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://i 234.photob ucket.com/ albums/ee2 69/craigcl avin/ANSYS Output.jpg
Surely it cannot be as simple as comparing these values to the recommendations made in ASME? Please see image below.
http:/ /i234.phot obucket.co m/albums/e e269/craig clavin/all owable.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.
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://i
Surely it cannot be as simple as comparing these values to the recommendations made in ASME? Please see image below.
http:/
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
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
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
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
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
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
In my opinion, EP is the way to go.