in order to display gauss point results at the correct location in space.

As @MiDi1791 indicated, there is not necessarily a 1::1 correspondence between the number of nodes and the number of gauss points on an element. Thus, when gauss point results are requested, they are output as nodal results (to use a data structure that the post processor understands) where the value is obtained from the gauss point closest to the node.

This scenario is not perfect as there may be some gauss point results that may not be output (for higher integration orders) or some values that may be duplicated (for low integration orders).

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-30-2018 10:55 AM - edited 08-31-2018 06:11 AM

Martin,

thank you for answering. You are right in pointing out the importance of quantity differences for GAUSS values and nodal values.

The problem for me wasn't having different stress tensor components on integration points and nodal position. That I did expect. My problem was that I didn't know that GAUSS values where stored at data base position of nodal values i.e. "stress - element nodal". I did assume that a new result component would occur.

So my final question is:

What's the common way to get stress or strain components at integration points? - Is there such a capability in NX NASTRAN?

Best wishes, Michael

*Production:* NX10; *Development:* VB, TCL/TK, FORTRAN; *Testing:* NX11 | *engelke engineering art GmbH, Germany *

| Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution".

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-30-2018 11:05 AM - edited 08-31-2018 06:11 AM

thank you for answering. We worked on thread at the same time, I guess.

So now, with your explanations, I assume that there is no common way to get stress or strain values at integration points out of data base. - I can imagine the dealing with those results afterwards would accumulate only additional problems or questions like:

- What are the shape functions?

- Where are the correct integration point positions in a real element?

- ...

Or do you have differing (happy) news for me?

Best wishes, Michael

*Production:* NX10; *Development:* VB, TCL/TK, FORTRAN; *Testing:* NX11 | *engelke engineering art GmbH, Germany *

| Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution".

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc