3D Design

3D Design

Pipe with pig

    • gowthamdada
      Subscriber

      Help me to draw this.. how to make a connection with pipe and pig also have to make mesh generation using ICEM CFD. 


      Please find the attachment.

    • peteroznewman
      Subscriber

      I can show you with ANSYS  DesignModeler and Mesh. I've never used ICEM CFD.  You should not care which software generated the mesh if the mesh is the same, and in this simple case, the mesh can be the same. You are using ANSYS 16.0 so DesignModeler should be included with your installation. Please confirm.


      Have you watched Raef's tutorial for how to use a dynamic mesh in FLUENT?  I did and made the geometry attached.



       


       


      In the first image, you can see an inflation layer around the corner of the pig and an inflation layer on the pipe wall. You can also see there are two fluid domains, the inner around the pig and the outer for the rest of the pipe.



       


      Below is the 5m long pig



      In DesignModeler, Sketch3 has a dimension H9 that I set to 25m.  You want 500m but I made it shorter for this demo.



      You can drag and drop a Fluent System onto the Mesh cell of this project and build a Dynamic Mesh model to push the pig along the pipe.

    • peteroznewman
      Subscriber

      I tried to follow Raef's video using the attached file above.  One issue that happened in double precision ANSYS 17.2 (may not happen in 16.0) is that is the mesh is found to be slightly in the -Y space and that generates an error message. The remedy is to translate the mesh upward by a small amount.



      After that was corrected, the next error was a negative cell volume.



      Attached is an ANSYS 17.2 archive, but I can open ANSYS 18.2 or 19.0 if anyone wants to take a look and reply.


      I am trying a smaller element size (10 mm instead of 25 mm) and a shorter integration time.


       

    • Vishal Ganore
      Ansys Employee

      Good start Peter.


      Some comments:



      • Having an inflation layer around a box normal to the flow would make the model more complex and it may not have any significance. You may want to focus on how to make structured mesh with more layers in the gap between pig and wall?

      • For structured mesh, you only need to use layering technique under dynamic mesh setting. Relatively easy to control compared to remeshing. 

      • You could start with the simple 2D case instead of 3D unless it offers you more advantage

      • What are the boundary conditions? Inlet pressure?

      • Pig material properties or mass? You need this data when you set up dynamic mesh motion in Fluent. 


      A quick snap of generating structured grid in 2D. I have just defined a number of divisions for each edge allowing more layers near the top face. You can get started with this model to get the setup and results right in Fluent.



       

    • Vishal Ganore
      Ansys Employee

      Here is the paper describing complete different approach to the problem using explicit dynamics considering friction between pig and wall.  


      http://dr.ur.ac.rw/bitstream/handle/123456789/146/Nshuti%20Rene%20Fabrice.pdf?sequence=1&isAllowed=y


      You might want to do similar.

    • gowthamdada
      Subscriber

      #include "udf.h"


      DEFINE_SDOF_PROPERTIES(projectile, prop, dt, time, dtime)


      {


      prop[SDOF_MASS] = 0.5;


      prop[SDOF_IXX] = 0.0;


      prop[SDOF_IYY] = 0.0;


      prop[SDOF_IZZ] = 0.0;


      printf ("nprojectile: updated 6DOF properties");


      }


       


      Will this UDF enough to move the the above mentioned model? 


      In the dynamic mesh panel, for which part i should consider rigid body? 


      I considered interior-inner-domain as rigid body and interior-inner-domain-outer-domain as rigid body but its still not moving showing error?

    • Rob
      Ansys Employee

      You may need to use non conformal interfaces to allow the pig to move up the centre of the pipe whilst the annular gap remains as a fixed mesh. It's similar to how valve motion is modelled in car engines.  I can't be too specific, but that should give the non-ANSYS part of the community some more pointers to help you. 

Viewing 6 reply threads
  • You must be logged in to reply to this topic.