×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Stress Linearization in ANSYS 12.1

Stress Linearization in ANSYS 12.1

Stress Linearization in ANSYS 12.1

(OP)
Hi guys,

After trawling through previous posts regarding stress categorisation I have landed here with a new question. Hope you can help.

With regards to ANSYS and ASME VIII Div 2, there seems to be questions regarding ANSYS' method of stress categorisation.

I am currently working with V12.1 which generates a handy Excel file for your selected path line, or "SCL" in this case. In the Excel file it appears that ANSYS has already categorised the stresses into Membrane, Bending, and Peak etc.
Also provided is the Stress Intensity, or Equivalent Stress, if required. Please see image below.

http://i234.photobucket.com/albums/ee269/craigclavin/ANSYSOutput.jpg

Surely it cannot be as simple as comparing these values to the recommendations made in ASME? Please see image below.

http://i234.photobucket.com/albums/ee269/craigclavin/allowable.jpg


I feel like I am missing something pretty huge, or that ANSYS does NOT assign the stress categories inline with ASME, meaning all the hard work is still to do......

Your thoughts and comments are appreciated.
 

RE: Stress Linearization in ANSYS 12.1

What ANSYS cannot do for you is to separate primary and secondary stresses (usually the most relevant part of stress categorization).
The constitutive character of secondary stresses is that they are self limiting, and only a plastic analysis can test this condition.
So you need to decide whether your M or M+B stresses are primary or secondary to complete the stress categorization.

prex
http://www.xcalcs.com : Online engineering calculations
http://www.megamag.it : Magnetic brakes and launchers for fun rides
http://www.levitans.com : Air bearing pads

RE: Stress Linearization in ANSYS 12.1

(OP)
Thanks for the reply Prex,

To put it in black and white for me

Once I am satisfied I have defined M and M + B as either primary or secondary, then I can compare the values to those recommended by ASME?

An earlier thread (way back in 2007) received a response from "TGS4" Quoting as follows

"When I said that ANSYS linearization doesn't follow the Code methodology, I mean that it does not follow the procedure in 5.A.4.1.2., which is a mandatory part of the new 2007 Edition of Division 2."

Is this a question for ANSYS, or are you, or anyone for that matter, able to confirm this is still the case.

*For those viewing this thread in the present (or future) that aren't familiar with ASME VIII Div 2 Section 5.A.4.1.2. – This section provides the calculations for the bending, membrane and peak stress tensors.

Thanks again

RE: Stress Linearization in ANSYS 12.1

GlorifiedTap, I will answer that question directly.  I believe that ANSYS linearizes the COMPONENT stresses correctly.  However, my issue has been how the COMPONENT stresses are combined to form the SINT and SEQV linearized M+B stresses.  You will note that 5.A.4.1.2 directs you to only use the hoop and longitudinal M+B stresses and the M stresses for the remainder of the directions/shears in calculating the invariants.

If you can confirm for yourself that ANSYS is doing it correctly, then you are fine.  Last time that I used ANSYS, I could not confirm that.  And, as an example, in ABAQUS, you have the option of choosing which components to use in the calculation of the M+B invariants.

Does that make sense?

RE: Stress Linearization in ANSYS 12.1

(OP)
Thanks for picking this one up,

It does make sense although I have spent so many hours reading through ASME and trawling the net I'm beginning to suffer from "can't see the wood for the trees" syndrome.

With my current basic knowledge I have concluded that SINT is derived as per ASME, I believe it's something along the lines of "maximum value of the stress differences". This seems to check out ok.

As for the equivalent stress, I have applied the von Mises equivalent stress equation given in ASME to S1, S2, S3 provided by ANSYS and I get the same that ANSYS gets.

Perhaps ANSYS can confirm that the bending stresses are indeed calculated using the local hoop and merdional component stresses.
 

RE: Stress Linearization in ANSYS 12.1

(OP)
TGS4,

I have just found a post you made a while back about now peforming only elastic-plastic analysis and not bothering with stress linearization.

Are you saying the laborious process of stress linearization is not required if we perform an elastic plastic analysis?

That is something else i have had a play with using the calculation for tangent modulus from ASME.

Thanks

Craig

RE: Stress Linearization in ANSYS 12.1

Yes - that's exactly the point.  If you perform an elastic-plastic (EP) analysis, the process of stress categorization and stress linearization go away.

In my opinion, EP is the way to go.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources