Boundary condition in Static structural Analysis

Dear Ansys Community,

I am conducting a thermo-mechanical simulation on the attached model below. For the stress analysis due to thermal loading, I need to apply support at the bottom surface, such that no stress is being developed there due to the support. Because in the oven we just place the specimen and not fix it. So please help me how to apply the BC. 

I tried

1. applying remote displacement on to the edge of the bottom surface fixing in all DOF. But that works only for a single thermal cycle. If more cycles of thermal cycle exists, stress concentrates on the edge and unlikely deformation is being seen. 

2. I also tried the combination of remote displacement on edge and frictionless support on face. But still unlikely deformation is happening. 

Please help me how to fix this issue ie, how to give boundary conditions  at the bottom without stress concentration at the fixed region.

 

Thanks in advance

Best Regards

Praveen

«1

Comments

  • Praveen95Praveen95 Member
    edited June 2020

    Hello,

    Please anyone guide me

    Best Regards

    Praveen

  • peteroznewmanpeteroznewman Member
    edited June 2020

    ANSYS staff are not permitted to open attachments. Please use the Insert Image button to put screenshots into your post.

    Take a radial slice and convert this to an axisymmetric model, assuming the temperature load is uniform.

    The axis of symmetry is the Y axis and the geometry is drawn on the +X side.

    Apply a Displacement constraint on one vertex on the axis, setting X and Y to 0.

     

  • Praveen95Praveen95 Member
    edited June 2020

    Dear Peter,

    Thank you for your reply.

    Please see the above images.

    The model consists of two parts as in figure1. Outer mould covers the inner Metal inlay. The metal inlay is not uniform through out. Inner metal has a ramp (out of plane bend) as you can see in the figure 2. So, in this case, I think you won't suggest using axisymmetric model. 

    In this case how to constrain free of stress?

    Best Regards

    Praveen

  • peteroznewmanpeteroznewman Member
    edited June 2020

    Yes, that information excludes axisymmetry.

    In that case, select one circular edge and apply a Remote Displacement with it set to Behavior = Deformable, which won't add any stiffness.

    Then set the remote displacement to have 0 in all six degrees of freedom.

  • Praveen95Praveen95 Member
    edited June 2020

    Dear Peter,

     

    Currently, I am using remote displacement at the edge (with DEFORMABLE as the behavior) as described by you Peter. But normal stress in Z direction is concentrating there, if I apply 22°C to 180°C to -40°C to 180°C to -40C to 22°C and then perform stress analysis. Also, the material bulges inward at the face enclosed by this edge applied with zero remote displacement. It is as shown in the figure. Also, unlikely plastic strain more than 30% is being shown. SO I thought the BC is not correct and It should be applied all over the face instead of edge.

    Best Regards

    Praveen

     

     

    .

  • peteroznewmanpeteroznewman Member
    edited June 2020

    I see that is not working.  I don't know if there is an option in APDL to assign the CTE to the elements created by the Remote Displacement. That would work.

    Here is a more involved, but perfect solution. 

    First create a Cylindrical Coordinate System at the center of the face, with Z normal to the flat face.

    Then create a Displacement using the Cylindrical Coordinates that has X = Free, Y = 0 and Z = 0.

    In the Cylindrical system, X = R,  Y = Theta and Z = Z.

    Select 3 Nodes, at approximately 120 degrees apart.

    If you want this to be independent of the mesh, then you have to go back to CAD, and slice the body up to create the three vertices and use those instead of nodes.

  • Praveen95Praveen95 Member
    edited June 2020
    Dear Peter,

    I would try this and let you know.

    But I would also want to tell you that, before using remote displacement method. I used to select three different nodes at 120degrees apart and then constraining each node on one direction or two directions and tried some combinations. But there was stress concentrations at these points.

    Is using cylindrical coordinate system works differently than what I described?

    Best Regards
    Praveen
  • peteroznewmanpeteroznewman Member
    edited June 2020

    Yes, cylindrical coordinates are required to allow a circular form to freely expand radially, because the radial (X axis) constraint is Free.

    You still need to provide six constraints, so three Z axis constraints and three Y axis (theta) constraints provides a grounded static support.

    This constraint pattern is equivalent to three balls in three Vee channels arranged in a 120 degree pattern.

  • Praveen95Praveen95 Member
    edited June 2020

    Dear Peter,

    Thank you for the detailed explanation. 

    I created a cylindrical CS with origin at the center of the face and is as shown in the figure

    I also created a named selection of the 3 nodes approximately 120° apart. It is as shown in the figure

    But during the displacement, I can select the cylindrical CS. But I cannot select the named selection of the 3 nodes or I cannot directly select the 3 nodes. I can only select the face.  Also, I cannot see the 6 constraints to enter 0. 

    Should I do something with the APDL command to achieve what you said.

    If there is any documentation, please let me know.

    Thanks alot

    Best Regards

    Praveen

  • peteroznewmanpeteroznewman Member
    edited June 2020

    I almost never create Boundary Conditions on nodes, since they are not persistent when I remesh, so I don't know what to do there. Did you try picking just one node?

    Instead of nodes, make some vertices in the Geometry. Note that the three points don't have to be at 120 degrees. You could do three points at 90 degrees.

    Open the geometry in SpaceClaim or DesignModeler, create two (or three) planes.

    Slice the bodies into three parts, and put the parts into a Multibody part using DesignModeler or use the Share button on the Workbench tab in SpaceClaim to create Shared Topology.

    Now you have three vertices that you can apply the displacement boundary condition on in the cylindrical CSYS.

  • Praveen95Praveen95 Member
    edited June 2020

    Dear Peter,

    Did you mean like this:

    It is actually working better than the previous.

    But, I have few doubts Peter

    a. Does the above setup create Moment? Because, if I see the deformation plot, the vectors show that torsion is acting. So does this mean that the vertices should be equidistant and  in equilibrium?

    b. Also, I divided the outer Body into three parts by hiding the inner metal part. I then clicked shared topography. Will this physically divide the body into 3 parts. If so, does that not create any effects on the stress and strain values?

    c. Stress is concentrating slightly in these regions as shown below even though maximum is not lying there (that's a good sign). Is it because the mesh is too coarse?

     

    I think these answers will definitely clear all my doubts.

    I really appreciate for your quick replies?

    Best Regards

    Praveen

  • peteroznewmanpeteroznewman Member
    edited June 2020

    Don't use the center point because the theta direction is undefined at r=0.  Use the three points at the same radius.

  • Praveen95Praveen95 Member
    edited June 2020

    Dear Peter,

     

    Sorry I was editing the post.

     

  • peteroznewmanpeteroznewman Member
    edited June 2020

    I suppose you could use the center point, but the constraint in the cylindrical CSYS would be X=0 (means R=0) and Z=0 leaving Y free.

    Three points around a circle with the cylindrical DOF of Y(theta) = 0, Z = 0 and X(radial) = Free is a kinematic constraint. That means in the absence of gravity or any other applied force, for just thermally induced deformation, zero reaction force and zero reaction moments go through the constraints.

  • peteroznewmanpeteroznewman Member
    edited June 2020

    Slicing the outer body, then using Share will cause the slice lines to imprint on the inner body.  The meshes all remain connected with no need for contact elements.

  • Praveen95Praveen95 Member
    edited June 2020

    Dear Peter,

    I didnot understand this. Do you mean,

    a. should I slice the outerbody keeping the innerbody active?

    b. or do you mean, that the contact between outer and inner body which is defined is not necessary?

    c. or do you mean, the sliced parts of outerbody will be in contact automatically

    If I keep both the bodies active and slice the body, I cannot save because, space-claim tells the number of faces crosses 300 (as inner body has unmerged faces). Due to this I hide the inner one.

     

  • Praveen95Praveen95 Member
    edited June 2020

    Dear Peter,

    If I apply the displacement BC only on the 3 vertices with same radius without applying anything at the middle, it shows 

    Not enough constraints appear to be applied to prevent rigid body motion.  This may lead to solution warnings or errors.  Check results carefully.

    So, is it forcing us to constrain even at the center?

    Thank you

     

  • peteroznewmanpeteroznewman Member
    edited June 2020

    That is just a warning. You can ignore it because you know that there are exactly six constraints which is the perfect number for a kinematic connection to ground.

  • peteroznewmanpeteroznewman Member
    edited June 2020

    a. You can slice the outer body only and do nothing to the inner body.

    b. No contact is necessary.  Delete any automatically created contact.

    c. In SpaceClaim, on the Workbench tab, click the Share button. Instead of contact, the bodies will share nodes on coincident faces.

    Yes, you have to stay under the 300 face limit.

  • Praveen95Praveen95 Member
    edited June 2020

    Dear Peter,

    As suggested by you, I have clicked the Share button and  I suppressed the contact defined. It showed solver pivot error. Again I unsuppressed the contact that is automatically defined, now it is running properly.

    The displacement defined is as shown in the figure.

    I will let you know once the run is completed.

    Thank You

    Best Regards

    Praveen

Sign In or Register to comment.