×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

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

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

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

(OP)
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.

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

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

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

(OP)
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.

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

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!

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

(OP)
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 !!!

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

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

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

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.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources