### FEA Stress Singularities

Equivalent Stress - 4 Models of Square Hole in Plate

What are stress singularities?
Stress singularities are artificial stresses computed because of simplification in the FEA model.

What are the common causes of stress singularities?
1. Corners: e.g. sharp corners has theoretically infinite stresses because the radius is zero
2. Stiff Boundary Conditions: e.g. a tension bar with one end surface fixed in all direction.
4. Constraint Equations, Coupled Nodes etc
How does one overcome stress singularities?
1. Submodeling
Creating a submodel at the high stress locations with enough detail (e.g. fillet radius) along with mesh convergence study is the way to go. There is still engineering judgement on deciding what radius to use to best reflect the actual part.

2. Stress Concentration Calculation
Roark's formulas for stress and strain is a classic that is often used to determine the appropriate factors relative to the nominal stress. This works great if the load pattern and geometry is close to the textbook cases. It serves as a good way to ball park a similar type geometry.

3. Hot Spot Method
This is similar to what is sometimes done to estimate stresses for weld fatigue. One first creates a path of stress to the singularity. At a certain distance away from the stress singularity (~1mm in the example plot below), it is assumed the stresses are adequately far away and are thus reported. Often times a fudge-factor on top of the extracted stress value is applied to build in some conservative margin. What distance away? and what fudge-factor to use? Well, that has to be developed on prior, more detailed, modeling of similar parts.

This method takes some upfront homework, is quick and dirty and may require good hand waving skills.
Stress Path to Square Hole

Other points of discussion
I'm not aware of a way to deal with stress singularities caused by boundary conditions or nodal constraint equations / coupling or point loads. These modeling short-cuts are done to get a useful stress answer elsewhere and are justifiably ignored.

PRERR in APDL lists the structural energy norm. Here's a good write up illustrating its many limitations. It doesn't overcome singularity problems but with some experience, can help reduce the mesh convergence study needed.

Everything else being equal, mesh convergence study is one of the best, full proof method of gaining confidence of the computed stress. Unfortunately it does not work for stress singularities because the computed stresses will chase infinity as finer mesh is used. It works very well in gaining confidence in stresses elsewhere.

(Admittedly mesh convergence studies are not commonly done because it is very time consuming. Many analyst claim they make up for it with experience. Unfortunately it's a painful mistake I've made in the past. Healthy skepticism should be exercised.)

How do you handle stress singularities in your models?

1. Thanks for this information.
Well until now I haven't had any singularities in the simulations I've done.

### ANSYS User Defined Results

There is an abundant of options in ANSYS classic when one wishes to post process results. ANSYS workbench default pull down menu post processing options are more limited but they can still be accessed via the User Defined Results. One way not commonly used but can come in handy is as follows: Zeroth: Under Analysis Settings, there is "Output Controls" where you can toggle to "Yes" what you would like to save before the solution starts. This is like OUTRES in APDL. Output Controls First: After solving the model, click on Solution in the tree to highlight it. Solution Second: Click on Worksheet in the toolbar. Worksheet Third: In the worksheet, you will see list of results that are saved. Right click on it to create the User Defined Results. Create User Defined Results So here we have it. You could of look up the different expressions in the help document but I find this method of accessing the results convenient.  Example: Aspec

### Export Stiffness Matrix from Ansys

It is sometimes useful to extract the mass and stiffness matrix from Ansys.     *SMAT, MatK, D, IMPORT, FULL, file.full, STIFF       *PRINT, matk, matk, txt Exporting mass matrix would be similar:       *SMAT, MatM, D, import, full, file.full, MASS The above script uses APDL Math to get the job done. (Please see previous post for another example). The ordering of the matrix is unfortunately not concurrently exported. To verify the sequencing is as expected, we will work to replicate a truss example in the  Finite Element Trusses course notes by Bob Greenlee. Figure 1: Truss Problem Setup Model Creation Script to create model: /prep7 !! Creates Model to reflect course notes ! Properties et ,1,1  mp , ex, 1, 29.5e6 r , 1, 1 ! Geometry n ,1 $n ,2, 40$  n ,3, 40, 30 $n ,4, 0, 30 e ,1,2$  e ,2,3 $e ,1,3$  e ,3,4 ! Boundary Conditions d ,1,ux,0 $d ,1,uy,0 d ,2,uy,0 d ,4,ux,0$  d ,4,uy,0 f ,2,fx,20e3 f ,3,fy,-25e3 ! solves /solu eqslv , sparse