Boundary Conditions and Temperature profiles manipulation?

The first question I have is if I have a temperature profile at SS can I create a linear ramp vs. time in ANSYS?

For example claim the system is at room temperature at 0 seconds and that my steady state file is at 25 minutes. Thus there is a linear ramp for 25 minutes at each node. My current solution has been creating CSV files in MATLAB to create this linear ramp.

Second Question:

I am preforming fatigue life analysis on a large pressure vessel used for a super sonic nozzle rig. However, the goal is to preform this with out fixed boundaries. The bolt holes will be expanding radially, and the pipe is free to expand axially as the entire rig will be on wheels. When fixing the bolt holes there are large stress concentrations that occur about the boundary conditions and virtually no stress downstream.

I believe the large stress concentration of the pipe to derive from the inability of the flange to expand outwards due to the fixed bolt holes. In reality our system will be expanding as the flange connection will be a similar temperature.

When using free displacement I result in errors about preventing rigid body motion. In conclusion is there a way in ANSYS to focus more on thermal generated stress and not have these boundary condition issues?



Best Answers

  • peteroznewmanpeteroznewman Member
    Accepted Answer

    @hblaine8

    Use two planes of symmetry to hold a 1/4 model of the pipe. That way the flange does not have to be held fixed and is free to expand radially.

    You need just one of the bolt holes to constrain the axial Z motion. Use a Remote Displacement set to behavior = Flexible and only set Z = 0 leaving all others Free.

  • peteroznewmanpeteroznewman Member
    Accepted Answer

    @hblaine8 Go back the the geometry editor.

    If you use DesignModeler, you can insert a Symmetry object and specify 2 planes and it will cut the geometry for you and export the object to Mechanical.

    If you use SpaceClaim, you have to make the planes and use Split Body twice and delete the 3 pieces you don't need. Then you have to add the Displacement Boundary Conditions in Mechanical of zero displacement normal to the cut face, leaving the other two displacements Free.

  • peteroznewmanpeteroznewman Member
    Accepted Answer

    @hblaine8

    You can't use symmetry unless your geometry and your loads area symmetric.

    You can support your flange without adding any stiffness to the model that would cause non-physical stress by using a Remote Displacement. Select all the bolt hole cylindrical faces and create a Remote Displacement. A new node will be created at the center of the flange. That node can have all six DOF set to zero. There are two settings for the behavior of a Remote Displacement: Rigid and Deformable. You must set it to Deformable. Rigid is like Fixed Support and will create non-physical stress.

Answers

  • peteroznewmanpeteroznewman Member
    Accepted Answer

    @hblaine8

    Use two planes of symmetry to hold a 1/4 model of the pipe. That way the flange does not have to be held fixed and is free to expand radially.

    You need just one of the bolt holes to constrain the axial Z motion. Use a Remote Displacement set to behavior = Flexible and only set Z = 0 leaving all others Free.

  • Thank you @peteroznewman

    Would the two planes of symmetry be in the setup or is this something I have to apply in the geometry editor?

    Or if you know of previous documentation about this, that would help a lot too. I am relatively new to ANSYS.

  • peteroznewmanpeteroznewman Member
    Accepted Answer

    @hblaine8 Go back the the geometry editor.

    If you use DesignModeler, you can insert a Symmetry object and specify 2 planes and it will cut the geometry for you and export the object to Mechanical.

    If you use SpaceClaim, you have to make the planes and use Split Body twice and delete the 3 pieces you don't need. Then you have to add the Displacement Boundary Conditions in Mechanical of zero displacement normal to the cut face, leaving the other two displacements Free.

  • @peteroznewman

    My temperature profile I am using is CFD generated and not axi-symmetric. Also, the one of the flanges is not perfectly axi-symmetric. It has 5 inlets on it. 4 90 degrees apart and 1 in-between 2 of the 4. So if I use the symmetry object to specify 2 planes will I lose this information in the analysis?

  • peteroznewmanpeteroznewman Member
    Accepted Answer

    @hblaine8

    You can't use symmetry unless your geometry and your loads area symmetric.

    You can support your flange without adding any stiffness to the model that would cause non-physical stress by using a Remote Displacement. Select all the bolt hole cylindrical faces and create a Remote Displacement. A new node will be created at the center of the flange. That node can have all six DOF set to zero. There are two settings for the behavior of a Remote Displacement: Rigid and Deformable. You must set it to Deformable. Rigid is like Fixed Support and will create non-physical stress.

  • Thank you so much for all of the help! @peteroznewman

  • @peteroznewman The remote displacement seems to have corrected a lot of the non-physical stress. Thank so much again. However, an error arises and I believe this to cause the solver to take a significantly longer time than before. "One or more remote boundary conditions is scoped to a large number of elements which can adversely affect solver performance. Consider using the pinball setting to reduce the number of elements included in the solver."

    Would it be acceptable to only use the circular edges of the bolt holes in the flanges instead of the bolt hole faces to reduce the number of elements? Should I use both sides (upstream edge and downstream edge) of the bolt holes or is there better solution to this issue?

  • @hblaine8

    Yes, use just the circular edges. That should work well and reduce the number of elements in the remote boundary condition. Try it with just one side.

Sign In or Register to comment.