Ansys does not comply with ASME Section VIII Div. 2 part 5

Question

Ansys does not comply with ASME Section VIII Div. 2 part 5

shiraz883 (Automotive)

(OP)

14 Dec 17 12:22

thread569-380066: ASME VIII Design By Analysis with Ansys WB 15

Hi,

This is in reference to the thread in which TGS4 says that "ansys does not comply with ASME VIII div.2 part 5". Can someone elaborate on that? Because I went through the ANSYS help topics and searched "stress linearization" and saw the same formulae as used in the code. I do not see a reason for non-conformation of ansys linearized stress with that dictated by the code.

Thanks,
Shiraz

TGS4 (Mechanical) · Answer 1 · 2017-12-14 12:52:25

RE: Ansys does not comply with ASME Section VIII Div. 2 part 5

TGS4 (Mechanical) 14 Dec 17 12:52

Have you reviewed 5-A.4.1.2?

shiraz883 (Automotive) · Answer 2 · 2017-12-15 06:59:28

Yes I did.

Please find the attached comparison between ASME and ANSYS linearized stresses.

http://files.engineering.com/getfile.aspx?folder=15519046-0b3b-42d4-a4ba-c7

shiraz883 (Automotive) · Answer 3 · 2017-12-15 07:00:52

The earlier post allowed only one attachment. Here is the ansys linearization snapshot from ansys help topics

http://files.engineering.com/getfile.aspx?folder=36ee6b56-1356-49b1-aa47-27

TGS4 (Mechanical) · Answer 4 · 2017-12-15 14:22:10

RE: Ansys does not comply with ASME Section VIII Div. 2 part 5

TGS4 (Mechanical) 15 Dec 17 14:22

See Step 2 (b). That's the critical parry.

shiraz883 (Automotive) · Answer 5 · 2018-01-11 12:14:54

Thanks TGS4,

I see that a macro is already there wherein this critical parry is taken care of. Saw it few weeks ago and there was a manual evaluation (in one of the axis-symmetric models) by taking the values of Sx,Sy,Sz,Sxy and Seqv using PDEF command in ansys and doing manual calculation by applying simpson's rule of integration over these data points.

Thanks
Shiraz

TGS4 (Mechanical) · Answer 6 · 2018-01-16 14:28:14

You're completely missing the point.

Quote (ASME Section VIII, Division 2, Annex 5-A, 5-A.4.1.2)
Step 2. Calculate the bending stress tensor.
(a) Bending stresses are calculated only for the local hoop and meridional (normal) component stresses, and not for the local component stress parallel to the SCL or in-plane shear stress.

The point is that when assembling the bending stress tensor, it is composed of the membrane-plus-bending stresses ONLY from the hoop and meridional directions. In the other orthogonal direction (through-thickness), as well as for all of the shears, only the membrane stress is to be used when forming the tensor. ANSYS generates that tensor using membrane-plus-bending for all 6 component stresses, without an option to revert any components to membrane only.

rickfischer51 (Mechanical) · Answer 7 · 2018-01-17 14:37:39

Sounds like a need for an enhancement request. Or maybe a job for APDL.

Rick Fischer
Principal Engineer
Argonne National Laboratory

TGS4 (Mechanical) · Answer 8 · 2018-01-17 19:34:17

Have been requesting it since 2002. And have been asking other users to request it, too. Even mentioned that ABAQUS has had this capability. We'll see...

I have a work-around, in any case.

rickfischer51 (Mechanical) · Answer 9 · 2018-01-17 20:18:57

What's the workaround? Macro?

Rick Fischer
Principal Engineer
Argonne National Laboratory

TGS4 (Mechanical) · Answer 10 · 2018-01-17 23:22:52

RE: Ansys does not comply with ASME Section VIII Div. 2 part 5

TGS4 (Mechanical) 17 Jan 18 23:22

Some APDL and some MathCAD worksheets.

rickfischer51 (Mechanical) · Answer 11 · 2018-01-18 14:17:45

I contacted our Ansys tech support guys. They are putting in an enhancement request, and they are sending me a macro. I'll keep you posted.

Rick Fischer
Principal Engineer
Argonne National Laboratory

Come Join Us!

Posting Guidelines

Jobs

Ansys does not comply with ASME Section VIII Div. 2 part 5