Help to do quasistatic analysis in static structural module

[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.