Optimum Mesh for Pipe Flange

Hello ANSYS,

Please I need guidance on best approach to mesh below geometry. My results are still changing while the Tet elements count is already 31,501. The internal of the geometry shown below also show minimal nodes present, but I am unable to refine further due to the limit already reached. Please is there a more efficient method of meshing this geometry (i.e. flange)?

Mesh internal 

I tried the Multizone method earlier but received "Multizone blocking decomposition failed" error, the Hexa-dominant method also gave me over 40,000 elements. 

Thanks a lot for your support.

Ayodele1.

«134

Comments

  • peteroznewmanpeteroznewman Member
    edited July 5

    Optimum mesh depends on details of the analysis.

    Is it possible to use symmetry?

    Where are the Supports?

    Are there any other parts/contact?

    Where are the Loads?

    What is the purpose of the analysis?

  • ayodele1ayodele1 Member
    edited July 5

    Thanks Peter,

    Please permit me to answer in the reverse order:

    1. What is the purpose of the analysis? My response: I am carrying out finite element analysis and to estimate the MAWP (maximum allowable working pressure)

    2. Where are the Loads? My response: The load is Pressure load, 1.6 MPa. Please see below for how I have applied it.

    3. Are there any other parts/contact? My response: There are no other parts/contact I'm modelling

    4. Where are the Supports? My response: The supports are at the point where it will be connected to adjoining pipelines, the raised face of the flange and the point at which it will be welded (please see below).

    5. Is it possible to use symmetry? My response: I wanted to explore the current geometry before attempting to use symmetry by re-creating the geometry in half. 

     

     Thanks a lot for your review and support.

    Ayodele1.

  • peteroznewmanpeteroznewman Member
    edited July 6

    The supports are not correct for this model. The two faces marked as Fixed Support are not, in reality, fixed. The flat face on the flange should be free to expand radially about the flange center due to the pressure. Delete the Fixed Support.

    Create two planes of symmetry to correctly support this geometry. One plane is through the axis to cut the geometry in half. The second plane is through the axis at an angle to the first plane. The angle could be 90 or 60 or 30 degrees, but let's use 90 because it is easy. So now you have a quarter model. The two cut faces and the flat face of the flange are each given symmetry boundary conditions, that is, the translation normal to the face is set to 0 while the other two in-plane displacements are Free. With that arrangement of support, the applied pressure is free to cause a radial expansion of the 1/4 model of the flange.

    The face that is welded to a uniform pipe section should have a 1/4 uniform pipe added, to a length of at least 4 pipe diameters.

  • ayodele1ayodele1 Member
    edited July 6

    Hi Peter,

    Many thanks for the guidance. As advised, I have created the 1/4 model of the flange and added a pipe length of 40", because the flange diameter is 10". However, the number of elements generated now is about a million, which I am unable to solve now.

     

    Should I reduce the pipe length to twice the internal diameter of the pipe?

    What may I do to bring the element count of this model within the 32,000 limit?

    Thanks a lot for your support.

    Ayodele1.

      

  • peteroznewmanpeteroznewman Member
    edited July 6

    Maybe cut the pipe length down to 20" instead of 40".  As I said above, you can get a proper solution on a 30, 60 or 90 degree slice. You can cut the model size down by making a plane at 30 degrees and using Split Body then you can discard 2/3 of the geometry.  You will need to make a Coordinate system on that 30 degree face so you can make a Displacement BC on that face to set displacement normal to that face at 0.

    You need to use a structured mesh. Open the Geometry in SpaceClaim, add a plane to slice the uniform pipe at the taper that begins the flange. Use the Split Body button on the Design Tab to split the body into two pieces. Then on the Workbench tab, use the Share button to have the mesher reconnect the two parts.

    Now in Mechanical, assign a Mesh control Method = Sweep on the pipe. Pick the inner face of the pipe as the Source Face, then you can assign 2 elements for the number of elements in the sweep direction. You can then put a Face Meshing control on the inner face of the pipe. Finally, you can assign Mesh sizing controls on the four edges of the inside face of the pipe to set the number of elements around the 1/4 circle and a different number of element along the length.

     

  • ayodele1ayodele1 Member
    edited July 7

    Hello Peter,

    Thank you for the support.

    I have not been able to carry out the steps in your second paragraph, I get "Unable to cut body" error message after I created the plane by clicking the plane button on the create section of the design tab, and going on to click the Split Body button, then selecting the edge at the taper where the flange begins. Please, what I'm I doing wrong?

    Thanks a lot for your time and guidance.

    Ayodele1  

  • peteroznewmanpeteroznewman Member
    edited July 7

    Move the plane a few wall thickness away from the taper and try to Split Body. That should work. If it doesn't please attach the .scdoc file to your reply.

  • ayodele1ayodele1 Member
    edited July 7

    Many thanks Peter.

    I couldn't get it to work, as there is no line after the taper on the uniform pipe. I tried attaching the .scdoc file, but replied "only JPEG, PNG and GIF images can be uploaded". 

    image

    " alt=""> 

    I await your response.

    Ayodele1

  • peteroznewmanpeteroznewman Member
    edited July 8

    Don't use the Insert Image button on the toolbar of the Post.  Click the Add Post button, then on the list of buttons on the right side after the post appears, the Attach button will show up.

  • ayodele1ayodele1 Member
    edited July 8

    Hello Peter,

    Thanks, I am trying that now.

  • peteroznewmanpeteroznewman Member
    edited July 8

    But no luck so far...

    There is a 120 MB file size limit.

  • ayodele1ayodele1 Member
    edited July 8

    Hi Peter,

    Indeed, there hasn't been luck so far. The file size is actually 117KB, so really should get delivered. I haven't seen the Attach button on the RHS of the post, it isn't showing up.

    Ayodele1

  • ayodele1ayodele1 Member
    edited July 8

    Hello Peter,

    I suppose you can see it now, thanks a ton. I look forward to your response.

    Ayodele1.

  • peteroznewmanpeteroznewman Member
    edited July 8

    Is the highlighted ring a gasket or a solid part of the flange?

  • ayodele1ayodele1 Member
    edited July 8

    A solid part of the flange actually. It's the raised face of the flange, where the gasket seats. 

  • ayodele1ayodele1 Member
    edited July 8

    Thanks a ton!

    Please for my learning, may I confirm the following:

    1. This appears to be the 30 degree slice, please did you achieve this by carrying out the particular steps in the first paragraph of your instruction to me?

    2. What length of pipe I'm I finally using?

    3. Why couldn't I move the plane a few wall thickness away from the taper and try to Split Body as advised?

    4. Did you execute the steps in the third paragraph to obtain the above mesh, are there other steps taken?

    5. I presume I am to proceed to define my boundary condition (b.c.) in Mechanical, please what b.c. should I apply to which face?

    Thanks for your guidance and support.

    Ayodele1. 

  • peteroznewmanpeteroznewman Member
    edited July 8

    1. Yes a 30 degree slice. There are many workflows that lead to this slice.

    2. I did it by eye. You can use the Measure Tool to find out.

    3. I don't know, when I picked the circular edge to create a plane, that plane split the body without issue.

    4. I did that and more. I will upload the Workbench Archive with the mesh where you can see all the pieces.

    5. Minimum BCs are 0 normal to each cut face, and 0 normal to gasket. The in-plane constraint is Free.

    Later you might want to model the bolt holding this flange to another flange.

  • ayodele1ayodele1 Member
    edited July 8

    Many thanks, Peter.

    I can see the steps taken to create the structured mesh in Mechanical, thanks for sharing this.

    Please what does the 0 normal BC mean, and the in-plane constraint being Free?

    Ayodele1.

Sign In or Register to comment.