General Mechanical

General Mechanical

Optimum Mesh for Pipe Flange

    • ayodele1
      Subscriber

      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.

    • peteroznewman
      Subscriber

      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?

    • ayodele1
      Subscriber

      Thanks Peter,


      Please permit me to answer in the reverse order:


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


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


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


      4. Where are the Supports? My responseThe 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 responseI 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.

    • peteroznewman
      Subscriber

      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.

    • ayodele1
      Subscriber

      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.


        

    • peteroznewman
      Subscriber

      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.


       

    • ayodele1
      Subscriber

      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  

    • peteroznewman
      Subscriber

      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.

    • ayodele1
      Subscriber

      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". 


      " alt=""> 


      I await your response.


      Ayodele1

    • peteroznewman
      Subscriber

      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.

    • ayodele1
      Subscriber

      Hello Peter,


      Thanks, I am trying that now.

    • peteroznewman
      Subscriber

      But no luck so far...


      There is a 120 MB file size limit.

    • ayodele1
      Subscriber

      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

    • ayodele1
      Subscriber

      Hello Peter,


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


      Ayodele1.

    • peteroznewman
      Subscriber

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


    • ayodele1
      Subscriber

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

    • peteroznewman
      Subscriber

      Here you go.


    • peteroznewman
      Subscriber

    • ayodele1
      Subscriber

      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. 

    • peteroznewman
      Subscriber

      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.

    • ayodele1
      Subscriber

      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.

    • peteroznewman
      Subscriber

      Create a Coordinate System on a Planar Face. The normal will be the Z axis, the X and Y axes will be in-plane.


      The BC for that face is X, Y Free and Z = 0.


      You need one on each cut face and one on the flange face.

    • ayodele1
      Subscriber

      Thanks Peter!


      I will proceed with this information received.


      Ayodele1.

    • ayodele1
      Subscriber

      Hi Peter,


      I have applied the BCs: the 0 normal on this geometry seem applicable to the Y-axis for the cut plane and the flat (raised) face. I like to know if this setup is correct?   



      Fig 1: BC setup for the cut faces


       



      Fig 2: BC setup for the raised face


      I have applied the BC based on my understanding from your above explanation, Kindly check if I got this right.


      When I tried solving the mathematical problem, I received an error message "An internal solution magnitude limit was exceeded. Please check your Environment for inappropriate load values or insufficient supports.  Please see the Troubleshooting section of the Help System for more information". I have therefore introduced "fixed support" at the back of the pipe, please see below.



      I however have doubt about this arrangement as it appears contradictory to the 0 normal BC I applied to the pipe inner surface. Kindly verify if the application of this fixed support to the outside of this pipe is appropriate?


      I have also applied equivalent "force" load to the internals of this 30 degree slice. I derived the equivalent force load by dividing the force component of the 16 bar pressure into 12 equal parts i.e. F = (P * A) / 12, and applied it directly to the inner surfaces. 



      I wanted to have your comments on the setup prior to further steps.


      I am thankful for your review and comment.


      Ayodele1


       

    • peteroznewman
      Subscriber

      You must set up a Coordinate System rotated by 30 degrees about Y to apply a BC to the face that has a cut angle of 30 degrees.


      You should just apply pressure to the inside face.


      With three faces normal to Y, X and X+30 each with a zero normal displacement, there is no need for a fixed support. Delete that.

    • ayodele1
      Subscriber

      Hello Peter,


      I have created the coordinate systems to the faces (please see below shot) and assigned "displacement BC" to the faces, in which I marked the X, Y axes free, and Z = 0.



      I however got below error messages when I tried running the calculation:


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


      2. An internal solution magnitude limit was exceeded. Please check your Environment for inappropriate load values or insufficient supports.  Please see the Troubleshooting section of the Help System for more information.


      Please can you clarify on how to execute your above recommendation, "setup Coordinate System rotated by 30 degrees about Y to apply a BC to the face that has a cut angle of 30 degrees". I do not know how to carry this out, kindly clarify further?


      I am relatively new to these steps, and indeed appreciate the guidance and support. I await your response.


      Ayodele1


       


       

    • peteroznewman
      Subscriber

      Please attach your archive, it will be easier for me to show you on your geometry.  You only need one Csys for all the faces in the same plane


      1. You can ignore the warning.


      2. You have a mistake in the Csys orientation or the assignment of the Csys in the Displacement BC.

    • ayodele1
      Subscriber

      Thanks Peter,


      I have created 1 Csys for all the faces in the same plane and attempted to correct the assignment of the Csys in the displacement BC, but the Solution was not successful. My archive is hereby attached.


      Ayodele1

    • ayodele1
      Subscriber

      Please how may I attach my archive?


       

    • ayodele1
      Subscriber

      Peter,


      Attached is the archive; thanks.


      Ayodele1

    • peteroznewman
      Subscriber

      Okay, there are two ways to get similar results.


      One way is with three Displacement BC. That is the one named Welding-neck_slice_corrected.


      Another way is to use Symmetry Regions and a Remote Displacement to simulate the bolt head.


      I think you have left a surface out of the Pressure load. That is the flat face inside the gasket surface.


         


      There is potentially a missing load. Is this a pipe or a pressure vessel? If it is a pressure vessel, and you cut the end of the vessel off there is an axial force in cylindrical section to support the pressure on the end face. You need to add that force if it a pressure vessel, but not if it is a pipe.


      You can use a Beta Option to graphically expand the display to get both sides of the hole.


    • ayodele1
      Subscriber

      Thanks Peter,


      It is a pipe actually, and not a pressure vessel.


      I am trying to understand the steps taken, will get back to you.


      Thanks a ton! 


      Ayodele1 

    • ayodele1
      Subscriber

      Hello Peter,


      I have taken a closer look at the 2 options, the approach with the 3 displacement BCs is clearer to me than the use of Symmetry Regions and a Remote Displacement to simulate the bolt head. I however did not see the pressure applied to the flat face inside the gasket surface, which you earlier pointed out. Any reason for this?


      Thanks for your time and guidance.


      Ayodele1. 

    • peteroznewman
      Subscriber

      No reason, I just did one, and while I was doing the other, noticed that the pressure should be on that face also.

    • ayodele1
      Subscriber

      Hello Peter,


      On the approach with the 3 displacement BCs (which you attached above), I can see the 4 edges of the uniform pipe selected for the Edge Sizing 4 mesh definition. I equally found in the Details of "Edge Sizing 4" window "2 edges" were selected for Reverse Bias, which I am not clear about. Kindly clarify on the 2 edges of the geometry to which the Reverse Bias has been applied?


      Thanks for your clarification and guidance.


      Ayodele1

    • ayodele1
      Subscriber

      Good day ANSYS,


      I am applying the above steps to another flange with slightly different dimensions, but have been unable to get past the coarse (initial) mesh. I have been unable to split the below highlighted part of the flange in 3 which I think might be responsible for this challenge, since I have seen this step was implemented on the original flange model. 


        


      I tried meshing without applying Sweep Method to the outer section beyond the flange raised face, but the mesh "failed to initialize" resulting in disappearance of main flange:


         


      Please can someone support me in how to split the main flange body in 3, basically from the outer radius (curve) of the raised face upward?


      The geometry is actually a slice of a 10" flange with a uniform pipe at the end.


      Thank you in anticipation.


      Ayodele1.  

    • peteroznewman
      Subscriber

      Regarding the Bias, you look at the preview and see if it is right and if not flip one or two of the edges until they all bias in the correct direction.


      Regarding the failed mesh, I could work on it now if you attach the file.

    • ayodele1
      Subscriber

      Hello Peter,


      Thanks, I figured out the Bias yesterday after some attempts at it. That's clear to me now, thank you. 


      I am attaching the .scdoc file now.


      Ayodele1 


         

    • ayodele1
      Subscriber

      Hello,


      I trust you can access the .scdoc and the workbench archive files now.


      Looking forward to your support on the split-up of the body for structured meshing, and any other useful information.


      Thanks a ton.


      Ayodele1

    • peteroznewman
      Subscriber

      Look at the two hidden surfaces. These were made using the Blend tool and two edges of the model, then the Pull tool to make them larger. Don't forget to delete those two hidden surfaces or set them to Suppress for Physics so they don't end up in Mechanical.

    • ayodele1
      Subscriber

      Thank you.


      I will delete the hidden surfaces as advised. I observed the 3mm round at the edge of the flange has been removed. Should I reinstate it, or leave it out?


      Secondly, how do you advise I execute my mesh independence, do I increase the number of divisions by 1.5, 1.3 or 1.2? 


      I await your response.


      Thanks a lot.


      Ayodele1

    • peteroznewman
      Subscriber

      I deleted the round because that will interfere with the Hex meshing of that body.


      Mesh independence ratio is better at either 1.5 or 1.3, but if you don't get to a flat part of the curve before you hit the Student limit, it doesn't matter.

    • ayodele1
      Subscriber

      Hello,


      I will proceed as advised; thanks a ton.


      Ayodele1.

    • ayodele1
      Subscriber

      Hi Peter,


      I will post my results once I'm done with the mesh independence.


      Many thanks for your support.


      Ayodele1.

    • ayodele1
      Subscriber
      Good day ANSYS,nI have not been able to obtain an FE solution for this problem - finite element analysis to estimate the maximum allowable working pressure of a nozzle flange. I have tried the 2 proposed methods: (1) Symmetry Regions and a Remote Displacement to simulate the bolt head, and (2) the use of 3 displacement BC. nThe solution however returned the following error messages:nA solver pivot warning or error has been detected in the UZ degree of freedom of node 3111 located in Solid111111. This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues. Check results carefully. You may select the offending object and/or geometry via RMB on this warning in the Messages window.nSolver pivot warnings or errors have been encountered during the solution. This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues. Check results carefully.nI have not been able to proceed with the analysis despite earlier guidance received, due to the above errors/warnings. nPlease how may I fix this problem?n
    • peteroznewman
      Subscriber
      Click on the Solution Information folder. Click on the N-R Residual Plot. The graphics window will show the plot. Reply with a snapshot of that plot.n
    • ayodele1
      Subscriber
      Good day,I have clicked on the Newton-Raphson Residuals under Details of Solution Information window, no plot was shown on the graphics window.nPlease what could I do differently?nThanks in anticipation.nAyodele1 n
    • peteroznewman
      Subscriber
      You have to type 3 where there is a 0 on this line:nthen you solve and there will be a three plots under the Solution Information folder if the solver performed at least 3 iterations.n
    • ayodele1
      Subscriber
      Thank you.nI changed the Newton-Raphson Residuals from 0 to 3 as advised, and tried solving but did not solve. I got below error messages again over the various attempts I made:nNot enough constraints appear to be applied to prevent rigid body motion. This may lead to solution warnings or errors. Check results carefully.nSolver pivot warnings or errors have been encountered during the solution. This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues. Check results carefully.nA solver pivot warning or error has been detected in the UZ degree of freedom of node 3111 located in Solid111111. This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues. Check results carefully. You may select the offending object and/or geometry via RMB on this warning in the Messages window.nSolver pivot warnings or errors have been encountered during the solution. This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues. Check results carefully.nThanks for your response.nAyodele1.n
    • ayodele1
      Subscriber
      Thank you.nI changed the Newton-Raphson Residuals from 0 to 3 as advised, the simulation however appear stuck at 10% and indicating that the Solver is Building mathematical model .... nIt's been in this state for almost 30 mins now; please what could be responsible for this?nAyodele1.n
    • ayodele1
      Subscriber
      Thank you.nI changed the Newton-Raphson Residuals from 0 to 3 as advised, the simulation however appear stuck at 10% and indicating that the Solver is Building mathematical model .... nIt's been in this state for almost 30 mins now; please what could be responsible for this?nAyodele1.n
    • ayodele1
      Subscriber
      Thank you.nI changed the Newton-Raphson Residuals from 0 to 3 as advised, the simulation however appear stuck at 10% and indicating that the Solver is Building mathematical model .... nIt's been in this state for almost 30 mins now; please what could be responsible for this?nAyodele1.n
    • ayodele1
      Subscriber
      Thank you.nI changed the Newton-Raphson Residuals from 0 to 3 as advised, the simulation however appear stuck at 10% and indicating that the Solver is Building mathematical model .... nIt's been in this state for almost 30 mins now; please what could be responsible for this?nAyodele1.n
    • peteroznewman
      Subscriber
      nI suspect you have not rotated Coordinate System 30 deg by 30 degrees so that it is normal to the face.nAlign the view with the Y axis so you are looking down the pipe axis at the flange. Click on that Coordinate System.nDoes the X axis of that coordinate system look normal to the face? I suspect it is still aligned with the Global X axis.nIf so, that explains the problem. That coordinate system must be rotated about y by 30 degrees, not just renamed.n
    • ayodele1
      Subscriber
      Peteroznewman,nThanks, saw that the coordinate sys isn't normal to the 30 deg face, please see below:nHow do I rotate about Y at 30 deg for my X to be normal to that face?nThanks in anticipation.nAyodele1n
    • peteroznewman
      Subscriber
      When you click on a Coordinate System, the ribbon has a Coordinate System tab. On that tab are buttons. Use the Rotate about Y button and type in -30.n
    • ayodele1
      Subscriber
      Hello ANSYS,nMany thanks: I have rectified the Normal orientation of the Coordinate sys as advised, please see below:nFig 2: Application of the Coordinate Sys_30 degnI have also attempted to solve, there was an error displayed:nNot enough constraints appear to be applied to prevent rigid body motion. This may lead to solution warnings or errors. Check results carefully.nThe solution has also not advanced beyond 10%. It says Building Mathematical Model ... and is being in that state for long now.nThe N-R Residuals had been changed from 0 to 3 to see the 3 plots under the Solution Information folder, I however haven't seen any plot.nPlease what should I do next to resolve this issue?nThanks in anticipation. nAyodele1n
    • ayodele1
      Subscriber
      Hello ANSYS,nThe issues have been resolved, I now have a solution.nThank you.nAyodele1nn
    • ayodele1
      Subscriber
      Dear ANSYS,nPlease can you clarify on how I may enter a temperature for my FEA solution. I am to use 115 degC in my simulation. I have updated this under Environment temperature on the Static Structural window, but the results remain the same as the default environment temperature. Kindly provide guidance on what I need to do?nThanks in anticipation.nAyodele1n n
    • peteroznewman
      Subscriber
      With no thermal load and none of the materials having temperature dependent properties, the Environment temperature will have no effect on the solution. nPlease select one of my replies above to mark as the solution or Accepted Answer to your original question. nOpen a New Discussion to ask about thermal loads and environment temperatures.n
    • ayodele1
      Subscriber
      Thank you.nI will open a New Discussion to ask about thermal loads and environment temperatures.nPlease how do I select your previous response to mark as the solution?nAyodele1n n
    • peteroznewman
      Subscriber
      nI just learned there is a difference between clicking New Discussion and clicking Ask a Question.nYou only get to mark items that show up as Answers when you started a thread using Ask a QuestionnIf you started a thread using New Discussion, then there is nothing to mark.nIt is best to keep a thread on topic and not to stray too far from the original post. That is why it is best to start a new thread.nIf you are asking, then Ask a Question. A thread that is trying to teach something would be best as a New Discussion.n
    • ayodele1
      Subscriber
      Thanks immensely. I'll take note of that.nAgain, thanks for the support.n
Viewing 68 reply threads
  • You must be logged in to reply to this topic.