CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   How to join together CFX results and solid parts (http://www.cfd-online.com/Forums/cfx/24654-how-join-together-cfx-results-solid-parts.html)

Giuseppe October 12, 2007 09:20

How to join together CFX results and solid parts
 
Hi there, my name is Giuseppe. I've performed a static simulation in CFX to study the flow rate through a simple tee-tube. The original solid part was in SolidWorks. I've imported it in DesignModeler and then I've created the fluid domain, I've defined the boundary conditions in CFX-Pre and ultimately I've run the Solver in CFX-Solver. The solver told me the simulation has completed normally. Right away I've plotted some results( temperature, pressure, velocity) in the fluid domain by means of streamlines, contours and vectors. This is my question: how could I see these results get together to my part since I've only the fluid domain defined in CFX. Is there a rule of thumb to view results in the solid original domain? Thanks in advance. Giuseppe

CycLone October 12, 2007 15:16

Re: How to join together CFX results and solid par
 
Hi Giuseppe,

There are a couple ways to do this.

1. Invert the suppressed bodies in DM so you have the solid parts active and the fluid domain suppressed. Go back to the Workbench Project page, select your DM model and click New Mesh. Create a coarse mesh on the solid parts, the Automatic method should suffice. Save the meshing database. Now go to Post and load the .cmdb file into your session, making sure you check the "Add to Current Results" box. This will add the solid mesh to your current results. Note that it will also add a copy of the fluid domain mesh that was in the .cmdb file, but you can simply choose not to display it.

2. The next time you set up your analysis, don't suppress the solid parts in DM. You can mesh these along with the fluid domain and load all the meshes into Pre. Within Pre, right click on the Simulation object and turn off creation of the Default Domain. Create your fluid domain selecting only the fluid body (or bodies) and leave out the solid parts. All you meshes will be saved to the .cfx file but only the fluid parts will be passed on to the solver and Post. When you get to Post, do as above but this time load the .cfx file in addition to your results.

Best of luck.

-CycLone

Giuseppe October 13, 2007 14:28

Re: How to join together CFX results and solid par
 
Thanks CycLone, Your advices have been very useful: I've tried the first way you've recomended and it works well. Thanks a bunch.... Giuseppe


All times are GMT -4. The time now is 01:30.