Torsion in a cylinder 1

[CNAMITMA]

Hi,
I begin with Ansys and I would like to know how can I apply torsion (a moment) in a cylinder made of rubber (hyperelastic behaviour and HYPER elements) ?
(I modelised an "armature": a rigid cylinder above the rubber cylinder glueded together)

I guess I have to modelise a keypoint or a surface+keypoint linked to my model and apply a moment but how can I do this ?
Any idea ?

Thanks for your help...
Regards

 

[Stringmaker]

Take a look at the RBE3 command in the documentation. This should do what you're trying here. In a nutshell, the RBE3 command creates a system of constraint equations between a master node (where the moment is actually applied) and a set of slave nodes which in effect transmits loads from one to another.

To generalize the procedure:
First, you will need to create a master node which is usually independent from the model itself. This is where you apply the moment at. Then create an array parameter containing all nodes (slave nodes) you wish for the moment to be distributed upon. Typically you would want to choose all nodes on a surface or something of the like. If using the GUI access this by:

Preprocessor->Coupling/Ceqn->Dist F/M at Mstr

Then just enter all pertinent information as prompted by the program.

Good luck,
-Brian

 

[CNAMITMA]

Thank you Brian for your reply

I understand, I was near the solution...
But How can I create this master node, independant from the model ?! creating a node in : prepocessor/modeling/create/node ?

An other thing, the array parameter containing the slave nodes how can create it ? creating a component (selecting the area and then the attached nodes) ?

 

[Stringmaker]

CNAMITMA,
Since you don't know how to create an array parameter let's take an easier approach in doing this. Use the following steps to accomplish what you desire:

1) Create a master node in which the moment will be applied upon as mentioned before. You are correct. This is done by:

Preprocessor->Modeling->Create->Node
or
N,,,,,,,

2) Use the contact wizard to create a multi-point constraint:
-Create New Contact Pair
-Under Target Type select "Pilot Node Only (Advanced Option) then click Next
-In the next prompt select "Pick existing node...". When using the "Pick Entity" you will select the node which you created to be the master node where the moment will be applied then Next.
-As the contact surface select the nodes attached to the appropriate areas where the moment will be applied.
-Set the Constraint Surface Type to be "Force-distributed constraint". Auto Constrained boundary conditions should be adequat for most cases. If not you can change these to your preference.
-Click Next then Finish to complete the contact pair.
-Apply your moment to the node which you previously selected as the master and you're finished.

Hope this works better for you.
-Brian

 

[CNAMITMA]

Thanks for your help and your precisions, torsion is now applied.

But I have another problem, I can't postprocess (read the results) the Mz or any load values of my model, neither for the Rotz. Why ? It's because of the method ?

 

[Stringmaker]

I don't think the method has anything to do with your post processing difficulties. What are you trying to do exactly? When you enter /POST1 and plot vonMises stress or displacement (vector sum) are any results being displayed for these? Are you trying to perform Nodal Calcs to verify the moment is transmitted? You need to be more specific as to what you're attempting before any help can be provided. Also, it may help if you post a copy of your input file here providing it isn't enormous.

 

[CNAMITMA]

In fact I would like to draw in a graph the evolution of the moment versus the angle of the torsion in order to compare the results obtained with ansys and experiences.
Now I only applied torsion to my model but the final aim is to apply torsion and traction. So in a second time i would like to postprocess the tensile load applied for the same reason as before. And finally see the results in a section of the cylinder to see for example the evolution of the hydrostatic pressure (and I don't know how yet).

To answer to your questions : yes I can plot vonMises stress, displacements or others contour nodal solution... but what I want is the values and in the time history postprocessor the moment is also invalid.
My input file is 5 pages long should I post it ?

Thanks again for your help

 

[nodalDOF]

What type of elemnts are you using? Do they have rotational DOF (RX,RY,RZ) ? From above discussion i suppose you are using some solid(brick) elements that doesn't contain rotational DOF. If not you should be able to obtainin moments at the "constrained" nodes.

Nodal..

 

[CNAMITMA]

Hello NodalDOF

I am using hyperelastic elements : SOLID186 (prism when I let the mesh free) and you're right they haven't rotational DOF ! but I added ROTX, ROTY and ROTZ in the preprocessor/element/Add DOF, apparently it isn't enough...
How can I do that? Knowing that I have a non linear material (rubber) modelised in 3D in order to apply torsion and then traction !

Cnamitma

 

[nodalDOF]

Cnamitma, I am sorry. I don't know how to do that. Am also new to FEM/ANSYS.

nodal

 

[pabelooo]

Hello,
I have question about post above.
Cause I am workin with ANSYS not so long and I right now I have to apply torsion moment on cylindric part.
I am working with solid(brick) elements.
I found out that I can apply "moment" by some operations.
First I created new cylyndric coordinate system.
Then I associated desired nodes coordinate systems with that CS by NROTAT,all,,
and finaly I applied force, divided by number of nodes, at that nodes in tangential direction to cylindrical surface (in that case it is Y direction).
It looks ok, It should respond as torsion moment, but I am not sure if solution is corect.
And my second question is if there is possibility to apply torsion moment in other way?
Unfortunatelly explanations above doesn't hit the mark for me....
I could not find procedure similar to extrusion of area around axis, what I consider the best way for such purpose.
If something similar exist I would be gaceful for some advice

bye
Pawel

 

[elogesh]

Hi,

We need to coat surface element over the solid elements.

That is mesh the cylindrical surface with shell63 and then the volume by solid elements.

Option proposed by pabeloo is also good.

Regards,
Logesh

 

[elogesh]

Hi,

One more point the thickness of the shell element should be very low and shouldn't add signficant stiffness in to the system.

Logesh.E

 

[ansysfreak]

Hi

I just wondering if im wrong but isn't it easier to use surface elements. So you can bring forces on the outer site of you solid in radial direction. So you have all the forces that you need to make your model accurately.

Or am I hadding the wrong direction?

Garry