Modal analysis of a submerged structure

[Anonymous]

Hi,

I need to conduct a modal analysis for a submerged (seawater) structure (aluminium bronze propeller) - I have come across the MFLUID command in my search, but can't find any worked examples. Is this type of analysis possible in Nastran and if so, does anyone have a worked example I can study?

Thank you

[John_Holtz]

Hi @Anonymous 

You can include the water effects by editing the Nastran file manually. See How to include fluid in a modal analysis in Nastran.

Sorry, but I do not have any examples that show anything helpful in this regards. Perhaps another reader has done it in real life and provide some feedback.

[Anonymous]

Thanks for the link @John_Holtz - I'll give that a try.

[Anonymous]

Hi @John_Holtz,

Please let me know if I should post this on a new thread,... I am getting the following errors when I try to run my underwater modal analysis study:

FATAL ERROR T2279: VIRTUAL FLUID MASS SURFACE ELEMENT LIST 12 DOES NOT EXIST

WARNING T2282: VIRTUAL FLUID MASS WET SURFACE ELEMENT LIST IS NULL

TOTAL WARNINGS = 1
TOTAL FATAL ERRORS = 1

I have followed the instruction I can find and have searched the web, but can't find a solution. I have attached a screenshot of my Nastran script before it goes into the list of grid points and elements.

Are you able to advise on what I am doing wrong with my code?

Thank you!

[John_Holtz]

Hi @Anonymous 

The message implies that there is no ELIST command. The ELIST command gives a list of elements that are wetted by the fluid. The ID of the ELIST command (in the second column) must correspond to the ID given on the MFLUID command (column 6).

What we need to see are these 3 blocks of lines (although you may have more than 1 line in some of the blocks):

1. The SUBCASE commands from the top of the file.
2. The MFLUID command added to the bulk data section (normally added at the end of the file for convenience).
3. The ELIST command.

You can copy and paste those lines of text instead of attaching images.

[Anonymous]

Hi @John_Holtz,

Sorry, realise now that my screen shot was a useless view anyway. Understood re the 3 blocks - I have included these but am clearly making a mistake somewhere. If you're able to advise, that would be much appreciated.

The model is a single, homogeneous item (nickel aluminium bronze) with no internal voids. The item is submerged by ~1.5m in seawater.

Here is first part of the code (also attached as a screenshot as the spaces between columns seem to disappear with the cut and paste) -let me know if it would be useful to have all the grid and element data too:

NASTRAN EXTRACTMETHOD=LANCZOS
ID 47697BE9-C2B0-4204-ADDC-778910822170
$
$ NORMAL MODES SOLUTION
$
SOL MODAL
CEND
ECHO = NONE
DISPLACEMENT(PLOT) = ALL
SPCFORCES(PLOT) = ALL
STRESS(PLOT,CORNER) = ALL
METHOD = 1
SUBCASE 1
LABEL = SUBCASE 1
SPC = 1
MFLUID = 7
BEGIN BULK
$
$ ******************************************************************************************
$ Written by : Autodesk Inventor Nastran
$ Version : 2020-SP0 -- Database V10.2
$ Translator : Autodesk Nastran
$ From Model : G:\Engineering\Department\R&D\02 Consultancy (C)\C001 Haida\PP18009 Section 2020-02-11 IG.ipt
$ Date : Wednesday, Wed Feb 12 08:13:52 2020
$ ******************************************************************************************
$
PARAM,UNITS,MM
PARAM,COUPMASS, OFF
EIGRL 1 10 MASS
$------1-------2-------3-------4-------5-------6-------7-------8-------9-------0
CORD2R* 1 0 0.0-2.4401199999-12*
* -4.xxx-xxxxxxxx+2 0.01.xxx-xxxxxxxx-122.761899999999+2*
* 0.0 0.0 0.0
MAT1* 11.160000000000+5 3.300000000000-1*
* 7.600000000000-91.599999999999-5 0.0*
* 5.900000000000+2 1
$ Physical Property
$------1-------2-------3-------4-------5-------6-------7-------8-------9-------0
PSOLID* 1 1 0

$ Fluid
$------1-------2-------3-------4-------5-------6-------7-------8-------9-------0
MFLUID 7 1500.0 1025.0 12
ELIST 12 1 THRU 100

$ Grid points
$------1-------2-------3-------4-------5-------6-------7-------8-------9-------0
GRID* 1 0-2.xxx-xxxxxxxx+09.886347060437+2

[John_Holtz]

Hi @Anonymous 

Thanks for the new information. I am surprised that the text did not keep the spaces to align the columns, but it did not. Fortunately, you provided an image that shows that you did have everything aligned to the columns, except for the following potential problems:

1. For the MFLUID command, column 3 was left blank. I suggest that you enter a number here. If your model is oriented with the Z axis pointed up, then enter the number 0. (If your model has another orientation, then you need to create a new coordinate system (last branch of the model tree) and enter that number.
2. For the ELIST command, the list of elements should start in column 3. You started the list in column 4. Try it with "1" in column 3, "Thru" in column 4, and "100" in column 5.

Also, column 5 of the MFLUID command is the mass density of the fluid. Since your units of length are mm, I believe the units of mass would be "t" (metric ton?). I think the seawater is not 1025 mton/mm^3! Maybe 1.025E-9 mton/mm^3.

[Anonymous]

Hi @John_Holtz ,

Thanks for the support on this, much appreciated.

I implemented the changes you suggested (including the incorrect density value!) and managed to get the model running once I realised that I had to use shell elements - managed to miss this despite it clearly stating so in the MFLUID instructions.

Unfortunately, the propeller blade I am simulating, whilst significantly thinner than it is wide and long, can't be accurately simulated with a shell element model (due to blade root thickness), so for the time being I will look for a different solution and keep the MFLUID option in my back pocket for future relevant problems.

Thanks again for your assistance,

Ian

[John_Holtz]

Interesting. I had forgotten that the MFLUID command only worked when "contacting" shell elements.

This may not be the best work around, but I wonder if you can do this:

• Add an idealization to the analysis and define the new idealization to be shell.
• Select the outside of the blades to be the geometry for triangular shells.
• Mesh the model using linear elements. Since the shell elements and face of the blades are using the same faces, the mesh will match.
• Make the shells thin (so that the stiffness is not affected) and massless.
• Define the MFLUID command using the shells. The shells are coincident with the solids, so essentially the MFLUID is "contacting" the solid.

[Anonymous]

Hi @John_Holtz , sorry for the very slow reply. I had a similar thought re a non-structural skin and have been trying to make it work (comparison with a validation case). I haven't succeeded yet, but when I do, I'll update this thread.

Thanks again for your help,

Ian