I am new to FEMAP, NX Nastran, and mid-surface FEA.
I have a closed bin with multiple compartments containing small solids (~5mm in diameter). I would like to see how the bin will perform if it is pressurized.
I created a mid-surface model of 1/2 the bin, restrained the bin mounts, applied a pressure load to internal surfaces that are exposed to a pressure differential, and applied a non-structural mass region to represent the mass of the solids.
I am doing a linear static analysis as a place to start and to get a rough idea if this existing bin will work under pressure.
When I run the analysis, I am getting a very large displacement on the end-walls of the tank (30.89 inches)...which is obviously wrong.
I am not sure what I am doing wrong. Did I improperly setup the symmetry constraint, or the mass region? Or am I misinterpretting the results?
I can post the .modfem file if that would help, but it is a very large file (850 MB).
Any suggestions on how to improve my results would be very much appreciated.
I don't have seen any stress results, I suppose that also these values are enormous, you can check all the values you have used and its units. Then try to run the analysis without the non-structural mass and then compare the results. A few time ago I have done a similar analysis and I forgot to use the proper consistent dimension factor for the non- structural mass.
You can also run the analysis without the non structural mass and convert pressure in an hydrostatic pressure taking into account the weight of the material inside the tank. You will get the same results!
A few suggestions for checking:
to check plate thicknesses, use thickness/cross section display
Just to clarify a few other possible issues, your nonstructural mass input only modifies your mass matrix, and therefore, unless you have used body load to apply gravity accelerations, it has no impact on your deflections.
If you are applying a gravity body load, and want to easily make runs with and without the nonstructural mass regions, in the model info tree, you can use RMB on the mass region and enable/disable a region and run your analysis both ways.
Also, note that pressure loads applied to thin flat plates can have unexpected large displacements in a linear analysis because the only load path for the pressure load is bending and transverse shear. In reality, membrane action can greatly reduce the deflection, but you must perform nonlinear/large displacement solution to account for this behavior.
I appreciate you looking at this. I checked all of the units, and I was consistent in using pounds and inches throughout. I did find an error in how I set the symmetry constraint while reviewing the model, and I turned off mass region just to have one fewer thing to debug. Unfortunetely I am still getting very large displacements.
Post your model and I'll try to see...
I am not familiar with custumary units...
This is my result of an head 3000 mm OD 5 mm thickness 3000 mm inside maior radius and 50 mm minus radius loaded by an internal pressure of 5 barg. The maximum displacement is only 17.37 mm! (don't consider the high stresses...)
I think your constraints are corrected but the loads have no consistent units...
Thanks for the reply. I really had a hard time bringing the geometry into FEMAP for this bin (it has some weird shapes in it, but that is a different story), so I figured out how to check thinknesses pretty early. I checked again, and they seem ok. The only thing I am not sure of is that the automatic midplane function missed assigning a few surfaces with thicknesses, so I assigned them using the PLATE element. Is this likely to cause a problem?
Thanks for the advice on the gravity, I was doing an unsucessful search through help yesterday trying to answer the question, "which way is gravity pointing in this model", and decided to put that part of the model aside for now.
Yesterday I also created a few very simple bin models (cylindrical, one fixed face) of similar thicknesses, diameters and lengths just to see what the results should roughly look like. I again noticed pretty large displacements, and knew that there must be something else going on. Your explanation on non-linear large displacement probably explains this.
What would I need to setup to perform a non-linear large displacement analysis? Would I need to define more advanced material settings? Do I need to make the pressure vary with time? Which solver would I use?
Thanks very much for your help!
For the gravity edit "Body Loads" then activate the flag "Translational Accel/Gravity...) and put your gravity acceleration value in the proper direction. I have done a better look at your model and pressure load and if I have understand correctly you put 15 psi on a almost flat head. In this case the displacement may be correct in a linear solution, but this type of tank cannot withstand such a big pressure.
Before trying to post a large model, I would suggest deleting all the results, and doing a File/Rebuild then save the modfem. Then zip the modfem before trying to post.
Another option that sometimes is more compact, is to write a Femap neutral, and then zip that file, it may be smaller. The final and most compact option is to compress the .dat file and provide just the Nastran deck. You won't be providing the geometry, but that is not likely a problem anyway.
Adding the plate element properties for the ones missing from the midplane tool should be fine.
To run a large displacement nonlinear solution does not require any change to your materials, they would still be linear. The only nonlinear effect will be large displacement, the stiffness will get updated using the deformed geometry, that is what captures the membrane effect I was referring to.
There is an example problem for large displacement of a cantilever beam in the Femap examples under the Help Menu.
Sorry for the long delay since my last posting, I have been spending a lot of time updating my FEA model and trying to validate the FEA.
I ran the non-linear large displacement analysis as per the suggestions here, as well as updating the model to take into account plastic deformation of the material, and the results looked believable. To confirm, I ran a hydrostatic test on one of my bins.
Where the FEA predicted that the tank would fail in some locations (with stress 2x to 3x the max 80 ksi UTS of the material), the bin did not rupture during the hydrotest.
The bin did see some very large plastic deformations (twisting, buckling, and warping) at the locations the FEA said the high stress are, but it did not rupture.
Is there a way to predict with a FEA model at what internal pressure and where the bin would rupture?