FEA of bolted connection on a check valve

[alok]

I have a check valve with flanged connection at the top (attached). The flanges (4.6" and 2.75" thk) are bolted together and have RTJ between them. Because of the RTJ, the flanges do not have any surface contact between them. I am trying to do the FEA to analyze the maximum stress at the bolt locations, but not sure of what type of contact to use between the flanges.

Any help would be appreciated!

Thanks!

Alok

[S.LI]

I guess the simple way is to simulate RTJ as new parts in brick element or 3D-Gasket element.

The connection between RTJ and flange could be either just banded, or surface-surface contact. 

[John_Holtz]

Alok,

I agree with S.Li, but what he did not mention is that 3D gasket elements are only in the nonlinear analysis (which is more complex than a linear analysis). Based on the geometry of the seal, I think the gasket element will not work so well. So, I think you need to model the seal.

But first, you should indicate what type of analysis you are doing: linear or nonlinear? If nonlinear, what material model are you using for the seal? What material properties do you have for the seal? These answers will dictate what you can and cannot do in each analysis type.

I just thought of another way to do the simulation. Do the analysis in two design scenarios. One design scenario for the top half of the valve, and another for the bottom half of the valve. Then, apply a force to simulate the bolt preload. You can either model half of the seal for each analysis and apply a symmetry boundary condition to the seal, or use some type of spring to simulate the seal.

Be sure to take advantage of symmetry if there is any (half symmetry, quarter symmetry, and so on).

[alok]

Hi John and Li,

Thanks for your responses.

I am doing exactly what John has mentioned. I have separated the top and the bottom half and planning to run the simulations separately. I am doing the linear static stress analysis. The whole point of doing this FEA analysis is that our customers want this valve to be in accordance with ASME Section VIII Div. 1. But after running the section VIII calculations the bolting on the bottom half is failing. So I need to check if the current bolting passes the FEA.

As I am currently working on the bottom half, I will go through the materials only for that part. The top flange (4.6" thk) is 17-4 SS with condition 1150. The bottom flange (2.75" thk), which is welded to the valve body is A216 WCB. The bolting is A93B7m and the ring gasket is soft iron.

[alok]

I got everything set-up. But when I run the analysis, I get the warning.. "*** Warning *** Distorted pyramid found, 1 have been split to tets".. and "Model may not be tied down enough, check the DOF".. The first warning is probably due to some meshing issues which I believe will not make any difference in the results. For the second warning, I have my assembly cut in half along the XZ plane. So I have specified the Y symmetry along that plane. But I don't understand what to specify along the X and Z axis.

[S.LI]

Not very sure your modeling. A screenshot is helpful.

My guess is:

1.) if you don't have explicit loads applied on X and Z, it might mean displacements in these two direction are not the that important in your model.

2.)apply X and Z constraints on at least two non collinear points, which should be as far away as possible from the sensitive regions (joints, bolts)

[John_Holtz]

You may also find it helpful to review the page in the documentation "Help > Autodesk Simulation > Setting Up and Performing the Analysis > Set Up Analyses Part 3 > Perform Analyses - Run Simulation > Perform Linear Analyses > Perform Analyses with Gap Elements".

When performing a static analysis, it is important that the model is statically stable in all 6 directions (3 translations, 3 rotations). Many people do not think about what stability the contact elements provide to their models, or in this case, do not provide to their model.