I am trying to simulate the how defects in glass impact the internal stress of the glass.
I am wondering if I can either; model the defect as a shell component or model it as a solid and tie the solid and shell meshes together. I attached a picture of the shell model with no glass defect as well as my attempt at incorporating a defect into the analysis. in my attempt I am getting stress concentrations on the border of the shell component which leads me to believe I am missing some contact setting. Both pictures are looking at the Mises stress and both are subjected to a 4-point bending test under 5 lbs of load.
You can place shell on top of solid and connect them like this: PrePoMax (CalculiX FEA) - Tutorial 11 - Four-point bending of a sandwich composite beam - YouTube
But when it comes to defect modeling, it depends on the type of defect - if it’s some intrusion, crack or something else.
1 Like
Thank you for the tip of using a shell on top.
The defect would be a chip in the glass. It is hard to see, but it is in the second picture. On the center of the long side of the rectangle.
I changed my fixed boundary conditions to replicate how you set them up in your video tutorial 11 and the results are closer to what I was expecting to see. I was previously fixing the translation in the z direction and rotation along the x and y axis. I also made the mesh finer.
You should be able to get nice continuity in Stresses too.
Recall there are some general rules regarding which surface is slave and which one is Master. Try to switch to see if gets better.
I would do the transition far from the area of interest.
EDITED: Upps I see you just solve it. Sorry I didn’t refresh before posting. 
1 Like
No problem, I was wondering if your image consist of 4 shells? and based on what you said about the transition being far from the area of interest, does it look like the image I uploaded that the transition location is acceptable?
Actually, this could be a good case for submodeling analysis.
2 Likes
My model are two shells and two solids.
That’s a very good question. I recently ask for some help and guidance about it in other forum but there was no answer.
I see this in some way related with the Saint-Venant’s principle. It is formulated for loads but we could read BC’s by their equivalent reaction force.
Translated would be something like: “… the difference between the effects of two different but statically equivalent loads/ (boundary conditions) become very small at sufficiently large distances from the load/( boundary conditions)”.
Then, one way to minimize any undesirable side effect of BC’s, mesh discontinuities, contacts, load uncertainties, would be to (if possible) set them as far as possible to the area of interest.
I guess the question is :
Âż Which is sufficiently large distance?
ÂżHow much should I extent my sub model from the point of interest to be representative?.
I actually don’t have a rigorous answer more than trying to increase distance of any contact close the area of interest if I detect sgnificant stress variations in the area (like the ones in the picture)
Yeah, it’s just a matter of the user’s judgment. But submodel results overlaid on global model results (with the same legend range) can show you if the boundaries of your submodel are sufficiently far from the region of interest. The results should coincide at the boundary.
Thanks FEAnalyst,
My only references about safety distances to discontinuities come from mechanical design codes not thought for FEA.
References like “The distance between two weld joints should be 4 times the pipe wall thickness or one time the diameter of pipe but never closer than 1.5 inch”
That is supposed to avoid undesirable stress interactions and set valid conditions for the solutions to be generalizable.
My intuition says to keep the stressed area away from too many things going on around. If I can choose , I would extend the contact area @ceiynck example outside the green color change even if there is perfect continuity of stresses in that area.
As I say there is not a rigorous base to affirm that.
My original doubt was related on how long I should extend my beams when modeling steel connections. As far as I have seen on professional software, it seems beams end where stresses become “homogeneous”. Like in this picture taken from IDEA Statica. I hope they don’t mind I post it here.
it depends on modeling of boundary condition (support/load), are use rigid body or coupling?
for coupling it may not differs greatly if someone only extent members shortly, but not for rigid body due to over-constrained condition.
i’m usually use three to four times greater values of member width or depth. at final steps of review, then the boundaries change to coupling type.
Hi, Synt,
Thank you very much for sharing. Nobody talks about this point in books or good practices or I haven’t been able to find it.
About distributing, it doesn’t work in MECWAY and it is not implemented in Prepomax.
@Matej . ÂżAre you planning to implement those coupling options ?
Thank again and regards.
There was a discussion about the implementation of those features here: RBE3 integration in PrepoMax (Kinematic & Distributing Coupling)
Distributing coupling constraints are quite tricky in CalculiX.
it can be checked by sub-modeling or partial model using free-body diagrams. an example of vertical members of square hollow section in vierendeel truss, it will deformed out of original sections due to compression forces or opposite in tension.
rigid body and reference nodes approach is violating this compatibility.
right, it’s not general way to define boundary condition for both the loads and support or prescribed displacement / rotation.
required the working flow to be separated,
- Load type using
*couplingwith*distributingkeywords - Support type or Prescribed displacement (translation/rotation) using
*couplingwith*kinematickeywords
need more steps and effort to properly define of boundary condition from sub-structure or partial model such as Disla case shown above.