Reaction Moments on Grille Vane

[generaluday]

Hello!

I'm trying to determine the torque required to hold a grille vane in position when wind at a certain velocity is blowing against it.

I obtained the pressure profiles on the vane from a CFD analysis, mapped those results onto an FEA mesh, and solved the analysis. I constrained one end of the shaft (about the axis of which the vane rotates - the Z axis) completely, and constrained the other end in plane, i.e., Tx, Ty, Tz, Rx, Ry.

Firstly, is this the right set of constraints for a case such as this? Secondly, how do I obtain the reaction moments about the Z axis which gives me the torque required to hold the vane in place?

I tried the "Freebody Display" but I wasn't able to get the reaction moments from it.

 

[rb1957]

without seeing the structure, maybe pinning the two supports (maybe Fz at only one end) and constrain Mz at one end.

don't know why Mz isn't showing in free-body display ... check that the "show moments" box is ticked.

if not, print the output and look it up in the f06 file.

 

[generaluday]

I tried everything that you suggested, but nothing worked. I even looked in the F06 file, but found nothing of interest.

I even simplified the model to a simple rectangular plate with 2 cylindrical pivots on the opposite faces, fixed the pivots, applied opposing forces on the top and bottom edges of the plate, and solved the analysis. I just couldn't figure out a way to obtain the reaction moments in Femap.

This is a simple problem in which the reaction moments can be calculated manually, but there's gotta be a way to get calculate them for more complicated problems analytically. I know how to get the moments in ANSYS, but I can't use that at work.

Blas, anyone else, any ideas?

 

[rb1957]

sorry, i really don't understand ... the "preamble" in the f06 file (before model detail results) includes (depending on what things you ask FeMap to print) ... "OLOAD RESULTANT" which shows the resultants of your applied loads about the origin (which may or may not be your hinge point), "FORCES AT SINGLE-POINT CONSTRAINTS" which are the constraints you set up in FeMap, and somewhere there has to be an element transmitting the moment to the constraint.

what does your deflected shape look like ?

 

[generaluday]

Well, nevermind the F06 file, but the explanation was certainly helpful.

All I had to do was create a node along the axis of the shaft on each end, a little outside the outer shaft surfaces, and connect each node to all the nodes on the outer surfaces using rigid elements, and then constrain those two nodes appropriately, i.e., one node completely, and the other about Tx, Ty, Tz, Rx, Ry. I can now see the reaction moment about the Z axis on the latter node when I do the freebody display.

Thanks for the help though!

 

[rb1957]

ah, so you had a shell model of a tube ... and RBEing the shell to a central node would provide a convenient point to constrain.

if you constrain each node on a tube surface as fully pinned, you are restaining the three moments as well, only you'd need to do some math to extract the results.

 

[generaluday]

Oh no, the shaft is not a hollow tube, but I don't know what I was thinking when I was expecting reaction moments on solid element nodes, which do not even have rotational DOFs. The point of the rigid elements connecting a node to the outer shaft surfaces on each end was to completely fix one (where the reaction moment can be extracted) and allow the other to rotate freely about the Z. Now I just have to fine tune it to account for the actual assembly geometry and conditions.

 

[rb1957]

so you modelled the beam as solid elements, which as you know now only have X, Y, Z freedoms at the nodes. so yes, you RBE the end face to a point on the CL and constrain that