## General Mechanical

#### Pipe Spanning

• AOSY
Subscriber

Hello, I'm new to ANSYS and I hope someone can provide me some guidance on the issues I'm facing.

I am working on building a pipe under spanning condition using ANSYS Static Structure. The work that I'm able to come up with so far is the model of the pipe as shown in the picture below.

But I have no idea what are the correct procedures to model the soil at both ends of the pipe to create the spanning condition. I hope someone can guide me on this matter.

Thank you.

• SaiD
Ansys Employee

Hi,

Could you explain what is "spanning condition"?

If the two ends of the pipe are just buried in soil, then you need to determine how much freedom do those two ends have to move around. If they are fixed completely such that they cannot move at all, then a Fixed Support boundary condition may be appropriate. But if they may have some relative motion, then using Displacement boundary condition to restrict movement in certain directions, while leaving other degrees of freedom unrestricted may be more appropriate.

Sai

• AOSY
Subscriber

Hi Sai,

Thanks for helping with my question. In my case, spanning condition is the location where a pipe loses contact with the seabed. Figures below show what I managed to come out with so far, before and after simulation.

I have added two squares at each side of the pipe as the seabed to create the spanning condition. However, I'm now facing new doubts.

1. How do I make sure that the 2 squares are a flat non-deformable are like what I want it to be? And is my pipe a rigid structure?

2. I'm not sure why after simulation, my pipe seems like it has expanded and is slightly deviated from its original position, which is at the middle of seabed. Besides, before simulation, the pipe was laying on top of the seabed, but after simulation, half of it seems like it has sunk into the seabed.

3. I have assign a thickness of 100mm under the geometry of the seabed as shown in the Figure below, i'm not sure is it okay to assign it this way and what does the thickness actually means here compared to the one we create in spaceclaim.

Thank you.

Amanda

• SaiD
Ansys Employee

Hi,

1. If you are not concerned about the deformation of the two blocks on the end and their deformation is not important in the analysis, then you may select those bodies --> Details-->definition-->Stiffness Behavior-->Rigid. If you define the pipe as a rigid body too, it will not deform in any way when loads are applied (and stresses on it will also be zero). If all the bodies in a Static Structural analysis are rigid, it does not make sense to do a Static Structural analysis (because no body will deform). What is the objective of this analysis? You mentioned you need to find the location where the pipe loses contact with seabed, but I am not sure why applying an internal pressure to the pipe would make it lose contact with the seabed. Is there something that I am missing?

2. The pipe likely expands because you are applying an internal pressure of 5 MPa. The sinking of the pipe in the seabed might be occurring because contact between the pipe and the two blocks might not be defined/detected properly in the simulation. If you go to Connections --> Contact, what type of contact is defined between the pipe and the two blocks? Is the geometry of the pipe defined to be a shell (which I suspect because of your next question)? If it is a shell, it's pinball radius might be small, causing the issues in contact detection.

3. If the Thickness Mode is Manual then whatever value you input in Ansys Mechanical is used. If it is Auto, then the thickness is based on what you defined in SpaceClaim. Go through the following section in Ansys Help:

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/wb_sim/ds_Thickness_Mode.html

Since 100 mm doesn't seem to be too small as compared to the length of the pipe, I would suggest defining the pipe as a solid body and meshing it with solid elements.

Hope this helps,

Sai

• AOSY
Subscriber

Hi Sai,

1. After listening to your suggestion, I have defined the stiffness behaviour of the two blocks as rigid, whereas the pipe's stiffness behaviour was remained as flexible. The objective of my project is to identify the total equivalent von mises stress acting on the pipe under the effect of internal pressure and also spanning condition. The spanning condition was created and it was represented by the space between the two blocks.

2. For the contact between the pipe and the seabed (the 2 blocks), I've tried both frictional as well as no separation. I would like to hear your advice on this matter. How do I check if the geometry of my pipe is defined as a shell? I actually wanted to model something similar to the picture shown below where the pipe will not sink into the seabed and the seabed is represented by an area and not solid blocks. Can you guide me in solving the pipe sinking problem?

When I model the seabed as area instead of blocks  by not assigning any value to the thickness, it will require me to input a value. Why is that so?

3. How do I define the pipe as a solid body and meshing it with solid elements, with reference to your earlier suggestion?

4. Figure below shows the latest progress on my model, hope you can advise me on anything that I can improve on.

This time, I have put the thickness of the seabed as 10mm and the seabed is defined as rigid structure. As shown in the picture, the sinking of the pipe into seabed still occur.

Thank you.

Sincerely,

Amanda

• SaiD
Ansys Employee

Hi,

Here are the possible solutions to your questions:

2. In the image you have attached it says Details of "SYS-44/Surface". The fact that it says "Surface" means that you have created a 2D body instead of 3D body. So Mechanical asks for some thickness since this is a 3D analyis. You can check if the pipe is modeled as a shell in a similar manner (select it and look at the Details; if it says surface, it's probably a 2D surface without a thickness).

3. To change the pipe to a solid body, you will have to edit the CAD geometry (In SpaceClaim or a similar software that was used to create the geometry).

4. If your parts are indeed shells, then defining contact between them might be a bit tricky. Since the seabed is Rigid, it will be defined as the Target side and the pipe outer surface will be the Contact side. Go to Details-->Definition-->Behavior--> Asymmetric. If the bodies are shells, their Pinball radius may be very small which may lead to contact not being detected properly. If there are too few substeps defined, contact detection may fail again.

You can click on the Contact pair --> Details-->Advanced-->Pinball Region-->Radius and define a slightly larger pinball radius. Also try going to Analysis Settings -->Auto Time Stepping --> On, then define either by substeps or time. (E.g. you can choose Substeps and increase the number of minimum, initial and maximum substeps).

Sai

• SaiD
Ansys Employee

I was unable to insert an image in the post, but to understand why you need to increase the number of substeps, go through this similar thread and have a look at the image about contact detection:

https://forum.ansys.com/forums/topic/structure-penetration/

Sai

• AOSY
Subscriber

Hi Sai,

1. From the picture shown below, is it correct to say that the pipe is a solid whereas the seabed is a surface? And does solid mean it is a shell? Can you explain more about what shell is?

2. Can I know why does changing the behavior to Asymmetric helps to solve the contact issue?

3. Is the problem of pipe sinking into the seabed mainly because of the contact issue or does the material properties of seabed affects as well? Does by assigning seabed as rigid should have prevented the sinking if the contact between pipe and seabed is properly defined?

Thank you.

Sincerely,

Amanda

• AOSY
Subscriber

Hi Sai,

I have few more questions.

4. What is the suggested pinball radius that I should assign?

5. As shown in the picture below, what does target shell face means? What should I select for the target shell face in my case?

Thank you.

Amanda

• AOSY
Subscriber

Dear Sai,

This is the latest simulation result that I got after assigning Asymmetry, increase the pinball region radius to 10mm and also increase the substeps with minimum and initial substeps to 2 and maximum substeps to 20. However, the result is the same as previous one.

Is there anything else that I might overlook?

Thank you.

Sincerely,

Amanda

• SaiD
Ansys Employee

Hi Amanda,

1. Yes, it looks like the pipe is a solid while the seabed is a surface. Solid bodies are meshed using solid elements (like tetrahedron, hexahedrons etc.), while surface bodies are meshed using shell elements. So in this case, the pipe is NOT meshed using shell elements because it is a solid. Shell elements are used when modeling structures which have a very small thickness as compared to the other 2 dimensions (like a shell). Solid elements only have displacements as their degrees of freedom (dof). Shell elements have displacements and rotations as their dof. An analogy I can think of is if you are familiar with beam elements: If you have a long bar which undergoes bending, and you mesh it with solid elements, you would need 4-5 solid elements along the thickness to capture the linear variation in stress across the cross-section. So to increase efficiency we use beam elements. Similarly, if you have a very thin, almost 2D solid, it's more efficient to use shell elements.

2. Auto-Asymmetric means that the Solver can switch the Contact and Target sides during the course of the simulation if it deems that necessary. But in our case we have a rigid body coming in contact with a flexible body. In  such cases, the Rigid body is ALWAYS the Target side and we son't want the Solver to switch this selection ever. So whenever we have a Rigid body coming in contact with a Flexible body, we need to define the Behavior to be Asymmetric.

3. The sinking occurs due to Contact not being detected properly. But the material properties of the two bodies in contact affect the contact stiffness, and hence they indirectly affect whether contact is detected properly or not.

4. There is no fixed value for Pinball radius. You may increase it if contact is not being detected properly. But if the Pinball radius is too large, contact would be detected in cases where physically there is no contact e.g. if your pipe and seabed are very far away i.e. there no contact in real life, but if you increase the pinball radius a lot, contact would be established between them in the simulation. So this would lead to inaccurate results.

5.  Surface bodies have a normal direction associated with them, which indicates the top and bottom surfaces. Imagine you have a thing membrane in real-life, that membrane has a top surface and a bottom surface irrespective of how thin it is. So based on which side (top or bottom) of the seabed, the pipe is at, that side should be the Target Shell Face.

Sai

• AOSY
Subscriber

Dear Sai,

I have few doubts.

1. Where can I check about contact stiffness? Is there any range for the value of contact stiffness that you can suggested in my case to allow proper contact being detected between pipe and seabed?

2. I have obtained the properties of soil from Ansys Engineering Data as shown in the figure below. I am not sure what type of soil it is and I like to know if Ansys provide any guideline for defining material properties for sand at seabed?

3. By looking at the properties of soil, is it the reason why it is hard for me to get proper contact between the pipe and the seabed? Which properties should I change to allow better contact detection?

Thank you.

Sincerely,

Amanda

• AOSY
Subscriber

Dear Sai,

How are you?

I've tried to model the seabed as a solid element and the pictures below showed my latest attempt. I'm not sure why after simulation, one of the seabed changes orientation as shown in the picture. Can you please explain what might go wrong?

Thank you.

Regards,

Amanda

• SaiD
Ansys Employee

Hi,

1. To get the Contact Stiffness, you would need to solve the simulation. Then go to Solution-->right-click on Solution Information-->Insert-->Contact. In the Details-->Type--> Min (or Max) Normal Stiffness. Choose the appropriate contact pair for Contact Region. Then right-click on the variable you just created and choose Evaluate All Contact Trackers. You should get a plot showing how the Normal Stiffness varies over time. Based on the values you get, you can try to manually increase the value of Contact Stiffness. To change the Contact Stiffness, go back to the Contact pair definition-->Details-->Advanced-->Normal Stiffness Value --> Absolute Value --> Enter a value higher that the contact values you got in the plot. This might help in reducing the penetration.

2. and 3. If you have defined the seabed to be Rigid, then it does not require any material definition.

About your latest posts: it looks like the seabeds weren't constrained properly. One of them probably underwent rigid body rotation. How are you applying the boundary conditions?

If any of these answers solve your issue, please mark that answer as "Is Solution" so that others running into similar issues can find the fix easily.

Sai