Implement a wire in a 3D Geometry and adding a constant temperature to it.

[m0lind04]

Hello everyone,

I am looking for a solution to install a wire in a 3D Geometry and adding Heat Transfer BC conditions to it later on. My problem so far is that I install the wire, I add a section, even put a BC on it, but it does not connect to the rest of the three dimensional mesh. It only connects in beginning and end points, and according to this also only applies the BC at those connected points to the rest of the geometry. - But i Would like to connect the wire BC to the mesh density of the bigger geometry. I am working in CAE.

It would be really helpful if someone has an idea how to solve this problem. Have great day!

 

[FEA way]

What kind of analysis do you want to perform (uncoupled heat transfer, coupled thermal stress or stress-displacement) ? Abaqus offers 1D link elements for heat transfer procedure (DC1D2 and DC1D3). There are also special truss elements for thermal stress analyses (T3D2T and T3D3T). These elements support thermal boundary conditions and loads. Apart from that you can prescribe temperature directly to elements without thermal degrees of freedom. This includes beams as well.

 

[m0lind04]

Hello, Thanks for the response.

I want to perform an uncoupled heat transfer analysis. I want to simulate the freezing of soil that surrounds one or multiple pipes. one solution in small geometries is to create an actual opening in the soil and apply a film surface coefficient. BUT now i am working on far bigger models, where I want to estimate the freezing around the pipe with the pipe simply being a BC to keep the total amount of elements fewer.

 

[m0lind04]

Hello,

I am using the suggested Elements but I still get the result, that the BC is only applied on the end nodes of the wire. Can anyone help?

 

[FEA way]

How is this 1D element connected with 3D mesh ? Did you use embedded region for that ? And what are the BCs applied to this wire ?

 

[m0lind04]

BC = konstant temperature of -30 celcius.

Thats the warning i am getting using embedded region constraint:
10 embedded elements have temperature, electrical potential or pore pressure degrees of freedom. They are not constrained to the host elements. The elements have been identified in element set WarnElemEmbeddedTempDof.

I have also tried a tie constraint, but then the results appear to be very inaccurate bc a lot of nodes are not connected.

I actually got closest when merging the two instances in the assemby mode. But The problem still exists that the wire elements do not connect to the mesh of the 3d geometry. ...

 

[FEA way]

Unfortunately embedded elements do not support temperature degrees of freedom. Try partitioning the solid model in such way that an edge will be created in a location where 1D element is placed. This will force Abaqus to place nodes on this edge. Then align the wire with this edge and use tie constraint between the wire and the edge. With proper adjustment tolerance it should connect the nodes and allow for heat transfer between the wire and solid elements (along the whole wire, not only at its ends).