Getting the Moment X Rotation - Steel Bolted Connection

  • 762 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

Fabricio.Urquhart posted this 15 June 2018

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?

peteroznewman posted this 15 June 2018

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.

Fabricio.Urquhart posted this 15 June 2018

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!

Attached Files

peteroznewman posted this 15 June 2018

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.

Fabricio.Urquhart posted this 15 June 2018

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.

peteroznewman posted this 15 June 2018

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.]

 

Attached Files

Fabricio.Urquhart posted this 15 June 2018

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.

 

Fabricio.Urquhart posted this 15 June 2018

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.

 

Regards.

peteroznewman posted this 15 June 2018

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.

Regards,

Fabricio.Urquhart posted this 15 June 2018

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,

 

 

 

Attached Files

peteroznewman posted this 15 June 2018

But Fabricio, I gave you a mesh with two elements through the thickness, I hoped you would use that.

  • Liked by
  • Fabricio.Urquhart
Fabricio.Urquhart posted this 15 June 2018

I tried to use, but I need a refinement meshing in the hole region, because the contact between plate and washers. So I did the slice in the plate in this region.

In your model the are two elements through the thickness, but It was automatically. In my model, it does not happen automatically, I do not why.

In the hole region now it is ok.

What do you think?

Fabricio.Urquhart posted this 15 June 2018

How can I divide in two or three elements through the thickness if automaticall, it does not happen for me?

 

Thank you!!

peteroznewman posted this 15 June 2018

Fabricio,

The attached archive has a boolean on some solids of the base of the beam, and added Sweep method on the base of the beam that specifies how many elements through the thickness of the base, and an inflation mesh control on the hole that specifies how many elements to inflate around the hole. I said 7 elements, but that is probably too many.

Check the material assignments!

 

Attached Files

Fabricio.Urquhart posted this 15 June 2018

Peter,

The nodes between the beam and plate are not together, linked or merged. Is there any problem?

We started the discussion because this...

Fabricio.Urquhart posted this 15 June 2018

Peter, now I am getting confused, because the nodes are not corresponding...

Fabricio.Urquhart posted this 15 June 2018

Peter, I tried again with your model. But I think that you do not understand, or I did not understand. Your model is not possible to run, becasue the contact between the washers and the plates, the plate area, which you configure contact is so big. And the inflation, you do not separe the plate area in smaller faces.

Another point, we started the discussion, because you said that the pick stress in the beam was occuring becasue there were elements the I was not seeing, that I have to link the beam elements and the plat elements. And in your model it doesn't occur. It is not clear for me.

Sorry, but it is so difficult for me, because I am studying Ansys modelling for the first time. Thank you for being comprehensive with me.

Can you explain better?I tried again to turn the nodes between beam and plate coincident, but it does not happen.

I tried with boolean, I tried with your model, I tried slicing all the solids (that become extremely difficult to sweep small solids). The best meshing that I have reached is below with some comments.

 

So I try came back and use edge size through the thickness plate. Just see:

Ok it divides. But the nodes between beam and plate are different. So I am thinking to come back to my first model. The master thesis example is attached. The model too.

 

Please, can you help me again?In the other softwares are the same problem with the mesh. The people, normally use other softwares as truegrid to do the mesh. I think that Ansys should have a good mesh that take true result to compare with the reality.

As you se the picture below, the elements thtrough the beam length are not necessary, I need a refine mesh in the contact and where I apply the load. SO because this, I use edge size in the beam length with bias 10.

 

Can you point where I am wrong, PLEASE?

 

Fabricio.Urquhart posted this 15 June 2018

Here I did a resume:

1 - The elements in contact, beam and plate, have to be linked or not?

2 - How can I divide small elements through the thickness plate if using sweep it is impossible?

3 - The square, that male contact with washers is parametric, depending on the bolt diameter, so, for me is easy, it is linked with the parameters. So I am keen on using it. I have articles that explain it, and it is my reference in the master thesis. But they use truegrid to do the mesh.

4- What is the meaning of: "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."

5 - The peak stress in the results, is because the nodes that is not  merged or near, or not?Because in your examples it does not. 

6- Modelling beam and plate together, is necessary to create contact elements between them?

7- If I use slice in the plate or beam, I have to use contact between the solids created?

Attached Files

peteroznewman posted this 16 June 2018

Dear Fabricio,

ANSYS can be very frustrating, because in one case, it shows its ability to form a perfect congruent mesh with hex element on the sliced solid with Shared Topology using no mesh controls, and then it fails to form a congruent mesh when some constraints are imposed on the mesh. I think the more bodies that are put into a multi-body part, the less likely the mesher is to form a congruent mesh. You can see why some people use 3rd party meshing software.

If you want hex elements, which you do, slicing is helpful to get hex shaped solids that can have 2, 3, 4 or more elements along edges. If the shared topology is working, then you don't have to do any extra work, as was the case in the 2 element example I provided above. When the shared topology fails, then you have a lot of extra work to do. You can put mesh controls on every edge of every block, set them to hard, and assign Face Meshing so that you get a congruent mesh.

1. For a study that includes large strain plasticity, you do not want contact elements to be in the plastic zone.

2. All the small bodies are sweepable so you can assign the number of divisions along the sweep.

3. Keep the slices around the bolt head as that is useful to you.

4. The meaning is one block is not merged with its neighbors. Add a Modal analysis to find if any pieces are not connected.

5. My examples were not ready for solving.

6. You do not want contact elements to connect the beam to the baseplate where they are welded together since this is where you are likely to see plasticity.

7. I don't know what you mean by splice.

Kind regards,
Peter

Fabricio.Urquhart posted this 16 June 2018

Peter.

1- I need contact elements, to simulate the beam and plate welded, no?Why not?If I don't use, there is a DOF.

2- But how I define along which edge it will sweep?

3- OK.

4 - It happens, I think because the number of slice that I am using, it is possible, isn't it?

5 - OK, but the mesh is important to solve.

6- Ok. But if I form a new part in the design modeler, is the same that beam and plate are welded, isn't it?

7- For example, if I slice a plate between to solids, when I go to the model, it will be 2 different solids in the same part. So it is not necessary to contact it, is it ok?

 

Thank you, very much!

 

peteroznewman posted this 16 June 2018

Dear Fabricio,

1. Contact elements are useful in stitch welded structures to obtain the forces transmitted between members to evaluate weld stress with a hand calculation. If you are not doing a hand calculation of weld stress you don't need contact elements.

2. The sweep direction is specified after you choose a source face. The sweep direction is perpendicular to the source face.

3. OK

4. Yes, I think one of the non-congruent blocks was not connected. A Modal would show that block flying out into space.

5. Once you get a good mesh, there is more work to get it to converge (after the Modal shows that it is connected).

6. Form New Part in DM is to weld the bodies together with Shared Topology. If that fails, then you have to do Node Merge.

7. When Shared Topology works, you don't need contact. When it fails, you do need contact or Node Merge.

I understand you are under a time crunch and I have time to help on Saturday.

 Kind regards,

Peter

peteroznewman posted this 16 June 2018

Fabricio,

Here is an example of using a Modal analysis to check if the mesh is connected.

You have to add the Fixed Support to the Modal system.

In this example, you can see that this body is not connected to its neighbors.

The corrective action is to make a named selection of all the bodies that are in that part, and create a Node Merge that merges the nodes in that group.

Once that is done, the Modal analysis gives a non-zero frequency.

Why should you have to do so much work just because the mesher doesn't do it's job is a good question.

 Now the Static Structural model solves. Note: I had to set all materials to Structural Steel to have Modal run.

Attached Files

Fabricio.Urquhart posted this 16 June 2018

Yes, I think that I am doing all the mesh again, the Shared Topology does not work, and I have to use contact or node merge again.

So the result are the same which I have reached, I am trying again here...

peteroznewman posted this 16 June 2018

Fabrico, I moved your reply to a new discussion because this thread was getting too long (Show More Posts).

I'm glad you have mastered the slicing and mesh controls and mesh edits needed to do this job. It's frustrating for me too.

I have downloaded your model and it is solving now. I will comment on your last post in the new thread.

Kind regards,

Peter

Close