FEA- how to add fixed constraints on a floating hollow ball?

[WAYNE_HOUWD]

Hi,

Now I am running out of ideas on FEA of a hollow metal ball.

The case is-

1. hollow steel metal ball OD 200mm, ID 190mm

2. Outside surrounding uniform pressure 10 MPa.

3. The ball is floating in a kind of liquid, so the gravity is neglected.

How to run FEA on this ball? My confuse is how to add fixed constraints.

Best Regards,

Wayne

[blair]

You should try and figure how deep the ball will float in the fluid first and then create a split-face at that depth. I might try a simple constraint on the split-face portion (in reality you should probably create a number of split-face rings with different pressures to simulate Hydrostatic Loading). Apply your load to the upper portion.

[JDMather]

This is a bit of a fudge.

Use caution fo whatever it is worth.  (could be very wrong)

...and I didn't bother to split the faces to try to more accurately represent hydrostatic pressure - I use the uniform pressure you specified.

You didn't specifiy the material properties.

[WAYNE_HOUWD]

Hi Professor JD,

Thanks for your reply on this FEA.

Actually, I have made it as simple as a metal ball when putting the question here. This question came from a cute submarine shell design. I read the science news from internet and then I asked myself how to check the whole shell strength? It may be not as regular as a ball, but an irregular shell, something like not symmetrical. That means the neutral plane is not easy to work out. In that case, we have to solve the shell strength as whole without any slice or split.

So the question back to the original, can we do some analysis on the whole shell without partial slice out?

Bow to all the replies,

Wayne

[JDMather]

I don't think I would bother with something like this in Inventor.

Autodesk Simulation Multiphysics or some other analysis software.

[henderh]

Hi Wayne,

 It may be possible to get what you're after with AIP by employing the inertial relief method via motion loads workflow of Dynamic Simulation in conjunction with Stress Analysis:

Prepare the model for simulation:

 1)  Create a new assembly that will be a 'wrapper' assembly

 2)  Create or add a "dummy part" (it is placed as grounded)

 3)  Place the model to be analyzed in the wrapper assembly (fully unconstrained)

Do the motion loads workflow:

 4)  In Dynamic Simulation, create a spatial joint between the dummy part and model to be analyzed  (you can do this easily using 'Convert Constraints' command after turning off 'Automatically Conver Constraints to Standard Joints in the DS Settings dialog)

 5)  Run the simulation (nothing will appear to happen, this is okay)

 6)  Export to FEA the mobile body (chose an arbitrary load bearing face)

 7)   In the Output Grapher, choose an arbitrary time step such as 0.00

 😎  Enter the Stress Analysis environment and create a new Motion Loads Analysis in the Simulation Properties

 9)  Add the appropriate pressures

 10)  Solve

Notice we didn't add any constraints in SA and we don't witness any rigid body movement or soft springs message (image attached).  You can further validate the results by probing the cylindrical portion and see that the hoop (circumferential) stress is twice the longitudinal (axial) stress as it should be with this shape of pressure vessel.

  It may be possible to neglect the effect of an increasing hydrostatic pressure load with depth if the model is very 'short' or at a very deep depth where the hydrostaic pressure % change can be negelected with respect to the model's height. The approximation may yield better results if using the "average pressure" that is acting at the area centroid of the projected side-profile.

Hope this helps!

Best regards, -Hugh

[Edit: fixed typo]

[WAYNE_HOUWD]

Hi Hugh,

Thanks for providing a wonderful solution with "dummy part" to anchor the marine. It really works very well.

Best Regards,

Wayne

[henderh]

Excellent!   We appreciate the follow-up Wayne.

[killinformula]

I just wanted to say how brilliant this solution is!  I deal with designing valves for engines that are not hard mounted to the engine and are basically like the "floating ball", and this solution is what we have been searching for to see the resultant stresses from the pressure inside the valve.  Thank you very much!

[vulic]

Dear @henderh

Can you you upload this assembly so I can see how it is done. I have stumbled up on the same problem and it will help me a lot??

[JDMather]

@vulic 

Can you Attach your assembly here?