Bolted joint comparison to Eurocode
-
-
[Edit: continuation of this post]
Yes, it happened as I was expecting. I did not use slice, but form the part, and use base face split with mesh control.
The results are the same, I have a peak of stress, and I do not know why. In the Eurocode this connection has Mrd = 100kNm.
With the model Mrd is under 30kNm. There is something wrong in the model. I think that it is impossible to be the weld. As you see, the results are completely different from your model. Really, I don't know where is the problem with the model. If I take the element results, ts the picture below:
If I take probe, in the node of the element before, the results are in the picture below. As you, see, completely different, nearer of the reality, but not reliable.
Just a moment, I will attach the model which is solved.
-
There is something wrong with your model.
Add a Directional Deformation for the weldment part in the Y axis and zoom in to the connection between the beam and the plate. The deformations should be continuous across the corner. Instead there is a 0.7875 mm gap opened up under this load.
Your beam mesh is only connected at 4 nodes, not along the entire edge.
I created a 2-element thick model, and when I do the same check on that as I describe above, it reveals an unconnected thin strip along the back edge, though there is a good connection of the beam to the plate.
The corrective action is to loosen the node merge tolerance and/or add mesh edge controls so that coincident edges have the same number of nodes along them.
-
I changed the Mesh Edit Node Merge group to a 0.5 mm tolerance and said yes to Face to Edge and Edge to Edge. Now 368 nodes were merged.
Here is the new Y directional deformation plot. It appears that there is no longer a "crack" in the mesh.
See this discussion for the question of how to find out about unintended "cracks" before solving.
-
-
Dear Fabricio,
I took the geometry into SpaceClaim and cleaned up all the faces, then made fresh sliced on the weldment and finally used Workbench Share to get the weldment to mesh properly.
When I get a mesh that works, I plan to plot the force vs displacement curve.
Regards,
Peter
-
To get a good mesh around the holes, I imprinted two circles and used Face Meshing to put 3 elements across the width.
This model is solving now...
NOTE: I changed all the materials, so change them back before you use this model!
-
I found a reason why meshing from the earlier DesignModeler geometry was failing to create congruent meshes.
The part shows Shared Topology Method is set to Automatic, which is correct but...
n
... the individual bodies had the Shared Topology Method set to None, which defeats the Part level setting.
All bodies in the Part must be set to Automatic.
-
-
-
-
-
-
-
-
-
PEAK STRESS AT ONE POINT
In the image below, the peak stress is at a point. That is expected. A thin member is pulling away from a thick plate and the interior corner is dead sharp. That creates a stress singularity.
If these materials were elastic, as the element size was reduced, the peak stress would increase without limit.
Fortunately, plasticity has been added to the material model, so the stress is limited by the material model.
If we look at just that one element in the corner and look at an earlier time with less load. Here is the picture:
Note that the yield strength for this material is 345 MPa and the yellow boundary is about to reach an integration point on this element. Now let's look at the stress-time history.
The stress went down after this point. How can that be correct?
Look at the plastic strain on that element. After this point, plastic strain begins.
There is nothing wrong with this model. At the next load increment, this element goes plastic, and reduces stress and the surrounding elements that had lower stress at this time and are still elastic, pick up a little more stress to carry the next load increment, while this corner element sheds some load due to the change to plastic behavior.
-
-
Peter, my strain graph is different of yours. Look at my graph:
Your graph is similar to the minimum strain graph. The maximum you have the same peak. I solved the elastic model minutes ago and saw that in this point the beam reach the plasticity.
But I did not understand why our graphs are different.
The name of the file is: "FTRd - Chapa de Extremidade - 2a linha PF"
The files are all types of verification, discondering the column resistance.
-
-
-
-
-
-
Peter, good morning!
Can you help me, explaning how I use line body orientation?Because element orientation is used to solid or shell bodies. So for line bodies I do not know how I change the orientation. Now I will try to change in the geometry. But is it possible to change in the model?
-
-
Ok. I understood. And the symmetry that I have applied, is it OK for the line bodies?
Another question, is about the load, I will add a load along the beam, and along the beam modelled by solids. So I have two points:
1 - The local buckling that will occure in the beam solid, or with the symmetry, the load is applied along the center line?
2 - Do I have to divide the load for two beacuse the symmetry, yes?
Thank you Peter!!
-
-
I have modeled the cross section with the proprietes of the same solid beam, but the half section, because the symmetry plane, so I think if I apply the load in the half load in the beam, and the same load in the top flange of the solid. It will be Ok. The question was, if the local buckling maybe result different stress results.
The objective is to analyse the stifness of the bolted connection. But now the problem, I think that is the bolts stress, because when the load starts to be applied, the bolts reach the yield stress.
-
-
Peter, thank you!
I will not include localized buckling of I-beam.
I will do those models and find the correct way. After that I show it to you. If I haD difficulty with it, I will ask you.
Ok, something has to give. But the bolt is given before the load is applied. The bolt gave with the pre-load tension. Did you understand?
-
-
-
Fabricio,
This thing that you modeled with the bolt pretension applied, I call that a fastener, you seem to call it a washer.
A fastener can have a head on one end and a nut on the other end (or it goes into a threaded hole on the joint).
A washer is the flat circular piece that goes under the head or the nut to spread the load and reduce the friction.
-
-
-
-
-
-
Using boolean in the bolts, this peak of stress disappear. See the picture below:
Thank you Peter!!
I am learning a lot with you!!!
-
-
-
-
-
@Sandeep, the zip file attachment on this post has a paper with the definitions for Moment and Rotation.
Hello Fabricio,
From the paper, M = PL is equation (4), which is for a point load P at a distance L from the column.
You have used a distributed load, q = 40 kN/m for a length, L = 0.872 for the symmetric half model.
You calculate the beam shear and moment diagrams for your problem. I used an online calculator.
So when q = 40 kN/m, M = 15.21 kNm
Regards,
Peter
-
-
-
Hello.
I would like your opinion about de moment reaction using symmetry.
When I compare the moment in the connection ( Moment reaction plus Horizontal Y Force Reaction multiplied for 2m, that is the column height) with the rotation (beam rotation minus column rotation, extremely near of the connection), have I to multiply for two, becasue the symmetry?I think that it is not necessary if I am comparing with the full solid, is it?
-
-
-
- The topic ‘Bolted joint comparison to Eurocode’ is closed to new replies.
You are navigating away from the AIS Discovery experience