CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Aerothermoelastic effects using MFX (http://www.cfd-online.com/Forums/cfx/75651-aerothermoelastic-effects-using-mfx.html)

aerothermoelastic May 2, 2010 01:47

Aerothermoelastic effects using MFX
 
Hey,

So I'm trying to do a combined aerothermoelastic analysis of a panel using MFX. Now earlier I was doing a standard aeroelastic analysis of the same panel with no problem via the workbench, however the workbench does not support a combined thermoelastic analysis.

After looking around I found that there is an element in the mechanical editor(Solid226) that supports thermoelastic analysis, so I remeshed the geometry in the mechanical apdl using it, and the procede to follow the instructions laid on in section 4 of the APDL help. However, when I go into CFX and give it the generated dat file, it refuses to acknowledge the presence of the defined interfaces.

Now looking in the dat file, I see that while it seems to define the transfers, no where does it seem to define the interfaces using the SF command. Now I'm wondering why doesn't the mechanical APDL do this when I tell it to generate the input file, and how can I change this?

BTW, I'm a grad student in aerospace engineering and I'm doing this for a class project.

Ok more details on what i did:

So in workbench I create a mechanical apdl and open it up.

In ansys I import the geometry which is stored as a .sat. Simple panel, longer then it is wide.

Import material properties, AL-2024 and the element type im using(Solid226). Also add the desired dofs.

Mesh the geometry using the standard tool. I tell it to sweep it with auto selection of the source and target.

I add the structure bcs, setting the displacements at the ends of the panel to zero. Also under the loads I open up the field surface interface and apply it the the appropriate area. Looking back at section 4.2 in the apdl help, I think I might be doing something wrong here, since according to what I printed out there is also a 'fluid/ansys' option, although that sounds like ansys' internal flow solver.

Now I go to the multifield tab. Turn on the multifield. Tell it to solve the system in series with cfx first since the panel basically just sits there, at least for now.

Then I tell it where and what data to transfer between the two fields. I just use the pre-defined choices, thermal and mechanical. When I look inside the dat file, these commands show up, strangely before the actually mesh information. Again, no SFA commands in the dat file.

After that i set up the time commands with a time step size of .05 and a total time of 1 second. I might increase this if I get it to work.

I don't do anything with the mapping options between the two fields or with the staggering options.

I do set the convergence criteria in one of the directions to be one, since it's basically a 2d problem so I dont want to running computions in the infinite direction.

Then I tell it to write and after looking at the lack of results in cfx, bang my head in frustration.

Any help would be appreciated. If anyone thinks pictures would be helpful I can provide them tomorrow morning.

Any help would be appreciated,
Danderson

aerothermoelastic May 2, 2010 18:45

It's working
 
Ok, so I got it to work. I had to abandon using the mechanical apdl. Instead I took the .dat file generated inside the workbench for the aeroelastic problem and edited it so that it used solid226 instead of the default, I think solid186 or so. Also I changed the cfx file so that the heat transfer at the fs_interface was also included in the multifield analysis.

Pocket May 5, 2010 02:57

Welcome to my world of hurt :cool:

Yes, i too write the input file from the structural solver in workbench and then change the element to 226 (227 for tets) with keyoptions (1) = 11 and (2) = 0 [11 = thermal and structural degrees of freedom, 0 = strong coupling]

When you load the modified file into CFX (Ansys 12.0 or 12.1) you can choose the thermal and structural coupling from the dropdowns in the "Wall"->Boundary Details

Be careful with your structural boundary conditions though!
If you create a fixed support, the thermal degree of freedom will be fixed as well to 0[C], which is bad :eek:

Unfortunately, it seems the temperature needs to be fixed in a three dimensional way at some place, therefore i began to put a thin pivot at a relatively central point and extrude it in the third dimension (running pseudo-2D, too). At the end of the Pivot, i fix all displacements to zero (d,all,ux,0,,,,uy,uz) and the temperature to room temperature (d,all,temp,22) manually in the input file. This temperature fixing is necessary to prevent "rigid body motion in the temperature dimension".

Another way is to first run a CHT-Simulation, pick the temperature at 3 remote points which don't lie on one line and fix them manually to the CHT-values.

If you find any workaround to this problem, or if the problem never arised in the first place, please let me know!

And, of course, if you got further questions, i am happy to share my misery :D

Cheers
Daniel

stumpy May 5, 2010 11:13

The easier way to do this is to insert command snippets in Workbench. Set it up as a structural analysis, then apply your thermal boundary conditions using a command snippet inserted into the Static/Transient Structural item in the tree, e.g:

toffs,273.15
ic,all,temp,25
sf,named_selection_name,conv,2000,25
d,another_named_selection_name,temp,100

To switch the element type, insert another command snippet into Geometry > Solid Body:

et,matid,226,11
KEYOPT,matid,2,0


All times are GMT -4. The time now is 13:09.