Shell to solid connections in FEMAP with NX Nastran 1

[Srki1982]

Hi everyone,

I have made a simple model in order to understand how to connect shell elements to solid elements.
Download link: [URL unfurl="true"]http://dl.dropbox.com/u/175649/Test%20of%20Shell%20to%20Solid%20Elements%20Connection.zip[/url]
I have attached the model and wonder if someone can help me out with this problem. My connection between shell and solid right now is glued connection but it is of course wrong. I have learned by checking the NX Nastran manual that attaching a plate or bar element to a solid element is a case of transition between dissimilar
element types. One method of handling this transition is to use RBE3 elements, but how do I do this in my model?

 

[rb1957]

something to remember with solid elements is that their nodes don't have rotational freedoms, which the 2D plate elements have, so you have to give the model a couple to react the moments.

model your 3D edges and your 2D plates so that you've got a reasonably consistent arrangement of nodes. then set up RBE3 elements joining the 3D nodes to the 2D plates.

 

[Srki1982]

Hi, thanx for a prompt response. I am aware of the situation but I dont know how to proceed. The model I have attached is just a section of a much more complex model but my purpose with the section is to learn the exact way to connect shell and solids together. What is the best and easiest way to do it? Can you maybe show me on my model I have attached? Its much to ask but I am really stuck and don't know how to proceed.

 

[rb1957]

i don't know where you want to join ? all i saw was a pipe run with a couple of support clamps.

i don't like opening models ... just attach screen shots.

i'd use RBE3 rigid elements, one independent node on the 2D plate, several dependent nodes on the edges of the 3D elements

 

[Srki1982]

I'd like to join in the exact way you decribe it but I don't know how to do that. I have tried following:

1. New projected surfaces from clamps onto pipe with command Geometry -> Curve from surface -> Project
2. Re-mashed the pipe
3. Instead of glued connection between the pipe and clamps I have now chosen the nodes on the projected surface on pipe to be connected with the nodes from the surface on clamps with command Mesh -> Connect -> Closest link. The connection type is chosen to " Rigid Elements" and the Connection DOF is all chosen.

The analysis can be run without any faults but the result is still bad. If I look at deformed view I can see the pipe rotating and pulling the nodes from solid elements so the shell elements still have rotational freedoms.

Or I can connect the nodes as you said (1 node from shell element and couple of nodes from solid element) but how do I set it correctly, how do I interpolate with RBE3?

 

[Srki1982]

For everyone else having the same problem, do like this (this is applied to the model I've attached):

Project the surface of the solid element to the shell element a remesh. Choose Custom Tools -> Spider Surfaces and choose all surface that you want to connect to the RBE2. Finally, choose Custom Tools -> Element update -> Convert RBE2s to RBE3s.

 

[BlasMolero]

Dear Srki1982,
Here you are a few suggestions:
• GLUE surface-to-surface contact is a correct resource, fast & reliable, an also very accurate, then no need to think in the use of RIGID elements, in this case not need at all. You need to understand concepts like SOURCE & TARGET, I hav revised your model AND THE FOUR CONNECTOR ARE DEFNED WRONG, you need to REVERSE source for target, simply RMB on the connectors and issue command REVERSE. Regarding accuracy, make sure to have similar mesh densities between target & source.
• Said the above, fisrt mesh correctly the PIPE tube using 2-D Shell CQUAD4 elements with quality mapped mesh, you have automatic mesh mixing triangle and quadrilateral mesh, not correct at all, in this simply geometry simply split the tube to have regular regions o mesh with QUAD-only elements.
• You meshed the clamps with tetraedral elements: wrong!, create a midsurface and mesh them with mapped and regular 2-D SHELL CQUAD4 4-node elements as well.

In summary, proceeding as explained above you will see that your model size will be very, very low in number of nodes & elements, but very accurate, allowing you to perform not only linear static analysis but also nonlinear or advanced dynamic analysis, faster & accurately, OK?.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Srki1982]

Dear BlasMolero,

Thank you for the tips, but that doesn't seem to help. The stresses are still the same. Because of that, I've tried the second suggestion you had. I made a new model with additional beams just to have as solid elements. The clamps are now as plate element as the pipe with the same mesh size. Connection between clamps and pipe is glued connection. The curves of the clamps are projected to the surface of the beams and the nodes are set as coincident nodes between these. I still get very high stresses because of the rotation of pipes. Why is that. I have attached the new model at following link:

Link

It's hard to believe that the internal pressure in pipe of just 12 bar may produce/give such high stress at both shell elements and solids. Please, how can I fix this?

 

[Srki1982]

As you can see above, I thought I've solved it but I still have problems with high stresses... Hope someone can help me out here

 

[BlasMolero]

Dear Srki1982,
I have re-do your FEMAP model to mesh with SHELL 2-D CQUAD4 elements, here you are the animation of displacement results of the linear static analysis (SOL101) using NX NASTRAN:

The following plot shows the vonMises stress results in bot TOP & BOT faces of Shell elements, as a result of the material properties used, the loads & constraints used in your model, the geometry & model dimmensiones, the element mesh quality, etc.. Assuming the YIELD STRESS of the stainless steel material is around say 275 MPa, then is obvious that the model dimensions, material properties, boundary condictions, etc.. are not correct to account with the pressure load applied inside the tube.

The following picture shows in detail the mesh used with the clamps:

Please check your model, investigating the material properties used I see some incoherence in units, in the following material property the YOUNG MODULES is defined in PSI units, then a mixing properties of PSI & MPA exist in your model. Please check that dimmension units are correct, etc.. if not the results maybe useless ...

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Srki1982]

Hi Blas Molero,

Thanx you so much for taking the time to help me out here. I saw that the material properties for beams was incorrect... simple fault because of fast modelling. Anyway, that doesn't change anything even if I adjust to correct units. If you think about another way; the pipe is just 60,3 mm in diameter meaning that the stresses will not be so high by the internal pressure of 12 bar (1.2 MPa).

I have now tried several different methods (Glued connection, reverse cmd of glued connection, Spider surfaces to RBE2 and than converting RBE2 to RBE3 and now even with complete QUAD element modelling) the result is still not reliable. It cannot be over 500 MPa. The quality of the mesh is good and it is as you can see just a simple model with a simple load of 12 bar in a small pipe. Now, if I cheat and put fixed constraints on pipe curves at the end, the rotation of pipe will of course disappear and the stress levels will drop to 12 MPa on pipe which is a level that is reasonable, but to constraint the pipe in that way is of course wrong in this case. As you can see Blas Molero, I need to have both solids and shell elements, there are many parts in my complete model that cannot just be modeled with QUAD elements and this little section have shared is just an example to learn how to overcome this problem with rotation of the pipe and to learn how to correctly connect shell elements to solid elements. What I can do now is to constraint the pipes curves at the end of both sides but I'm afraid that is a big approximation. Or is it? According to the manual of NX Nastran it is said:
The RBE3 is an interpolation element, which is ideally suited for this application. By using RBE3s, the rotations of the attached grid points is simply slaved to the translations of the adjacent grid points.

But I just simply don't know how to do this. How you done this before?

 

[BlasMolero]

Dear Srki,
Do not get confused with the connecting method choosed between clamps & pipe, the GLUE surface-to-surface is correct here, not other better method exist, forgot at all using RBE2/RBE3 rigid elements, the problem is your design, the method you used to structuraly support the model, do not "blame" FEMAP & NX NASTRAN, it simply tells you what will happens in real life if you do things as designed, FEMAP is a tool for the engineer, but only you are the engineer .... fortunately!!.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Srki1982]

Dear Blas,

I was talking to one calculation engineer that works with ANSYS and he told me that it seems that there are unbalanced forces in my model. If I choose not to have pressure load on the last section of pipe bending the stress is reduced to 130 MPa instead of 466 MPa. See my pictures for better view.
The connection is still chosen to glued between solids and shell and as you can see the last section is cause of this high stresses. But that doesn't seems to be right. The pressure is acting on all sides inside the pipe so it should't give such big difference in the result. Do you have any solution for this?

Best regards

 

[jerza]

Hi,
if is model a bit simple, I used bonded contact between plates (shell) and bricks mention here.

 

[Srki1982]

Hi,

According to NX Nastran manual and BlasMolero here on this forum, glued surface to surface or edge to surface connection should work.
Glue is a simple and effective method to join meshes which are dissimilar. It correctly transfers displacement and loads resulting in a an accurate strain and stress condition at the interface. The grid points on glued edges and surfaces do not need to be coincident.

So I needed to remodell and put the pipe clamp on the side where it receive mostly compressed stress and not so much bending stress. It reduced the stress to 101 MPa on the solid element instead of 460-470 MPa.

Thank you