Displacements out of node location 1

[andreamordini]

Hallo all,
I have a model of beam elements and I need to extract from the solution the displacements in some particular positions which do not coincide with the FE nodes.
How can I do this?

Andrea

-------------------------------------------
Andrea Mordini, Civil Engineer, Ph.D.

http://www.andreamordini.com

-------------------------------------------

 

[cbrn]

Hi,
no way. Export the results to Excel, then plot against longitudinal position, make a least-squares interpolation curve, take its equation and then apply it to the coordinates you need...
Equivalent workaround: make a path with a number of divisions set in such a way it matches the positions you want (if it is possible).

Regards

 

[meshparts]

Cbrn, never say never...

One can use the command

*MOPER,ParR,Par1,MAP,Par2,Par3

For example, you want to interpolate the displacements ux, uy and uz at Nout output nodes from the displacements of Nin nodes. Then you must define 4 array parameters:

! coordinate locations at which to interpolate.
*dim,Par1,array,Nout,3

! array containing the interpolated values
*dim,ParR,array,Nout,3

! array of values to be interpolated
*dim,Par2,array,Nin,3

! array of coordinate locations corresponding to the values in Par2
*dim,Par3,array,Nin,3


Regards,
Alex

 

[pja]

If you aren't afraid of a little coding you can use your nodal results along with the shape functions for the elements which contain the points you are interested in. Otherwise just do a linear interpolation via *MOPER. The method you choose would depend upon how accurate you want your interpolation along with how many of these points you are interested in(and your knowledge of the shape functions used in the analysis)

 

[cbrn]

Hi,
Alex, great tip! I had totally forgotten it... a star for you!
Now I feel a bit stupid because in many analyses I also had to perform something like this and I did it with Excel... Well, I save myself in corner because by doing so I can obtain much better "operability" on my data as well as better graphs when needed...
Pja, you're also right, shape functions can be retrieved in any good FE-theory book, given that Ansys' theory manual describes the math each element type relies upon. But in this case it's only intra-element interpolation, for inter-element interpolation one has to do piecewise-functions interpolation or, as you say, *MOPER.

Thank you to all,

Regards

 

[andreamordini]

Thanks for the suggestion.
The problem is that *MOPER works over triangles (surfaces) and therefore, in case of linear elements it does not work...
I have tried with this trick: duplicate each node by moving it by a very small eps and apply the same value to be interpolated also to this node.
But in this case, the Par1 locations are always on the domain border and in some cases, probably due to numerical precision, the searching point are considered outside the domain resulting in very bad values...

andrea


-------------------------------------------
Andrea Mordini, Civil Engineer, Ph.D.

http://www.andreamordini.com

-------------------------------------------

 

[pja]

Intra-element?? Do you mean you want to know the displacement on the interior of an element? If yes then of course you can use the nodes..the displacement at any point INSIDE an element is define by the nodal dof and the shape functions.

 

[meshparts]

Andrea,

There are 2 possibilities:

1) Like Pja said, shape functions

2) Define more beam elements, by dividig one beam element into more beam elements, so that you get nodes also at the inner locations. The you can directly get the displacements.

Regards,
Alex