The problem definition is insufficient to give solution. It seems you are interested in finding the natural frequency of the free span of pipe with its contents and hydrodynamic mass of sea water acting above it. Try changing the density of pipe so that total mass of the pipe will be pipe own mass+ content mass + sea water mass acting on it.

Thank you Nikhil! That worked perfectly! I have another question as well. How can I implement the deformed shaped on the free span (from the static analysis) into the dynamic eigen value analysis? 

According to DNV-RP-F05 the pipe-soil interaction should be represeted by springs with vertical STATIC spring stiffness for the static analysis and vertical and lateral DYNAMIC spring stiffness in the dynamic eigen value analysis. 

How can I implement the deformed shape from the static analysis into the dynamic eigen value analysis?

The static vertical spring stiffness is lower than the dynamic vertical spring stiffness, hence the static deflection is larger. 

You are welcome, Andres. Now after doing the static analysis you want to use the same deformed model for the modal analysis, right? Then follow the steps given in the link as below. 

https://caeai.com/resources/generating-geometry-deformed-shape-using-ansys-workbench-v12

Thank you Nikhil. It seems to me that you are experienced within FE-modeling. Can I ask you an additional question? Do you know if the attached image shows a sufficient method to approximate pipe-soil interaction? Linear-elastic springs in vertical and lateral direction. I have made faces in a grid-like pattern on an Autodesk Inventor model, which is imported into ANSYS Workbench. The springs are body-ground springs connected to the edges and intersections between faces on the model.

Thanks for your appreciation. I don't have extensive experience of PSI problems. But from my gathered knowledge about PSI, I can say that soil behaviour is highly nonlinear and one should be cautious to include the correct soil behaviour in their FEA model to get desired results. In that context please check the correctness of your model and validate your model with some published/reference/textbook work or with analytical formulae if available. Otherwise one thing you can do is prepare a small scale actual 2D/3D model in which soil as plane area/solid with non linear material properties of soil and pipe as beam/solid and then you can compare the results of your pipe-soil as linear elastic spring model with pipe-soil actual model. You will get the idea of approximations of your model with simple static analysis deflections of pipe. I would recommend to get experts view because of the nonlinear soil behaviour.

Reduce the problem size and solver time by setting different element size such that interested areas get finer mesh.

Hope this helps.

Thank you very much!

 You may also take a look at a conference paper i wrote, with more detailed descriptions for pipe soil interactions: https://www.researchgate.net/publication/273130288_Flexible_Pipe_On-Seabed_Stability_Upheaval_Buckling_and_Hub_Protection_Methods  

Conference Paper Flexible Pipe On-Seabed Stability, Upheaval Buckling and Hub...

Hi Anders, referring to your post 

"I have made faces in a grid-like pattern on an Autodesk Inventor model, which is imported into ANSYS Workbench. The springs are body-ground springs connected to the edges and intersections between faces on the model."

I am currently doing a study on interacting pipeline free span as well and I have been trying to model my pipeline in ANSYS workbench for modal analysis.  May I know what you did on your model in order to have the spring attached to the model? Did you generate manually or automatically by ANSYS?  Your reply will be much appreciated.

It is usually convenient to have springs evenly separated by 1.0m since you then can make a script to assign the same spring property to all springs that have the same support conditions (on seabed/ trenched/ rock dumped/ free spanning), however different springs in direction x/y/z. But note that the non-linear springs themselves should not be just 1.0m since lateral/vertical springs then may influence longitudinal expansion/ retraction motion. Springs lengths of 100m will work ok, with a pin-type attachment to a pipe node and clamped at the far end (avoid singularity).

Results for a model of a free-spanning pipe down from a Template to the seabed with an upheaval buckle, into a rock dump with a lateral buckle and then into a trench transition with a new upheaval buckle, continuing down into soft mud in a trench that allow small lateral buckles will look like this: (springs hidden in plot)

Thank you for the answer Sir Rolf-Hugo Kirkvik,

As I am new to ANSYS workbench, there are several more questions I would like to ask you regarding creating springs in ANSYS workbench if you don't mind.  Referring to the image I have attached, I wish to create spring elements on each and every mesh node.  In this case my element size are 0.08415m and therefore I wish to create every single individual spring along 16.83m pipe length with the distance between springs of 0.08415m.  The figure I attached are springs I created by manually input each location of every single spring.  I wonder what are the faster way to create the spring automatically along the 16.83m without having to do it manually?  I wish to have it done automatically as I will be reusing the model with different pipe diameter and pipe length and having to remodel every single spring is going kill off a lot of time.  I have tried object generator but failed to generate those springs.  I apologize for my inexperienced questions and greatly appreciate your help.