Solving an Ansys WB Stress Concentration Issue on Stiffener Tip

In summary: The mesh is not an all-quad mesh and there are contact conditions between the stiffeners and column. You should add a meshing method parameter to the mesh to make it a continuous mesh. You can also sum the bodies together in your CAD software to make a single object.
  • #1
EngAB
7
0
Ansys WB, getting non-realistic stress conce. (stiffener tip on pipe column face)??

Hi,
I am facing a problem in getting accurate stress in Ansys WB for stiffened base plate supporting pipe column (See attached pics)

The problem is that I'm getting very high stress concentration at the tip of the stiffener connected to column face. The column is under pure tension (as a simplified case) but I have the same problem if having moment.

I have tried to modify keyopt(3) and (8) but that didn't solve the problem maybe I'm doing it wrong as I'm not experienced on this.
I have added these commands under the bonded contact region connecting stiffeners Or weld to the column:
keyopt,3,2
keyopt,8,2
keyopt,11,1

I have also tried to add fillet weld generated in Cad modeling, to join the stiffeners to column but there is a problem that I couldn't solve that causes no bonding between column and stiffeners as shown in the attached picture.

in the attachment there are 2 pics;
one for the model without fillet welds
https://www.physicsforums.com/attachment.php?attachmentid=32262&stc=1&d=1297874602
and the other with.
https://www.physicsforums.com/attachment.php?attachmentid=32261&stc=1&d=1297874602

I'm sure there is a solution, because this is not a complex structure, if not it would make the software kind of useless!

I want to verify my hand calculation.
Regards
 
Last edited:
Engineering news on Phys.org
  • #2


Okay I have solved the problem of bonding between weld and column but still the stress is non-realistic.

Any help is extremely appreciated.
 
  • #3


I have really spent tremendous time but couldn't solve the problem, the stress concentration is not solved, either by weld or without.

Any help please?
Regards
 
  • #4


What does your mesh look like? As screenshot of it in the problem area would be helpful. You might consider doing two things:

  1. Make the mesh an all-quad mesh by inserting a meshing method parameter into the mesh.
  2. Make the mesh a continuous mesh rather than using contact conditions (but you might need the contact conditions for a weld stress analysis). Doing this requires making it a multi-body solid in DesignModeler, or simply summing the bodies together in your CAD software.

Remember that a "perfectly sharp" corner in an FEA model causes a stress singularity which cannot be resolved- the more you refine the mesh, the higher the stress gets. Your options are to either fully model a fillet weld in that region (might not be a very good option since accurate material properties in and around the weld region are problematic) or to simply discount the stress within a certain distance of the sharp corner as false.

EDIT- I also notice your second picture shows that your modeled welds apparently do not have a contact condition to the side flanges. You should add contact conditions there to prevent the separation you're seeing.
 
  • #5


Thanks dear Mech_Engineer
I appreciate your help,
Unfortunately I have tried the all-quad mesh choice but didn't solve the problem,
A screen shot in the attachment for the mesh,

and zip file is here:
http://files.engineering.com/getfile.aspx?folder=b75e05e2-3e2b-435d-8bf4-2c6b31331246&file=basep.zip
containing the model as .igs file and the ansys WB file, I have converted the model to igs because maybe the Cad software I'm using "Pro/e" is not used by the members here.

After conversion I have set the settings to what I believe to be the same with my current model, but I don't know why the stresses has gone extremely high.

Also regarding making the stiffeners and column as one part then mesh them (And even I made the stiffeners penetrate column face for 3 mm to make sure there is no gap but still it is high (Although it reduces)).

I don't feel that it would be suitable to ignore these stresses because I'm mainly concerned on stresses related to the existence of the stiffeners. Also I will use the FE to examine the stresses when having moment and shear forces and other cases.

I have gone through this guide,
http://wenku.baidu.com/view/1460b80e76c66137ee061991.html
and tried to add the commands stated, but no much difference.

If there is somehow a solution I will be grateful .
 
Last edited:
  • #6


Regarding the weld issue yes you are right there was a problem in the contact with column, I tried it yesterday and it reduces the stresses sufficiently (Although I have used large throat size) but at the top the Cad software won't make continuity at the top corners which causes over stressing at the top middle.

To model it my self, should it be shell? (The auto generated fillet weld is shell) or I can make it as triangle then extrude as solid? I'm not sure It is possible to make it as an isolated shell part with that shape.
 

1. What is a stress concentration issue in Ansys WB?

A stress concentration issue in Ansys WB is when there is a localized area of high stress in a structure, typically caused by a sudden change in geometry or material properties. This can lead to structural failures and needs to be addressed in order to ensure the safety and integrity of the structure.

2. How can I identify a stress concentration issue in Ansys WB?

Stress concentration issues can be identified by analyzing the stress distribution in a structure using the post-processing tools in Ansys WB. Areas with high stress values and a sudden change in stress gradients are indicators of a potential stress concentration issue.

3. What causes stress concentration issues in Ansys WB?

Stress concentration issues can be caused by various factors such as sharp corners, changes in cross-sectional areas, holes or notches in a structure, and material discontinuities. These features can create stress concentration points where the stress is significantly higher than the surrounding areas.

4. How can I solve a stress concentration issue in Ansys WB?

The first step in solving a stress concentration issue is to identify the cause of the problem. Once the cause is identified, you can make design changes such as rounding off sharp corners, changing the geometry, or adding material to reduce stress concentrations. Another approach is to use advanced modeling techniques such as fillet or blend features to redistribute the stress more evenly.

5. What are some best practices for avoiding stress concentration issues in Ansys WB?

To avoid stress concentration issues in Ansys WB, it is important to consider the design and material selection carefully. Designing with gradual transitions and avoiding sharp corners can help to reduce stress concentrations. It is also important to select materials with consistent properties and avoid changes in material properties along a structure. Performing a thorough stress analysis using Ansys WB before finalizing the design can also help to identify and address potential stress concentration issues.

Similar threads

ANSYS Static Structural boundary constraints issues
    • Mechanical Engineering
Replies
3
Views
5K

Hot Threads

Recent Insights

Back
Top