Learning Forum

[Devaiah]

I have a cylindrical shell, I need to apply a moment(UDL) along the edge on one of its edges such that it is normal to the surface along the edge of the cylinder.

Requesting for some info on the above--

Thank you.

[Sandeep Medikonda]

Hi Devaiah, 

Right click on your analysis settings and insert a moment as shown:

Change the Define by to Components and enter a value for the moment, which would be 'Z' in your case.

Regards,

Sandeep

 

[peteroznewman]

Hi Devaiah,

Sandeep says to use components, which is useful, but he describes a moment that would twist the tube along its axis.

Your sketch looks to me like you want to apply a moment to the edge in a way that would turn the tube inside out, or begin to roll it down its length. I don't know of a simple way to do that. It is simple to define a cylindrical coordinate system and apply a radial force to stretch the opening of the tube radially.

An inelegant and imprecise method is to slice the tube up and apply individual moments to the edge segments using components. I made 4 slices to get 8 edge segments and applied a moment to two of them.

I hope someone will reply with a more elegant way to to that.

Regards,

Peter

ANSYS 19.1 archive attached.

[Devaiah]

Hi Mr Sandeep,

  Thank you for the answer at the earliest.

But the problem as I mentioned above is that the moment should act normal to the surface at each and every point along the edge.

 

By using components, it satisfies the normal condition at only one of the points along that edge as shown above.

I'm trying to verify an analytical result using FEA as shown below.

 

Here as the author mentions, both the shear force and a bending moment is applied along that edge and is normal to each and every point along the edge.

Any info in the above would be great.

Thanks a lot.

 

Regards,

Devaiah

[Devaiah]

Hi Peter,

 Firstly thanks a lot for the quick reply. 

Wow that's actually very close to how I want the moments to be applied.

Let me slice it up and compare the generated results with the analytical solution and comeback to you.

 

Thanks and Regards,

Devaiah

[peteroznewman]

Hi Devaiah,

I recommend an axisymmetric model in ANSYS. That means a radial slice is modeled, but the full 3D equations and all components,including hoop stress, are computed. I believe you can apply a moment to that edge in an axisymmetric model.

Regards,

Peter

[Devaiah]

Thanks for the additional info as well Peter.

I'll try that out as well and comeback with the results.

 

Regards,

Devaiah

[peteroznewman]

Here is the axisymmetric model. I had to create a surface, but then I could apply a moment to the edge.

If you revolve this result around the axis, that is the 3D solution.

The point the author is making in the book is that these moments (and shear forces that you didn't mention) die out quickly and can be neglected compared with the other terms in the analytical derivation.

Regards,

Peter

ANSYS 19.1 archive attached.

[Devaiah]

Hey Peter,

Thanks a lot.

I'd been stuck with this for more than a week now.

Really grateful to you.

 

Regards,

Devaiah

[Devaiah]

Hi Peter,

 

 I observed the file that you had attached. The element chosen is a plane element.

I had to use a shell element for the above analysis.

Any other means by which I can use a shell181 element as well as conform with the moment along the edge?

 

Thanks and Regards,

Devaiah

[peteroznewman]

Hi Devaiah,

The only way I know is the imprecise method of slicing the tube into segments and applying the different orientations of moment to those individual segments.

The textbook also mentions shear force Q, which is illustrated as a radial force. That can be done with a single Cylindrical coordinate system and a single force applied to the circular edge.

Regards,

Peter

[Devaiah]

Thank you Peter.

Let me try that out.

 

Regards,

Devaiah

[Thomas M]

 

 

I have the same issue, but my geometry is not axissyemtric.

Having a moment with its normal following the curvature of a line seems like a simple ask. My application is for a curved structural beam.

Edit:
I was able to apply the moment as I intended using a Mechanical APDL block, APDL code,  and excel.
First, I dragged the Mechanical APDL block onto the Model in the project schematic. I then edited the Mechanical APDL Analysis, and used file>save as. This made a copy of the entire model (including named selection for my edge).
Then, in APDL I used cmsel,s,edgeName and nlis to get the node list. I copied this list to excel, space delimted (300 nodes).
I then sorted the nodes in increasing z order.
1. I made a series of colunms for  nsel,s,node,NodeNumber    This selects each node individually. this gets dragged down for all nodes.
2. I made a column for the local,#,xcoord,ycoord,zcoord,0,thyz,0 command. This uses geometry to rotate the nodal coordinate system so that its aligned to its neighbour. I also set the origin of the coordinate to be the node xyz. This gets dragged down for every node.
3. set active coordinate system: csys,NodeCoordSys (from above) for every node. drag down.
4. generate a copy of the node at a particular distance away from the edge: This will be the normal direction because of the csys command previous.  ngen,2,1000000,nodeNumber . Drag down for every node.
5. Run the nrot,all,all command each time you change csys (drag down for every node).
6. couple the offset node to the original node.   cp,next,all,originalNodeNumber,OffsetNodeNumber (drag down for every node).
7. apply force to each node:  f,NodeNumber,fz (force direction in its nodal coordinate system),value (drag down for every node).

Combine and sort all of these 7 steps so that they execute 1->7 for each node.
i.e.
nsel,s,node,,221007,,,,
local,20,0,3.125,-107.75,9.3758,0,90,0
csys,20,,,,,,,
ngen,2,1000000,221007,,,6,0,-1.5
cp,next,all,221007,1221007,,,,
nrot,all,all,,,,,,
f,1221007,fz,32.4202,,,,,

nsel,s,node,,221006,,,,
local,21,0,3.125,-107.75,9.7506,0,90,0
csys,21,,,,,,,
ngen,2,1000000,221006,,,6,0,-1.5
cp,next,all,221006,1221006,,,,
nrot,all,all,,,,,,
f,1221006,fz,32.4202,,,,,

….etc

Lastly, assign mass21 elements to the offset nodes. Otherwise, the couple won’t work. Assign an arbitrarly small mass using the real variable (r,1,massInSlinch).:

! Note: cannot use node coupling if the node isn’t attached to a element. Fix: add mass21 elements to free nodes (small mass)
!create,element,type,MASS21,,,,,,,,,,,,,,,
et,5,21,0,1,2,,,,,,,,,,,,,! select an unused element number (in my case 5)
!,,,,,,,,,,,,,,,,,,
!,Define,real,constants,according,to,MASS21,definition,in,the,APDL,Element,Reference,,,,,,
!r,#,mass,!if,kopt(3)=2,,,,,,,,,,,,,,
! mass,per,node=2.10313657437385E-06,slinch
r,1,2.10E-06,,,,,,,,,,,,,,,,
!,,,,,,,,,,,,,,,,,,
type,5,!choose,element,type,5,,,,,,,,,,,,,
real,1,!choose,real,constant,1,,,,,,,,,,,,,
!Define,elements,by,node,according,to,MASS21,definition,in,the,APDL,Element,Reference,,,,,,
en,1221007,1221007
en,1221006,1221006
… for each coupled node

Then, copy this entire pile of code into a command snippet just before the solve. Make sure to start the code snippet with
/prep7
and end the code with
allsel
/solu