Hello, I am a student at Auburn University working on a senior design project. I have been modeling with the student version. My team and I are tasked with designing a 30 foot pole made out of carbon fiber sections. each section has a hex cross section with 1 or two ohles on the same hex face. I ran the sections with laminate plates with properties and layups given by the manufacturer. When I saw the results I noticed drastic drops in stress between elements seen below.
I tried a few different things to try to elimate the error like remeshing and reducing element size. I did check for conicident nodes and found none. The only lead I found is in the right hand rule element directions seen below.
(The pictures are the same section I just find it eaiser to see in the nodal sloution). The elements whose RHR are parellel to the axis have significally less stress than those whose RHR are alligned in the hoop direction. I am trying to get the model to behave more realistically, so is ther a way to set the right hand rule to all be uniformed or is there another solution to get more realistic behavior?
When you refer to the RHR, are you referring to the material direction of the laminates? If so, do you have consistent material direction assigned?
Try aligning the your element directions by using Modify > Update Elements > Orient Plate Normal/First Edge. I would select all of them and align them by a vector. Then rerun your analysis.
This will update the first edge of the shell elements which is used as a part of determining the element coordinate system.
When you are looking at plate element forces, they are oriented in the element coordinate system, so for results to make sense, you need to make sure the element X and Y directions are aligned for all of the elements of interest. Troy's suggestion above will correct that issue, but also check the element normals to make sure all the normals point the same direction(based on RHR).
Since you are using laminates, you also need to set the material angle for all of those elements. This indicates the 0 degree direction for the layup you create. If you look at ply level stress and strain, this ply level info will be in the "ply" orientation not the element system.
Thank you so much for the help. I did check the normals and they were all pointing away from the center of the pole. I will be updating the model as soon as I can. Thank you all again.
I believe that the model has been fixed. The new stresses seem correct and the nutral axis is in the correct location with the maximum stresses around the hole. Here is what the newest solution looks like. I would load the file but it seems to be larger than the alloted amount. I am rotating the force arround the pole to check different loading conditions.