Apply a Stress Field to a Model


Hi, I would like to apply a stress field to a transient structural model to define a complex pre-stress. I have looked around in Ansys manuals and saw that you can apply material fields (e.g. for density) as shown in the screenshot but I am not sure if I can do something similar for stress. I was also wondering if you can export a stress field from Ansys results e.g. by exporting the stresses on all nodes of the model? Any help would be greatly appreciated!

Best Answer

  • peteroznewmanpeteroznewman Member
    edited December 2020 Accepted Answer

    @Manatee

    Yes, you could create an initial state of stress in the pipe wall so that when you apply the pressure, the pipe doesn't expand. You can do this in the simulation. How do you do that in the real world?

    What you can do in the real world is change the initial shape of the pipe so that it has a slight reduction in diameter at the center which flares out to the ends. You can actually make that. Then when internal pressure is applied, the pipe expands out to an approximately cylindrical shape. You can simulate that.

    I suggest you create parametric geometry in DesignModeler (or SpaceClaim) that has a parameter for the center diameter of the pipe and a smooth curve to flare out to the end flange pipe diameter. Then do a Parameter study where you sweep over a range of center diameter values and plot the center diameter with the full internal pressure applied.

Answers

  • peteroznewmanpeteroznewman Member
    edited November 2020

    @Manatee

    The easy way to create a stress field is to apply the loads and boundary conditions to the structure and perform a static structural analysis.

    In a Transient Structural analysis, you can create a 3-step solution. Step 1 applies the loads and boundary conditions as you would for a static solution, and by turning off Time Integration under Analysis Settings, you get a static solution. Step 2 changes nothing and also has Time Integration off. The purpose of step 2 is to assign zero velocity to the model because otherwise the deformation of step 1, divided by the time, would define a velocity for the next step. Step 3 is the start of the Transient loads and Time Integration is turned on.

  • ManateeManatee Member
    edited December 2020

    Thank you @peteroznewman !

    I would like to create an internal pre-stress in the wall of a pipe to counteract a static internal pressure to create a starting point for an FEA simulation where the pipe does not (significantly) extend when this initial pressure is applied.

    Do you think your described approach would work for this?

    I was thinking about doing the following but I am not sure how to do this in Ansys:


    Step 1: First iteration: Time: 0, Load: 0 / Time: 1, Load: Pressure

    Step 2: Take stress distribution and apply/map it back to the pipe wall as pre-stress

    Step 3: Second iteration: Time: 0, Load: Pressure / Time: 1, Load: Pressure

    There should be less extension now. Repeat iterations until distension is sufficiently low.


    A colleague of mine did something similar in Abaqus but I am not sure if this is possible in Ansys? Thank you!

  • peteroznewmanpeteroznewman Member
    edited December 2020 Accepted Answer

    @Manatee

    Yes, you could create an initial state of stress in the pipe wall so that when you apply the pressure, the pipe doesn't expand. You can do this in the simulation. How do you do that in the real world?

    What you can do in the real world is change the initial shape of the pipe so that it has a slight reduction in diameter at the center which flares out to the ends. You can actually make that. Then when internal pressure is applied, the pipe expands out to an approximately cylindrical shape. You can simulate that.

    I suggest you create parametric geometry in DesignModeler (or SpaceClaim) that has a parameter for the center diameter of the pipe and a smooth curve to flare out to the end flange pipe diameter. Then do a Parameter study where you sweep over a range of center diameter values and plot the center diameter with the full internal pressure applied.

  • @peteroznewman

    Thank you, I did something similar to what you recommended in your first line. I created the desired contractive stress profile in my model by expanding it in a preparatory simulation, exported the resulting stresses and nodal locations and then fed it into a new Mechanical simulation via the External Data module in Workbench. This created the desired pre-stress profile I needed for the start of the actual simulation.

Sign In or Register to comment.