CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FloEFD, FloWorks & FloTHERM (http://www.cfd-online.com/Forums/floefd-floworks-flotherm/)
-   -   Query regarding temperature distribution in Solidworks flow simulation (http://www.cfd-online.com/Forums/floefd-floworks-flotherm/112902-query-regarding-temperature-distribution-solidworks-flow-simulation.html)

 syarif February 7, 2013 08:15

Query regarding temperature distribution in Solidworks flow simulation

Dear all,

I am Syarif, engineering student and new to this forum and this software. I am hoping that I can get some suggestion and idea for Solidworks flow simulation.

Currently, I am simulating a cold chamber. My aim is to observe the temperature distribution inside the chamber due to difference design. I was wondering, for flow simulation, is there any built in tool that I can use to evaluate the temperature in specific region/or area? I know that I can use cut plot or surface plot to plot the temperature distrbution, but here I am interested in 3d area (volume) rather than 2d plot.
Can anyone advise me if it is possible in Solidwork flow simulation? If possible, can I extract the data to excel?

 Boris_M February 18, 2013 12:31

Hi syarif,

you can use isosurface which represents the a 3D surface of a specific temperature. So for example if you look at -10°C surface it will show you the surface where this temperature is and if you plot another surface of -15°C for example, you will be able to see on which side of the first surface it is colder. Or use one of the other plots to see on which side it is.
You can plot kind of a volume if you use the isosurface and the surface plot for the room walls and limit the room walls plot scale to the max or minimum of your isosurface. That way you will have for example the surface plot going from -10°C to your coldest temperature for example -23.6°C and you can select the values on the scale that are out of the defined limits to be transparent. This way you get colors from -10°C to -23.6°C but not above -10°C, here there are no plots on the surfaces of the room and with your isosurface beeing -10°C you will get a surface in the 3D room volume to close the volume plot.

Any export for excel are either surface values on solid surfaces like the room wall or defined volumes such as the wall volume or as points on a plane or a surface with the point parameters. You can create some planes and then use a point distribution of either a equally spaces number or define the spacing by a value. That way 10 planes with a spacing of 10cm and on each a point parameter with a defined spacing of 10cm between the points will give your a well defined grid.

Boris

 syarif February 22, 2013 16:35

Hi Boris,
Thanks a lot for the brilliant suggestion. I really forgot about the isosurface function. However, I am still unclear how you can combine the isosurface and surface plot to get the 3d volume? Could you please kindly explain to me a little bit deeper?Also I am quite unclear on your explanation on the exporting the value to excel. Do you meant we need to create fixed planes of the volume that we want and extract the value at the specific points?

 Boris_M February 27, 2013 06:22

the 3D volume is relative simple:
- Create a surface plot of the room walls and set either min or max values of the scale to the value you want the isosurface to be. For example if you want to see the volume of air that is colder than 10°C then use max value as 10°C and min value as the minimum plot value.
- change the plot color bar settings by double click on the color bar and change the out of range settings to transparent. That way everything above 10°C is transparent and the walls below 10°C are colored according to the color bar.
- create an isosurface with the temperature of 10°C which will give you the closing surface of the 3D volume that lies in the fluid.

With that the surface plot will close the volume that is in contact with the wall and the isosurface as the surface of the 3D volume that is in the fluid.

For the 3D data in Excel:
- create a "Point Parameter" and select the type to be "pattern".
- select a reference plane (e.g. the room wall on the one side) and select spacing as option to place the points to avoid any more or less random distribution of points in the volume but to give a fixed spacing between the points.
- then select the parameter you are interested in and click "export to excel".
-repeat this but with increasing offset to the selected reference plane or wall. Ideally you probably want to have the same offset as your point spacing is in each definition. For example if you spacing of the points is 10cm the your first plane will be directly on the wall, the next will have the offset of 10cm and the next then 20cm etc. that way you get a discretization of the room results in 10cm steps in all three coordinates.

Another option but way more linked to the mesh size is to use the feature in the result tree "Mesh".
- Here you put the "Mesh" on "show" to get into the menu of this feature.
- Then select which cell type you want to get the values from (e.g. fluid cells) and select the output option (Excel in your case).
- Under "output" you can select the location where this file shall be stored.
- under "Parameters" you have to select the parameter you want of course.
- and in region you can narrow the region of the computational domain to the area you want the data from.
- and finally under transient you can also select the time steps you want to have the results from but you will need results for these time steps, or better said, it will only show you the time steps to select from of which you have result files.
Then click ok or apply and your file will be created.

Be aware that you will get the value of each cell, from large to small and therefore also a none equal spacing as the cells when the get smaller the values and their coordinates get closer to each other, so not constant 10cm as mentioned in the other method.
Also for both methods it may take some time for getting the data into Excel depending on how many data point will be created.

I hope this helps,
Boris

 All times are GMT -4. The time now is 02:14.