Equation Constraint - Thick Walled Pipe 3

[connor1406]

Hi everyone,

I am quite new to Abaqus and FEM software in general. I am trying to model a thick walled pipe (closed) in Abaqus. The way I have been doing this is extruding a solid pipe section and constrain one end (BC) in the axial direction only (to allow for radial and hoop expansion). I have then applied a uniform internal pressure to the pipe and the associated axial pressure (calculated for a closed thick walled pipe).

The problem with the model is the way the pipe is deforming, it does not seem to make physical sense. I am expecting radial and hoop deformation to be uniform. I am unsure why this isnt working, could someone please outline how to fix this problem so i can have a well behaving closed thick walled pipe? (I am currently trying equation constraints)

Thank you! Please ask any questions and I will respond asap.

 

[StefCon]

Hi,
You could try to make a cylindrical coordinate system (x in the radial direction of the pipe), then use a coupling to couple the end face of your pipe (free in x (radial) direction)). On the coupling's mater node you can apply a BC (DOF 123456). This should allow for radial expansion.

Hope it helps.

Br,

 

[corus]

You need to constrain the other (free) end of the pipe so that it can expand in the axial direction but is restrained rotationally. You do this by using *equation at the free end so that all the nodes are equated to have the same axial displacement as one of those nodes on the free end.

 

[Mustaine3]

If the whole end face is constraint in axial direction, then you only need to add BC on two nodes like shown on the attached image to remove all rigid motions and to allow a free expansion.

 

[connor1406]

Hi All,

Thank you for your suggestions! I managed to get the pipe to behave as expected, this is what I did:

-> Assigned material orientation in the Parts Module to a cylindrical coord system
-> BCs: Constrained one face in the axial direction
-> Loads: Internal Pressure and Axial Pressure (calculated using closed thick walled pipe equations)
-> Constraints: Equation, I created two sets.

​

Set1: On the free face of the pipe I created a set consisting of ONE node in the I.D. of the pipe

​

Set2: On the free face of the pipe I created a set consisting of ALL the nodes , EXCLUDING the node I selected in Set1.

This worked using these sets in the equation constraint and in a cylindrical coord system (that was defined in the Assembly Module).

If this isn't clear and anyone wants me to explain in more detail just ask. Thanks All.