FEM Analysis - LISA

Homebuilt Aircraft & Kit Plane Forum

Help Support Homebuilt Aircraft & Kit Plane Forum:

Matt G.

Well-Known Member
Joined
Nov 16, 2011
Messages
1,265
Location
Kansas, USA
I figured in light of recent discussion on this forum that it might be a good idea for me to share a recent FEM project that others may be able to use as a learning experience. I put this in Hangar Flying since this is for a new glider trailer I'm designing and eventually building for my glider, and not an aircraft itself. If the moderators feel it belongs somewhere else, feel free to move it. Anyway...

I'm in the midst of designing a new steel tube-framed clamshell trailer for my Schempp-Hirth Austria, and one concern I had was the deformation of the sides of the trailer (when the wing is being removed from the trailer) due to the design of wing root cradle I have chosen. The wing root cradle is shown below. The view is looking right and slightly aft; the left front corner of the trailer is visible (with many things hidden for clarity).

dolly.jpg

This fixture applies a lateral load to the trailer sides. It is not a large load (27 lb static, but more assuming some wind...TBD later). This is a concern to me, as the sides of the trailer are not braced to anything at the rear of the trailer, thus making the uprights cantilever beams. This is not ideal, but there cannot be bracing since the inside of the trailer must obviously remain unobstructed. I decided to do some light finite element analysis of this problem for several reasons:

-Assuming that this lateral load is applied to the aft-most vertical member only is not realistic, as some portion of the load is transferred through the top rail of the trailer side to other vertical members.
-Assuming that the vertical members are a fixed-end cantilever beam means that torsion is applied to the lower frame rail, and some deformation will result due to this. This cannot easily be estimated by hand.
-A typical truss hand analysis is not valid because the members all carry bending moments through their joints with other members.

Step one is to construct the model. There are two sizes of tubing used for the frame, plus a third for the tongue. The gray members are 1.75" x 0.125" wall square tubing; the blue members are 1" x 0.078" wall square tubing; the tongue (purple) is 3" x 0.1875" square tubing.

Model.jpg

Like I have mentioned elsewhere, LISA is pretty clunky for defining the mesh (although not as bad as a couple other "free" FEM packages I've tried). It took me 2.5 hours to more or less manually define all of the nodes and elements (this model contains around 700 elements). This would have taken maybe 45 minutes at most in FEMAP or a similar commercial pre-processor. I used all beam elements, as I needed to model bending and transfer bending moments at the intersections of the members. With the exception of the tongue, each member has at least five elements between intersecting members. At the end, I'll explain the mesh density. The tongue has four elements in a couple of places, but it is so far from the applied loads and the area of interest that I don't care if the results aren't as accurate.

The model is constrained in the vertical (Y direction) at the tongue and the axle mount on either side, as well as the two aft corners of the trailer, as they will be supported when the glider is being assembled. The left axle mount has all three displacement degrees of freedom constrained, and the right axle mount has a fore/aft (Z direction) displacement constraint to keep the model from rotating around the LHS axle support. If perfectly balanced load cases are applied, this is not necessary, but in this case it helped me find and correct an error in the logic of my loads application (more on that later).

The 27 lb lateral load from the wing root dolly is split between the two wheels on the dolly, as is the 120 lb vertical load applied to the floor. Due to the lack of the trailer floor in this model, I could not apply the vertical loads in an accurate location, but this will not affect the displacement I desire. There is also a 27lb lateral load at the floor reacting the lateral load applied to the trailer side, which I initially neglected. Below are the displacement results in the X-direction.

Disp_X.jpg

The displacement of around 1/8" is what I was hoping for, so now it's time to do some checks on the model to make sure this result will be valid. First, I plotted the deformations with a large scale factor so I could see that I was getting moment continuity at the joints. If there was no moment continuity, the angles at the joints would vary greatly from their original values. Everything looks ok here:

deformed_X.jpg

I started paging through the various outputs of bending, shear, torsion etc, and noticed something odd in one of the bending moment plots.

bendingmoment_unbalanced.jpg

Notice the red areas aft of the axle attachment, and also the deformed shape in the previous image; these bending loads don't make any sense and are because I have constrained both axle mounts in the fore/aft direction. These bending moments mean the entire trailer is trying to rotate. As you recall, I neglected the lateral reactions from the wing dolly at the floor, but this makes the applied loads unbalanced, which causes a 'hot spot' in the structure that doesn't actually exist. This is why you have to be really careful with your inputs in a finite element analysis. I have years of experience with this, and for the sake of analysis simplicity, I neglected something I didn't think would matter...but it did, and that was not obvious until I was poring over the results. I next added the lateral load at the floor so I would have a balanced load case. I re-ran the model and checked the bending moment output again. Now, the trauma is contained to the area where the loads are applied, and there are no far-field hot spots.

bendingmoment_balanced.jpg

The last step was to make sure that the mesh density I had selected was appropriate. To do this, I modeled one of the vertical members on the side by itself as a cantilever beam, 24" long made from 1x1x0.078" square tubing. I used five elements along the length of the same formulation as those in my actual model. I applied a token transverse load of 25 lb at the end.

validation_results.jpg

The maximum displacement is 0.09677". Per Roark's Formulas for Stress and Strain, the deflection at the end of a cantilever beam of length L with load P is PL^3/3EI. Assuming E = 29e6 psi and the moment of inertia of the cross section, I calculate a deflection of 0.09678". This correlates very well with the simple test FEM, so my results should correlate well with any realistic hand analysis I could attempt to perform.

Note that there has been no mention of stresses in this; this trailer has been sized by similarity to others, and a few simplifications I have made in the construction of my FEM may preclude me from extracting accurate stresses from it. If I were interested in stresses, I would have to modify my model. This is a major pitfall of finite element analysis; depending on what you are looking for, you may need completely different modeling methods to capture both accurate deflections, loads, and stresses. This example is probably valid for deflections and loads but not stresses.

Now that I've spent the time making this model, I'll probably use it to check various configurations to see if my existing tubing sizes are sufficient, or if I can drop one wall thickness on some of them to save weight.
 

Topaz

Super Moderator
Staff member
Log Member
Joined
Jul 29, 2005
Messages
14,752
Location
Orange County, California
Thanks for taking the time to post this, Matt. Excellent description of both issues and solutions. I especially like that you showed the "error", how you found it, and how you resolved it. Too many worked examples are "perfect" and don't really help the people they suppose to aid.
 
Top