hollow cylinder torsion modelling in ABAQUS by rotational displacement 1

[halston]

Hi,

I am trying to solve a simple hollow cylinder torsion problem in ABAQUS 6.7. Instead of applying a moment I'd like to apply the angle of rotation as a boundary condition to the surface at one end and get the resultant stresses. I first defined a reference point and then a coupling constraint between the RF and the surface that I wanted to apply the torque and then applied a moment on the RP. It works good.
Actually I don't have any idea of the amount of torque but I know the angle of rotation. So, I have to define a "displacement/rotation" BC to solve the problem. I followed the same procedure as when I'm applying a moment but it's not working. I rotate the cylinder 1 degree and the stresses are in the order of e-10.
Can anyone help me with this? Thanks.

 

[rstupplebeen]

I can't remember if Abaqus is in degrees or radians. I would check that if your stress of e-10 seems inappropriate. I would also check that your coupling is only for the rotation DOF you are interested in. I hope this helps.

Rob

Rob Stupplebeen

 

[vumat721]

Abaqus uses radians.

What are the stresses when you apply a moment? For the case when you apply a moment, you can output the rotation and torque from the reference node to the history data by requesting TM and UR. I would then apply this rotation in your case that is rotation driven and see if the stress levels are the same. (which for a linear elastic material they will be)

 

[corus]

1e-10 is another way of saying the stresses are zero. Check the displaced shape to make sure it's what you expect. 1 radian must be about 60 degrees so the stresses would be significant, presuming you've restrained it somewhere else?

corus

 

[halston]

Thank you all for your replies.

The unit of rotation in Abaqus is radians. So when I apply 1 degree of rotation I convert it to radian (0.0174) and then I enter it in ABAQUS. I do the coupling for all 6 degrees of freedom between the RF and the surface.

When I apply a moment(100 Nm) the Von Mises stress is around 800-900 MPa for the material that I'm using (EN25 Steel). I give ABAQUS both elastic and plastic data. For this amount of torque the rotation on the outer surface is around 4 degrees. So for 1 degree of rotation I should get a considerable amount of stress (not 1e-10).

I also checked the displaced shape. There is no change in the geometry. Deformed and Undeformed shapes are exactly the same (It should be because the stress is almost zero). I have encastered the cylinder on the other end.

Please let me know if you can think of any solution to this problem.

 

[vumat721]

You could try another modeling approach. Instead of the coupling, try tieing a rigid plate to the end of your tube. Then, apply your rotation/moment to the rigid plate's reference node.

 

[rstupplebeen]

If the model is this simple post it and we can probably help more.

Rob Stupplebeen

 

[halston]

How can I create a rigid plate and tie it to the end of the cylinder?

I've attached the file to this message. Please have a look and see if you can possibly help me.

 

[vumat721]

Create an analytical rigid part with a reference point. Then create a surface on the part. Put the part into your assembly and tie that surface to a matching surface on the deformable cylinder.

(Sorry, can't open tars on this computer)

 

[halston]

Ok I'll try to do it.

 

[halston]

This is the .jnl file of the model!

 

[vumat721]

The first thing I noticed in your file is that you are applying your rotation to axis 2 (UR2), but the cylinder is oriented along axis 3, so you should use UR3 to apply your rotation.

Also, you should apply a zero displacement boundary condition to your reference node in all the other DOFs (U1,U2,U3,UR1,UR2).

For your kinematic coupling, only constrain UR3 (remove constraint from UR1 and UR2).

 

[halston]

Thank you for your instructions.

In my kinematic coupling constraint if I constraint all degrees of freedom, then it works very well, but when I just constrain UR3 (as you said), it doesn't work (it is for the case that I'm applying rotational displacement). On the other hand, to get my model with applying moment to work, If I just constrain UR3 it works and otherwise it doesn't. Why is it like that?

 

[vumat721]

Not sure....

You shouldn't have to change the BC's and Constraints when switching from Rotation to Moment control. How are you applying the moment? You should apply it to DOF 6 (which is rotation about axis 3). In the input file, it should look like:

*Cload
<node set>,6,<magnitude>

 

[halston]

I'm applying the moment to DOF 6 (CM3)in moment type edit load dialog box. It's weird!

This is what is shows in the input file:

*Cload
_PickedSet22, 5, 100000.

Why is it 5?

 

[halston]

Oh sorry,

this what it shows in the input file:

*Cload
_PickedSet18, 5, 0.
_PickedSet18, 6, 100000

 

[vumat721]

oh, remove the cload on degree of freedom 5, maybe that will help.