2D Axisymmertic vs 3D Brick Rotational Stress

[cody.macneil]

Hello,

This is kind of a follow up to previous posts I have made regarding meshing issues with large 3D bodies with small stress concentrations. I have decided to try and utilize the 2D Axisymmetric element to determine the stress fields in a rotor since I was having difficulty determining stress concentrations at the trunnions in the 3D models.

The problem I am now having is that the 2D Axisymmetric models are very inaccurate at the centreline of the shaft (y=0). I have attached a picture of the 2D vs 3D model so the differences can be seen. I am getting much higer stress values at the centerline vs the 3D model and the X-X Tensor components do not closely match the closed form stress calculations as the 3D model does.

I am hoping there is some settings or boundary conditions I can apply that will yeild the correct stress fields such that I can add refinement points and study the stress concentrations that form as a result in the abrupt change in diameters.

Important information to note about the model is:

- Top bearing surface is fixed in x,y,z

- Bottom bearing surface is fixed in x,y (allowed to move up and down along the rotational axis)

- 4130 Steel

- Spin Rate 10,000 RPM

Thanks,

Cody

(As a side note - I could not use quadratic bricks in the 3D model since upgrading to the 2013 version. It says it fails to run the analysis and does not give me a specific error)

[PipePakPat]

Access the Element Definition screen for the 2D element part and change the "Compatibility" to "Enforced" and re-run the 2D analysis.

[PipePakPat]

I was not able to replicate your issue working with higher order brick elements using the 2013 software.  I accessed the Element Definition screen and changed the "Midside Nodes" from "Not Included" to "Included".  This action also changes the "Compatibility" to "Enforced" and raises the integration order.

[cody.macneil]

Thanks for the input so far.

I was able to utilize the enforced compatibility function to get something more reasonable but I read on the help file that this may cause inaccuracies due to linear approximations. I did as suggested and made seperate parts - Part 1 being at the centre line and Part 2 the rest of the rotor and am having the same problem as before if I turn off enforcement for Part 2.

Additionally, I don't mind running a much higher resolution mesh to mitigate the stiffness problem but I am having the same issues I mentioned earlier with the program not running. It seems this occurs above a certain mesh density.

I have attached pictures and the datalog to this reply. Any help running a more accurate 2D model would be greatly appreciated.

Thanks,

Cody

[PipePakPat]

Your model is demonstrating a "singularity" where the geometry steps from one diameter to another.  A stress singularity is when the stress continue to climb as the mesh size is reduced.  Typically, stresses would converge on a single value as the mesh size reduces.  In your case, your model as right-angles defined at geometry transitions which acts as a stress riser.  No matter how this part is machined or manufactured, there will be a small radius at this transition of geometry.  If you include this radius in your model and re-mesh the model, then you will find that the stresses will converge and will occur in the center of the radius.  There are many places in the geometry where these fine geometric details can be ignored, since they are not locations of significant stress in the model.  Please let me know if you have further questions.

[cody.macneil]

Thank You,

Your advice has helped my quite a bit on reaching some level of convergence. However I am still having the issue of the program not running once I exceed a certain number of elements in my model. Any idea what could cause that?

Thanks,

Cody

[PipePakPat]

It is odd that your 2D analysis would contain too many elements to solve?  Perhaps you could upload an archive of your model (without results) and provide the exact wording of any warning or error messages that appear on your computer?