Deformation due to a torque on a pipe 1

[gwang]

I have a tubular structure model in 3D solid element (CTETRA) in Nastran. The model is fixed at one end. I applied a torque at the another end in two ways: 1) a moment applied on a node at the center of the tube and conect to the top edge of the tube through a RBE2 element; 2) apply a radial load on the top surface in cylindrical coordinate system. Both BC give very similar results. What concerns me is that the total deformation of the tube is in a cone shape. Is this correct? I understand that CTETRA does not carry rotational DOF. Please help.

Thanks in advance,

Gary

 

[SWComposites]

No, it is not correct. Your fixed end boundary condition is wrong; you should only be fixing tangential direction displacments and not the radial direction displacements. Also, rigid elements (such as RBE2's) almost always add too much stiffness to the model unless used with extreme care and lots of experience, so you should avoid using them to load the model. I don't see how a radial load on the end can induce a torque in the tube; shouldn't this be a tangential load applied around the periphery of the tube?

 

[jhardy1]

gwang,

Check your actual displacement results very carefully - I suspect you are looking at an exaggerated deformation scale. (I have seen people ask this same question MANY times!)

Every node on the perimeter of the tube / shaft SHOULD have a displacement in the tangential direction only. That is, the actual deformed shape is pure twist. However, when you scale the deformation by a factor of 100, 1000, or whatever, every node APPEARS to move both tangentially and radially, which makes the shaft / tube look as if it is getting diametrically bigger at the free end (i.e. "a cone shape").

Think about a node at theta = 0 degrees (i.e. lying on the X axis). It's true displacement should be a small amount in the Y-axis direction, with zero displacement along X. However, when you scale the displacement by a large multiplier, you find the node appears to move by a significant amount in the Y direction, but still has zero X displacement, so it appears to move both upward and radially outward. This is just an artifact created by viewing with an exaggerated deformation scale.

If you query the displacement results carefully, you should find all of the displacements are purely tangential.

Hope this helps!

 

[Kwan]

I agree with SWComposites. I think that your surface constraint should only be in the tangential direction. You would have to fully fix one node to cover the other DOF's. The nodes must be free to deform in the radial direction. If you try this I think you will see the full tube will reduce in the radial direction (poisson's effect).

SW, I think the RB element isn't causing an issue in this case because it is only tied to one node. Am I wrong on this? If the RB ties two or more nodes together I can see where this could cause a problem.

 

[gwang]

Thanks for all the responses. Regarding the BC, the pipe is fully fixed at one end, or cantilevered. The torsional load is applied at free end. I have tried to constrain the outer diameter in radial direction at the free end and still see the "cone" effect in the deformation plot. I think that it could be caused by the scaling effect like JulianHardy described but I still need to confirm it. One thing I see is that the displacement at X axis is very small but not zero, so it should get scaled at well. I'm using FEMAP for post-processing. Does it have anything to do with it?

 

[SWComposites]

Check to see if the stresses in the tube are a constant value and match the value from a hand analysis. If they are not, then something is wrong with your b.c's and/or loading.

Also, why would you model a tube with solid elements, especially with worthless Tet elements?? Try convering the model to use shell elements. FEMAP can automatically generate a mid-surface in a solid.

 

[gwang]

Good point! Except the actual model has many features that is time consuming to shell it out. I have verified the reaction and stresses and they are OK. I can do a test model with shells to see it does the same thing. Thanks.

 

[jhardy1]

gwang,

All you need to do is look at the numerical displacement results at a few key nodes, as reported by your FEA program.

Like I said, the actual displacement of the perimeter nodes should be purely tangential (assuming an axially symmetric shaft under pure torsion, of course!). This is a very easy check to undertake.

Simply get the (x,y,z) displacement values at the selected nodes, and see which direction the true resultant displacement vectors point. If the true exaggerated vectors are tangential, your analysis results are as expected; if not, you have some sort of problem.

As per my first example, suppose we have a shaft which has a radius of 10 mm , with its axis lying on the Global Z axis. Take a node on the free end at Theta = 0 degrees - i.e. lying on the X-axis, with (x,y) coordinates of (10,0). We expect the actual displacement of this node to be a small displacement in the Global Y direction - perhaps 0.01 mm say. This is too small to see, so we usually plot with an exaggerated displacement scale.

However, when we plot the displaced shape with a scaling factor of 1000 say, the apparent displacement of the node is now 10 mm in the Global Y direction. That is, the undisplaced node coordinate was at (x,y) = (10,0), the true displaced position is (10,0.01), which is visually indistinguishable from the undisplaced position, but the exaggerated displaced node position is plotted at (10,10).

Repeat this example for all the nodes that lie on the perimeter of the free end, and it becomes apparent that when plotted with a large exaggerated deformation scale, the shaft appears to twist AND expand radially at the free end. Like I said, this is just a consequence of plotting with exaggerated deformations.

Hope this helps!

 

[gwang]

Thanks JulianHardy. I calculated the deflection and they are all tangential. That means there is a positive radial deformation at the free end. Should this be the case? I was expecting a pure rotation with no radial expansion on the tube. Thanks.

 

[jhardy1]

gwang,

No, no, NO!!!

If your computed displacements are all tangential (as expected), then there is obviously zero radial expansion. (If there was in fact any radial expansion, you would get a radial displacement component!) As I have tried to explain, the apparent radial expansion at the free end that you see on screen is simply an artifact produced by using exaggerated deformation plotting.

This will be my last posting on this topic, because I don't think I can express myself any more clearly.