How to map Fluid Pressure data at Node into Pressure B.C ?

[feelsoogod]

Hi.

I completed CFD analysis in fluent s/w, and want to use its Pressure data at Node as B.C which should be applied to element surface.

How to map Fluid Pressure data at Node into Pressure B.C ?

Any ideas will be very grateful.

Thanks.

 

[cbrn]

Hi,
unfortunately, you have to write a routine in order to interpolate the Fluent data into your FEM's model nodes.
As a general idea, you should:
1- read the Fluent output file node by node, and get the set of data "node number - coordinates triad - pressure value"
2- make a selection in your FE model in order to "isolate" the nodes nearest to the one currently read
3- interpolate the values based on the distance and on the already attributed values
4- repeat iteratively on all the nodes, and possibly make more than one complete "pass" (i.e. either specify the number of "passes" you want, or the maximum nodal value's change between one "pass" and another)

All this is because CFD mesh and FE mesh are hardly exactly identical (oh, well, if you have the opportunity to get a nodal coordinates file and an element definition file from Fluent, then have your FEM read them in and you're done!).

Hope this helps...
Regards

 

[feelsoogod]

Hi, cbrn !

I intentional meshed CFD mesh(Volume mesh) and FE mesh(Surface mesh which include the Volume mesh) as exactly identical at Surface Region. So, I have no problem in getting Pressure data at Node. But, in general, The pressure loading should be applied to Element Surface.

Thanks anyway.

 

[johnhors]

feelsoogod (is that a miss spelling of feelsogood?)

What FE system are you using? Because few FE solvers allow you to specify a variable nodal pressure on an element face, I know Lusas does with ease, Nastran can but with difficulty, but the vast majority only allow a uniform pressure to be applied. Otherwise you will have to convert your pressures into equivalent nodal forces. To do that correctly you will have to get involved with element shape functions!

 

[feelsoogod]

Hi, johnhors!

I use i-deas nx for FE analysis. It seems that I'd better make input file using Lusas or nastran, and export to i-deas nx solver. This is what I looking for.

Thanks, johnhors !!!

 

[cbrn]

Hi,

I recognize that this small contribution on the topic can be of little help at this point, but this is only a very general suggestion:
very few FE systems, as Johnhors says, can apply different pressure values at the corner nodes of an element face; BUT, one should check that his FE doesn't have a way to apply "tapered pressure" over an element face. For example, in ANSYS, if you try to directly assign pressure to nodes with the SF command, the effect will be that uniform pressure will be applied to the elem face(s) described by these nodes; BUT, if you first fill-in an adequate table of values, and issue the SFFUN command before the SF one, then, "magically", tapered pressure distributions will be mapped over the elements' faces...

Regards

 

[freiFEM]

Hi feel,

I would do it in NASTRAN. As Johnhors said, it is difficult to apply variable single pressure value on different elemental surface.But what i would do is, observe the range of presuure values in CFD and apply the same range in your FE model by selecting for each range some group of element. With the layers and element groups i hope it would be not so difficult in NASTRAN and may be this idea helps to you.

good luck.

Tobias.