Learning Forum

[mhannan]

Hey, I am doing quasistatic analysis in static structural module of ansys. My whole load curve is for 3 second and it’s not linear or constant load for 3 second. The loads changes within a very short time like 1 have almost 30point of load in between 0 to 1 second. There are almost 137 points of load in the whole 3 sec curve and loads for all the 137 points are different.

How can I get result for the individual 137 points ??

 

This loads are my input pressure and how can I get output for the all individual point(input points of pressure vs time are generated from the graph by webplotvisualizer) in ansys static structural.

[peteroznewman]

In Static Structural, under Analysis Settings, Step Controls, you can set the Number of Steps to 3 and set the Step End Time for each step to 1, 2 and 3 s.

In the Pressure load, there is a pull down menu that allows you to select Tabular data input.

In the Tabular data window, click once in the blank cell to the left of Steps to select the whole table.

In Excel, copy the 2 columns and 137 rows of numbers plus one blank row at the bottom. In Mechanical, right click on that same blank cell in Tabular data and select Paste. My example shows 8 rows of data and I have selected 9 rows to copy.

You can do the same thing with just one Step.  Just set the End time to 3 and copy paste the data in the same way and you will get the same load history.

Finally, you want to force the solver to take small enough time steps to not skip over any part of the load history.  Under Analysis Settings, change Auto Time Stepping to On then Define By Time.  Set the Initial and Maximum Time Step to a value smaller than the smallest time increment in your table.  Set the Minimum Time Step to a value one tenth of that smallest time increment.

If you used one load step of 3 s you are done.  If you used 3 load steps, you have to repeat the previous paragraph two more times for each load step. 

[mhannan]

hey, I tried your process and I faced errors:

error1: The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose.

error2: Element 10365 located in Body "for fsi - Copy|Sclera" (and maybe other elements) has become highly distorted.  You may select the offending object and/or geometry via RMB on this warning in the Messages window.  Excessive distortion of elements is usually a symptom indicating the need for corrective action elsewhere.  Try incrementing the load more slowly (increase the number of substeps or decrease the time step size).  You may need to improve your mesh to obtain elements with better aspect ratios.  Also consider the behavior of materials, contact pairs, and/or constraint equations.  If this message appears in the first iteration of first substep, be sure to perform element shape checking. Named Selections for the offending element can be created via the Identify Element Violations property on the Solution Information Object.

warning 1: The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose.

warning 2: Solver pivot warnings or errors have been encountered during the solution.  This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues.  Check results carefully.

 

https://drive.google.com/file/d/1EHkE4lLSBiPs3Mqmd5lNLObQtBCc4mmJ/view?usp=sharing

[peteroznewman]

I can't open your model because it contains modules that are not included in the free Student license.

Try deleting the mesh and archive the project with no mesh, then upload that archive to see if that helps me to open it.

[peteroznewman]

The process I provided was to import 127 rows of time history into the pressure load, you must follow a different process to obtain convergence.

The highly distorted error message contains some good advice which you should follow. Try incrementing the load more slowly (increase the number of substeps or decrease the time step size). You know where to find that.  It is helpful to first look at the Force Convergence plot under the Solution Information folder. The graph shows you what time the solver ran into problems converging. The graph also shows you how many times the automatic time stepping algorithm used bisection to reduce the time increment. You can also change the plot to show the size of the time increment vs time.

Another piece of advice in the error message mentions that you may need to improve the mesh. However, you need to know where on the mesh the solver is having difficulty converging. To see that, edit the Analysis Settings. Click on the Solution Information folder and on the line that says Newton-Raphson enter a number, say 3.  This will make 3 contour plots under this folder that show you where on the mesh the force imbalance was largest for the last three iterations. If there are large elements there, you may need smaller elements or if the elements are of low quality, you may need to improve the shape.

[mhannan]

Rather than time step, I use step number and now the simulation converges, can you look into this???
I am also facing problems in implementing subroutine, can you tell me the process?

https://drive.google.com/file/d/1g1vRm8BfO_--YiE75Kg3b2pGuTZTStO2/view?usp=drive_link

[peteroznewman]

I was able to open the model and look at the solid bodies where I noticed that there is a body called Lens and another identical body called NONE. They are both meshed. Is that intentional or a mistake?