Getting the Moment X Rotation - Steel Bolted Connection

  • 340 Views
  • Last Post 16 June 2018
Fabricio.Urquhart posted this 08 May 2018

Hello,

I would like to plot a moment versus rotation diagram of a bolted connection, to compare with Eurocode-Part 3. Are there any people in the community that did some similar work in Ansys?

I have found a lot of articles and thesis, but neither of them say how they plot this graph. And example of article is attached.

 

I am using solid elements.

 

Thank you,

Regards.

Fabricio

 

 

Order By: Standard | Newest | Votes
peteroznewman posted this 08 May 2018

You have to put the article in a zip file to attach it.

Fabricio.Urquhart posted this 08 May 2018

Hello Peter, I am sending the zip file, thank you very much!

The figure 10 is the diagram that I would like, I have difficult to find the point featured in blue. For you understand, now I am using the contact problems that you helped me, somedays ago. I am applying the geometric nonlinearity theory in Steel boled connectins.

Regards,

Fabricio

Attached Files

peteroznewman posted this 08 May 2018

It seems rotation is really vertical deformation divided by cantilever length.

That seems simple enough.

 

Fabricio.Urquhart posted this 08 May 2018

Thank you for your promt response Peter.

Yes It is simple, but is there anway using like "User defined Result", to write the equation: M (F * Lbeam) in Y axis, and r (Uz / Lbeam) in X axis?

I am looking for it, despite this I am using Excel. But I think that it is possible. I have read some article that was written it, but I could not find the article or site web where I have read.

Thank you, very much.

The question is about  the point featured in blue in the post before. Because my diagram seems to be linear, when it had to be nonlinear, because the contact. The beam that I am using, is W200X80, the beam Mp = 406,9kNm. I would like to do this nonlinearity, when is near of tensile strength.

 

peteroznewman posted this 08 May 2018

Have you added Plasticity to your material model?

  • Liked by
  • Fabricio.Urquhart
Fabricio.Urquhart posted this 08 May 2018

No I have not. Do you you think that is mandatory/indispensable?

Fabricio.Urquhart posted this 08 May 2018

I think that, that problem may be it. But my teacher comments that the geometric nonlinearity has to appear without the material plasticity, I became in doubt with this comments.

peteroznewman posted this 08 May 2018

Plasticity will dominate the nonlinearity. You can run the same model with and without plasticity and show your teacher that plasticity causes a very large change in the shape of the curve.

Fabricio.Urquhart posted this 09 May 2018

Good Peter! I will do it to show her.

Another doubt about Moment X Rotation in Ansys. For the picture below:

The beam length is 1 meter. So the moment will be the force applied. But if I calculate the plate stress:

S = -M/W = -6*M/B*L²

The plate is 400mm X 600 mm. So the stress will be -6*M/(144000cm². For example, force of 24 kN, the minimum plate stress wil be 1 MPa. But the Ansys results were 66,154MPa. So there is something wrong.

I think that the force applied in Area, maybe give differents results. The stress display option was average.

What could be wrong?

 

Thank you very much again Peter!

 

peteroznewman posted this 09 May 2018

Fabricio,

I don't recognize the equations you used above.

The geometry of this model does not fit any simple equation you can find in a textbook.

Trying to use simple equations on geometry that is not simple is what is wrong.

Regards,
Peter

Fabricio.Urquhart posted this 11 May 2018

Peter, I am trying to calibrate the model, that this why I am comparing with some simple equations. For example a cantilever beam displacement by the beam theory. A cantilever beam with a concentrade load in the extreme, has the max displacement:

So E= 20000 kN/cm² I = 12550 cm^4 (approximated, beacuse I am using a commercial steel)

With the model I am finding 17mm the maximum displacement in Z, but with the equation is 2mm. So ten times more. I am looking for the error in the model, but I am not finding. Can you help me?I am not working with simmetry, beacuse in the future, the load will not bee simmetric.

 

I plotted the graph below to compare, maybe it is easier o understand my difficulty.

 

The model iss attached. I did not attach the complet model, because It would be so big. So I did not attach the results.

Thank you very much!!

Attached Files

Fabricio.Urquhart posted this 11 May 2018

Sorry

L = 100cm. I forgot to write the beam length.

peteroznewman posted this 11 May 2018

Fabricio,

The ANSYS model includes a flexible baseplate and a flexible beam. They both contribute to the tip deflection.
The illustration below is not to scale, but you get the point that the majority of the tip displacement is due to baseplate flexibility.

If you use a fixed support on the edges at the base of the beam instead of the bolts, then the ANSYS model will give you a very similar displacement to the cantilever beam equation, which assumes a perfectly rigid baseplate.

Fabricio.Urquhart posted this 23 May 2018

Peter,

In the graph below, the "Bisection Occured" means the moment at which the plastification started, doesn't it?In other words, the yield strength was reached.

Thank you!

peteroznewman posted this 23 May 2018

You can get bisection in a model without plasticity. It is not necessarily linked.

I will oversimplify this to describe it briefly. In a nonlinear analysis, a small portion of the total load, say 20% is first attempted, which is called a substep. The solver inverts the stiffness matrix to solve for the unknown displacements, then plugs them back in to see if the force is within a small tolerance of being in equilibrium. That is called an iteration. If the tolerance was exceeded, the solver updates the stiffness matrix and inverts it to solve for revised unknown displacements and repeats the check for being in equilibrium. In your image above, it took 12 iterations for the force error to drop below the tolerance, which is called the convergence criterion and we say the substep has converged. Having successfully solved the first 20% of the load, it attempts to solve the second 20% of the load (the next substep), and the whole iteration process repeats. The second substep took only 3 iterations.

The software has rules built-in to prevent it from iterating too many times, trying to find a set of displacements within the force equilibrium tolerance. For example, it might take 49 iterations to converge on a 20% load increment, but instead, after 10 iterations, the software changes to a 10% load increment and starts a new set of iterations. That is called a bisection. It cuts the load increment in half. Then it uses 3 iterations to find equilibrium for the first 10% load increment, and it increments another 10% and uses another 3 iterations to find equilibrium for that substep.  So in this example, it took 16 iterations to attempt 20%, give up, then succeed at 10% twice in 3 iterations each. This is better than taking 49 iterations to get 20%, but if you could have told it to take 10% in the first place, it would have only taken 6 iterations.

This discussion has more info.

Fabricio.Urquhart posted this 23 May 2018

Peter, thank you. Now "bisection occured" make sense.

 

But I have difficult to understand, using bolt pre-tension, when the plastification starts. I lock the pre-tension load in the first step. Then I use the model load, and increase subtep by substep.

 

But if I analyse the bolt normal tension, in the begining of the second step, it reached the plastification, I think that it occured because of bolt pre-tension.

peteroznewman posted this 23 May 2018

In step 1, you ramp on the tension force in the bolt shank. If the pretension force is high enough, you can get plastic strain in the model at step 1. You can plot plastic strain and find out where that is happening and by how much. If you don't want plastic strain in step 1, then change the material, the pretension or the geometry.

In step 2, the bolt length is locked, while the load is applied to the structure. You can have a second plot for time=2 for plastic strain to see how much that changed after the structural load was applied.

Fabricio.Urquhart posted this 24 May 2018

Ok.

But as you see in the picture, in the step 1, the bolt normal stress is high, almost the yield stress. So when the load is applied, the yield stress is reached in the first substeps. So with low load, the bolt plasticity is reached. You can see what I am trying to say in the picture below:

peteroznewman posted this 25 May 2018

The bolts are pretensioned to nearly the yield point. That is good and correct.

Then the load is applied. The stress of the parts approaches yield. That is also fine. 

It seems you are done. What is your question?

Fabricio.Urquhart posted this 25 May 2018

There is something wrong, because the stress of the parts approaches yield so early, with a very very low load.

The question is, sorry if it is obvious, but if the pretension is nearly the yield stress, the next load applied will do the bolt starts the plasticity, won't it?

Thank you!

Fabricio.Urquhart posted this 25 May 2018

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.

Thank you!

Fabricio

peteroznewman posted this 25 May 2018

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.

Kind regards,
Peter

peteroznewman posted this 25 May 2018

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.

Fabricio.Urquhart posted this 04 June 2018

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!!

 

 

Attached Files

Fabricio.Urquhart posted this 11 June 2018

Peter, could you help me?I do not know what is happening, and I am not trusting in the results.

Regards

peteroznewman posted this 12 June 2018

Dear Fabricio,

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?

Kind regards,
Peter

Fabricio.Urquhart posted this 14 June 2018

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

Solid Peak Stress very very different of the node stress.

 

And if you see the probe normal Y stress, in the same element, or node, at the same time:

 

I did not understand it.

 

peteroznewman posted this 14 June 2018

Dear Fabricio,

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.

Kind regards,

Peter

Fabricio.Urquhart posted this 14 June 2018

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!

 

peteroznewman posted this 14 June 2018

Dear Fabricio,

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.

Warm regards,

Peter

Show More Posts
Close