Another question is about the structural error. Because the contact, I have the structural error so large in the contact surface. I think that the mesh maybe better. Despite this, the strctural error will no be 0. Is there any problem with it?If I do the convergence test, refining the mesh, and the results are so similar, 3% is the difference between them.
So I do not know how I consider this ansys structural error in my thesis.
Fabricio, please read this discussion for an answer on how to report numerical error in your model.
You should read some references on Joint Stiffness Analysis to understand how a fastener holds a joint together and the proper design of that joint to bear the applied loads without separation. You can create a similar graph to the one below for your joint.
If you have detailed questions related to your specific model, please archive and attach your .wbpz file to your reply.
Fabricio, here is another way to plot the joint force analysis, by displacements.
When preloading, the bolt gets a tensile force Fb. The joint members are subjected to an equally large compression force Fj. These forces are introduced during preloading and are usually denoted by Fp (Blickford & Nassar 1998), figure 1 is a joint diagram that shows the relation between force and deflection.
Figure 1 — Force deflection diagram of a assembled joint, without external force F
When external force Fe is applied to the bolted joint the force relation between Fb and Fj changes, Figure 2 shows the relation between forces when applying external load.
Figure 2 — Force deflection diagram for bolt with external load applied.
The more external load that is put on the joint, the less force will clamp the joint material. The external load that is so high that the clamping force Fj falls to zero is a called the critical load (Bickford & Nassar, 1998). If the external forces are higher than the critical load the joint material cannot absorb part of the load, hence the forces will be absorbed entirely by the bolt. If the load is cyclic and above critical load it can lead to rapid fatigue failure.
Here is a reference that explains joints in more detail.
Hello Peter, I understand the "prying forces"
But I do not understand, why in the exact momment that I apply the load, the safety factor reaches values under of 1. If you see the Maximum Principal Stress, to compare the Safety Factor, that is Slim/Sigma1, the maximum principal stress, is under the yield stress.
I think that is wrong, beacuse the safety factor should compare the normal Y stress (in this case) with material yields stress. I think that I have to change the limits, but I do not know where I change it. Can you help me with it?
Thank you very much!!
Peter, could you help me?I do not know what is happening, and I am not trusting in the results.
I was away last week at a wonderful conference on FEA and had little time for this board.
I downloaded and solved the model attached above.
You ask why does the Safety Factor drop below 1 after bolt is preloaded at T=1.
My first point is the Safety Factor plots are not very useful with materials that include plasticity.
The Stress Tool safety factor default uses Max Equiv. Stress and compares with the Tensile Yield of the material.
Max Equivalent Stress at T=1 is 286 MPa and the Yield Strength of the material is 250 MPa so 250/286 = 0.873.
You can change the Stress tool to use another component of stress.
If you choose Max Tensile, then you will get this result for that body at T=1.
Did you do a mesh refinement study to see if this result will change with a finer mesh?
Yes, I am trying to refine the mesh, but the results, using the safety factor, are wrong, I think that because I am using plasticity. if I compare the Y normal stress with the yield stress, the results are neralier the reality. So I am comparing the yield material stress with the Y normal stress, it is ok, isn't it?
I do not understand the peak stress in the beam, that is resulting. If you see the results below
And if you see the probe normal Y stress, in the same element, or node, at the same time:
I did not understand it.
My first point is the Safety Factor plots are not very useful with materials that include plasticity (repeated from above).
My second point is you are using contact elements in the peak stress area. Don't do that. You have no visibility to those elements. Do what I said before and slice the base on the planes of the beam, and use Node Merge so there are no contact elements between the beam and the base.
My third point is that once you use plasticity, stop looking at stress and start looking at strain. The failure criterion is Equivalent Total Strain < Elongation to avoid failure. The safety factor is Elongation/Equivalent Total Strain.
Peter, I do not understand when you say: "slice the base on the planes of the beam". Should I slice the base on 8 planes, like the picture below?
or is the anye slice type by surface or solid?
Thank you, very much Peter!!You are helping me a lot to do my master thesis!
You have understood perfectly. Define the plane using the face of the solid.
Making a plane and a slice should take about 15 seconds each, so you should be done in DM in about 2 minutes!
If you select all the bodies and Form New Part, you don't have to do Node Merge in Mechanical, the mesher will have common nodes automatically because of Shared Topology.
Peter, if I use the slice, I have a problem with the meshing. Because now I have at lot of solids, and the nodes are independent each other, in the plate mesh.
Can you help me?
It doesn't look like you have done the Form New Part in DesignModeler correctly. All bodies that belong to the base or beam that are welded together need to be in one part, the fasteners and baseplate are separate parts. Show me the DM outline or upload the archive.
I would also delete the slicing of the base around the fastener and just use the inflation meshing technique since it makes better element shapes around the hole that are closer to the hex head that is making contact.
Peter, now I do it. The material between beam and plate are different, can if form new part with different materials?
There is a warning now: "Solver pivot warnings or errors have been encountered during the solution. This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues. Check results carefully."
As you said, forming a new part, the plate and beam are bonded, so I took out the contact elements between them. The slicing of the base around the fastener is because the contact, between the plate and bolts, to have any less conatc elements.
The model is attached.
Thank you very much Peter!
Yes Fabricio, you can assign each body a different material, even if it is put in the same part. You can limit how far away contact elements are made by using the Trim Contact setting. I will look at your model soon, but I see only one element through the thickness of the base and baseplate. That is not good and may be the reason for the ill-conditioned matrix.
But the real reason seems to be the mesh is not congruent. Shared topology seems to have failed. Look at how the nodes don't line up.
Remind me which version of ANSYS you are using.
Yeees!!It is what I am trying to do at the moment, more elements thorugh the thickness of the base and baseplate. But, now I have a lot of solids, that is difficul to take eache one. Before, I did an edge sizing through the thickness, but now I have to do the edge sizing in each one edge of the solids. Is there other way to do it?
The version is 18.2.
Fabricio, here is my first mesh that works. Note that I used no mesh controls other than on the fasteners.
[Edit: shared topology failed to connect the mesh in this case, see this post for the diagnostics and corrective action.]
Now, with the slice, to divide the thickness and use edge sizing,take too much time...
When you said: "But the real reason seems to be the mesh is not congruent. Shared topology seems to have failed. Look at how the nodes don't line up.".
Why when I divide in the same number of division, the hole and the side of the square, it was not congruent to hole center?
Thank you!It is being so difficult to model with true results...I need yet to compare with Eurocode, I do not know If will have time enough, I am becoming afraid to do not finnish it.
Peter, your model has the same warning. Can you send me a print of your contacts?Because there are a lot of contacts which are wrong, I think that it happens when I restore the file.
When I said a mesh that works, I meant a mesh that is congruent. You still have to repair all the broken supports, contacts and loads. What I uploaded is not ready to solve. I left that for you as it is getting late here. I will check back in the morning.
Peter, I think that I am the correct way...thank one more time!The warning about the thickness is: "At least one body has been found to have only 1 element in at least 2 directions along with reduced integration. This situation can lead to invalid results or solver pivot errors. Consider changing to full integration element control or meshing with more elements. Offending bodies can be identified by Right-clicking in the Geometry window and choose Go To -> Bodies With One Element Through the Thickness. Refer to Troubleshooting in the Help System for more details."
Just as it is better.
Now I have three problems:
1 - The meshing through the plate thickness, hou can I turin it up, with out selecting edge per edge of the solids?
2 - The meshing between the web and flange of the beam, I use mesh controle with bia along the beam, to turn down the numer of nodes and elements.
The model is attached,
Ansys customers with active commercial software licenses can access the
customer portal and submit support questions. You will need your active account number to register.