- **CFX**
(*https://www.cfd-online.com/Forums/cfx/*)

- - **EMAA flow/expansion simulation**
(*https://www.cfd-online.com/Forums/cfx/97531-emaa-flow-expansion-simulation.html*)

EMAA flow/expansion simulationHi
I'm trying to model and measure the change in diametre of EMAA thermoplastic under pressure and with respect to time. In my domain, I modelled a plate pushing down at a certain force for 30 minutes against a melted EMAA fluid disc in double symmetry. The plate is modelled as a rigid body and since the plate is moving, it is a transient moving mesh problem. Currently, i've been running the model for two full days. The simulation time is only at 0.1s with steptime hovering around 7x10^-6. I've defined steptime as adaptive with max coefficient loops at 10. The mesh at the moment is rather course with only about 130000 elements. I used Patran to mesh. The simulation is running on i5-2400. Besides using a faster computer and multiple computers, is there anything I could do to speed up the simulation? Are there any settings that I can change? Thank you. http://img855.imageshack.us/img855/3446/12713full.png Regards, eugenec |

Why have you used 2 symmetry planes? Does the flow have 2 symmetry planes or is it actually a 2D axisymmetric flow? If it is 2D you will save heaps of time by running it 2D.
Also your mesh is triangular in the plane shown. Why did you do this? If a hex mesh will work you should use that. When you are checking the run is working feel free to use a very coarse mesh, just with enough detail to vaguely capture the effects you are looking for. But as soon as the physics is working you should do a mesh refinement study to establish exactly what mesh size you require. The choice of mesh size is very important - too coarse and your results will be rubbish and too fine and the simulation will never complete in your life time. |

Hi Glenn
Thank you for your reply. The fluid disc which I want to see flow under applied pressure is an axisymmetric problem. I've tried modelling in 2D. However, the results doesn't seem to reflect my experimental results of the same problem. I had doubts about the 2D simulation properly reflecting the physics of the problem and therefore decided to try modelling it as a quarter disc with double symmetry. http://img401.imageshack.us/img401/5122/1251full.png While modelling in 2D, I also had negative element volume problems with the mesh around the edge of the plate. Initially, I was using quad elements but that gave me alot of mesh problems. The triangle elements delayed mesh problems. |

Triangular elements are not a good fix for folding mesh problems. You should go back to hex meshes and fix the folding mesh problem. Also, if you expect the flow to be 2D axisymmetric you should model it 2D axisymmetric.
Can you describe the motion the mesh goes through? |

Using the pictures from my second post as an example, the plate (the void in the middle) simply moves in the -ve Y axis due to a downwards Y force which I've applied onto the plate. The plate is defined as a rigid body. As the plate moves downwards due to the applied force, the EMAA plastic fluid should 'compress' and spread out in the x axis.
So the mesh above the plate is expanding while that beneath is being compressed. Negative mesh volume always happens at the 90deg edges of the plate. Especially at the lower corners. Instead of having a plate compressing down onto a fluid, can I simulate this with a single rectangular 2D domain in the XY plane with the 'top wall' moving down? Essentially, the domain volume becomes smaller? |

Why do you need to model the edge and top of the plate? Does the plastic go beyond the plate edge? Or does the fluid is displaces (air?) have a significant effect on things?
Assuming that you need the region at the edge of the plate (see above questions), rather than do this as a single moving mesh domain I recommend you have a fixed domain outside the plate and a separate moving mesh domain above and below the plate. You then connect the domains with GGI interfaces. Hey presto, no folding mesh :) And don't forget that if the flow is 2D you should model it as 2D. |

Well, actually for now, I don't need the area around the edge and above the plate. All I require to model for a start is the volume beneath the plate. Basically, just a rectangular 2D volume with the top wall pushing on the plastic. The thickness of the plate is not critical at this stage. And the plastic does not flow beyond the edge.
If I were to model with the volume around the edges and above the plate, are you saying that I should create 2 subdomains and 1 domain where the left and right volume around the plate is one subdomain, the are volume above the plate is another subdomain and the volume beneath the plate is the main domain? I then define the subdomain at the plate edge as stationary mesh and link all domains with GGI interfaces? |

I would probably put the top, bottom and edges all as separate domains for a total of three domains. But you could use sub domains if you like.
But sounds like you can model it in 2D with a simple rectangular mesh. You should have no mesh folding problems with this. But use hex elements, not tets. |

I've gone on to model my problem in 2D.
As the top wall moves down to compress the plastic, the thickness of the plastice changes but does not spread out / flow in the x-axis. I am unsure what is going wrong here. How can the volume of the plastic be lost as the thickness changes? The top wall is defined as a rigid body and no slip wall. The bottom wall is no slip wall. The left and right walls are openings with 0 relative pressure. http://img687.imageshack.us/img687/2782/24435465.th.png http://img594.imageshack.us/img594/6219/77882193.th.png |

hi
the right wall should be a symmetrie boundary. If you have an opening you get a outflow. |

Hi Frank
http://img692.imageshack.us/img692/8199/4525full.png Uploaded with ImageShack.us The whole 2D domain looks something like this. So I don't think I should define the right wall as a symmetry. Still not sure why the volume is missing as the top wall moves down and the domain changes size. :( |

It should be a routine bug-finding exercise to fix this.
* Have you checked the air is escaping out the ends as it should? * If you are modelling this in 2D have you put symmetry planes front and back? * Have you checked you are modelling the free surface flow? Have you done the tutorials on free surface flow? * Is your simulation sufficiently converged? Especially the second point - that would explain what you are seeing. |

All times are GMT -4. The time now is 23:19. |