NX Advanced Simulation 3D 1D connection 1

[obe0009]

Hello,

For students I am preparing an exercise for working with different types of elements tetra10, cquad8 and a 1D element.

The exercise is to calculate the results from a solid eg. 200 6 12 (l w h) calculate the displacement with FEM and manually.

2nd is two separate solids each 100m long connected to each other eg. meshmating or glueing calculate results

3rd exercise is create a mid surface plane of the "right" solid. and connect this to the solid with appropriate method eg. meshmating /glue/spider and verify.

I have trouble to connect a bar or a beam element to the 3D element. the element connects but gives a displacement in the order 1E14 when the solid bends.
See attachment.

With an axial load I get a normal result.

Can anyone direct me in the correct way?

Regards,

Olaf

 

[obe0009]

Forgot to select the link button

 

[Tuw]

Hello Olaf,

This is about Degree of Freedom (DOF).

This is because 1D element beam or bar elements has 6 DOFs, except of 1D rod element has 3 DOFs.

3D elements have 3 DOFs only.

When you connect the node of 1D beam element to the node of 3D element, the connection is representing a pin joint, because the rotational DOFs from the 1D element could not be transfer to the 3D elements. Thus information loss.

If you are applying axial load at one end (the other end fixed), the displacement is still normal, because the pin joint is there to secure the position to achieve equilibrium. However, not for bending load (if you are using linear static solution).

A quick fix to this problem, is to apply a spider connection (in NX called 1D-connection), using RBE2 element, node to node type, that linked the 1D node (independent node) to the adjacent surface's nodes of the 3D elements (dependent nodes). This would ensure the moment be transferred/converted into force load at the connected nodes of the 3D elements.

Hope this helps.

Tuw

 

[obe0009]

Hello Tuw,

I thought it had something to do with DOF's
I tried it with point 2 point, no good results.
I have in NX7.5 only source and target, maybe I mixed it up.
After that I tried it with point 2 face
and I got the expected results

See attachment

Regards,

Olaf

 

[Tuw]

I am more like a manual guy, that's why I choose node-to-node most of the time. Anyway, glad you make it.

Tuw

 

[obe0009]

Hello Tuw,

I tried it with node to node but i got not the expected results.
I will try again next week.

Regards,

Olaf

 

[Tuw]

Hello Olaf,

The difference between point-to-face and node-to-node, is the former is geometrical associated, while the latter is non-geometrical associated. Both methods are capable of doing the job, because in the end, it all boils down to an exact/similar input keywords in the input file (.dat).

For the source node, it is usually the 1D element's node, while for the target nodes, it is usually at the 3D elements' nodes. Perhaps while selecting the target, you could set the selection method as "Feature Angle Nodes", which would help to select all the nodes (within the angle tolerance) at that particular element face you click. Please note that if you only selected 1 node as the target, most likely it would not work.

If it still wont work, you can attach your input file (.dat file) here for diagnosis.

Regards,
Tuw

 

[obe0009]

Hello Tuw,

Thanks for your time and expertise.
I did indeed select only one node instead of many nodes on the 3D part.
I was misled by node to node name of the item should be node(s) to node(s)
Results are as expected.

Regards,

Olaf