Three Point Bending Constraints

alex · May 2015

Hello
I'm trying to do a simple three point bending simulation. Can anyone advise what would be a good way to model the constraints? My model is basically of a shoe orthotic insole of nylon plastic. This means I can't use the flexible joint because I have curved ends. I have tried applying a load on the central elements and then using a fixed support constraint on the ends, but for a three point bend the object should be able to rotate on the end supports.
I feel like this should be a simple case on my FEA learning journey. A model is only as good as the assumptions after all!
If anyone can offer any ideas I would very much appreciate it.

Victor · May 2015

Hello alex

You can use the "displacement" constraint as a pinned or knife support. Here's an example using both shells and beams. It would be similar for solids.

alex · May 2015

Hi Victor,

Thanks very much for that. It makes sense. I think the forum is a great resource. Instead of answering questions individually, the whole community can share and benefit from the answer.
Alex

Victor · May 2015

Yea I hope that too. Thanks for posting it on here. I answer a lot of similar questions by email. It would be nice if more of that was public and searchable. Feel free to share your results too if they're not confidential.

max · May 2016

Hey there,

I am currently working on a three point bend test for a composite laminate plate. Does anyone know if it would be possible to model two actual cylinder bars instead of the displacement constraints? If so, what would be the constraints for the cylinders and the plates? Any examples would be much appreciated!

My thoughts are that this would model real world conditions more closely than with just knife edge supports.

Max

Victor · May 2016

To model localized crushing at the supports, you would need contact, which you can do by adding the CalculiX solver together with meshes of the cylinders.

To model the changing position and direction of the supports as the deformed shape of the beam changes, you would need large displacement nonlinear analysis. Again you could do this with CalculiX.

I wonder though, isn't the test already designed to minimize the effects of these details? If there's disagreement between the model and the test, are you sure it isn't due to other factors that are easier to correct for?

max · May 2016

Hey Victor,

Thanks for explaining that to me. I will take into consideration what you have just said. For now, I think I will be using the displacement constraints as you have mentioned.

Just another question, when trying to model a composite laminate is there a way to change the angles of different layers? I want to be able to change the lay up angle of the composite layers and model its effects. For example, I might have a carbon epoxy composite as my first layer with its fibres at an angle of 0 degrees and for my second layer i might have a glass epoxy at an angle of 45 degrees. The composites will have orthotropic material properties so I would imagine that the change in angle would affect the results in mecway.

At the moment I am using the "element properties->u and v axes" option to change the angles. U being my Z axis and V being my X axis. From what I understand in the Mecway manual, this means that I am rotating V about U (or X about Z). However, I am not entirely sure if this is doing what I explained above regarding the change in angles for the different layers.

I have attached an example of what I am working on at the moment.

Max

Victor · May 2016

Your method is basically right except for the problem you pointed out - since the angle only rotates about the U axis, it won't change the direction of the U axis itself. It's probably clearer to explicitly set the U axis as components (1,1,0) to get 45 degrees.

Use the "Show element axes" button to show the axis of each element for confirmation. U, V, W are red, green, blue respectively.

max · May 2016

Thank you very much for your help Victor, that made it much easier to understand.

max · May 2016

Hi Victor,

I am trying to model the three point bending test using nonlinear analysis and CCX contact as you have mentioned. However, I could not select the orthotropic properties when trying to change the material properties? Is there anyway to incorporate the orthotropic material properties when using nonlinear analysis?

Thanks
Max

Victor · May 2016

This is a problem. Thanks for pointing it out. You would have to work around it by setting the analysis type as Static 3D to allow entering the data then change to nonlinear for solving. I know this is going to be quite inconvenient sorry.

max · May 2016

Hi Victor,

Thank you very much for letting me know that the non linear still works with orthotropic. I have tried to recreate a three point bending test with pin rollers at the top and at the bottom as mentioned before. However, I have not been successful in obtaining the results in mecway. I have been prompted with this error in the CCX output:
"*ERROR: solution seems to diverge; please try
automatic incrementation; program stops
best solution and residuals are in the frd file"

Can you please advise on what I can do to get the analysis to work? I would really like to get this model to work so I know that it is possible to recreate a three point bend test in mecway with contact. I have attached the model for you to view.

Max

Victor · May 2016

There are several problems. I'm not sure which one(s) are really important but here's what I changed:

Changed the top roller's contact faces from the top to the bottom

Changed Glass_Epoxy's shear modulus units from Pa to GPa

Suppressed one of the force loads just to make it easier to work on

Changed the other force load from nodes to faces. Applying a force uniformly over quadratic element nodes will lead to a choppy deformation. Use faces, not nodes for distributed loads.

Increased the magnitude of the force to make other effects more visible, you might need to turn it down again

Changed the force from constant to ramped up from time=0 to time=1 s. This can help convergence because each increment is only a small change from the previous one.

Turned on automatic incrementation with default initial time step size. See this other comment of mine
http://mecway.com/forum/discussion/comment/1076/#Comment_1076
The next version will have an easier way to turn this on because it should really always be used by default.

You might need to increase the contact stiffnesses because the rollers are penetrating the beam.

max · May 2016

Hi Victor,

I have tried to run the revised model that you have provided but the ccx solver is exited with an error message:
"*ERROR: too many cutbacks
best solution and residuals are in the frd file"

Did you get the same error message when you tried to run the model?

Really appreciate all the advice and changes you have made so far.

max · May 2016

Also, is the transformation of the local axis not allowed in the non linear static 3D analysis? When I set my U axis as 1,0,0 and V axis as 0,1,0 in a static 3D analysis it is allowed. However, when I switch to the non linear analysis the component is highlighted in red and is prompted with this message:
"Some elements have an incorrect local axes orientation option"

Would this be the same case as the orthotropic material properties, where an error message is prompted but the analysis will still be done?

Victor · May 2016

The error messages on red items in the outline tree are for Mecway's internal solver, so you often have to ignore them for CCX.

Now I somehow can't get that to converge anymore so maybe I accidentally changed something else. I suspect the main problem is because if the beam is not in contact with the bar, there's no stiffness to resist the applied force and it can't find any static solution. This is a common issue with multiple parts connected only by contact. Two ways to solve it are:

- Use a displacement for the load instead of a force
- Add weak springs to gently hold it in position so the force can't push it too far away when the contacts are open.

I did the 2nd option and it seems to solve OK now. I also removed the top roller just to make it easier. When you include that, you might need to extrude a weak spring element from it also.

max · May 2016

Hi Victor,

That makes sense now. I have tried the other method you mentioned which was to use a displacement instead of the force as a load while still keeping the rollers. I have also switched the material of the laminate just to simplify the model for now. It seems to be working well, although the rollers are somehow penetrating through the laminate. Any idea as to why this is happening? I'm guessing it is either something to do with the contact settings or the step settings? I have had this issue before with Abaqus and I managed to get it to work it by turning on the "nlgeom" setting when creating a step. In Abaqus, "this setting controls the inclusion of non linear effects of large displacements and affects subsequent steps". Would there be something similar I would need to do in Mecway?

Victor · May 2016

Good to see it's just about right! NLGEOM is already turned with the "Nonlinear Static 3D" analysis type setting in Mecway. Contacts penetrating each other is also because the "Slope of pressure-overclosure curve K" on the contact is too low. It should be OK if you increase that by a factor of 10 or 100 or so. The higher it is, the more accurate the solution, but also the more chance of convergence failure.

max · May 2016

Hi Victor,

I have tried to increase my "slope of pressure-overclosure curve k" to 20000Gpa. I have also tried to use smaller element sizes for the laminate and a concentric cylinder for the top roller, but the contacts are still penetrating. Any other ideas as to how I can stop the contacts from penetrating completely and why this is happening?

Also I am fairly new to the concept of finite element analysis and Mecway. Can you please explain what the "slope of pressure-overclosure curve k" setting does to the model? And how it would affect the results of the analysis (eg are the results affected by the fact that the contacts are penetrating)?

Victor · May 2016

It probably needs to be increased further. I turned it up to 1,000,000 GPa/m. "slope of pressure-overclosure curve" is a kind of stiffness. When CCX detects a pair of faces have touched each other, it connects them with stiff springs to prevent them from penetrating. The stiffer these springs, the less the penetration distance (overclosure). If you plot contact pressure vs overclosure distance, the steeper the slope, the more "hard" the contact is. Ideally it should be infinite but it can't solve with too high a value.

I've simplified the model to speed it up and reduced the Young's modulus of the beam because it was about the same as the rollers (steel).

max · May 2016

Thanks Victor, that has been giving me much better results! I am currently trying switch to a force load instead of using the displacement as a load. For my analysis, I need to be able to vary the force instead of the displacement.

I have tried to change the faces in which the force is applied to from the side of the roller, to the faces on the bottom half of the roller with a force of z=-0.000001 N (Time, t = s). At the moment, it seems as though the roller is penetrating through the laminate, although I am not sure what it is showing. I have attached screenshots of the model undeformed and deformed (image with top roller missing).

Any pointers on how I can get this to work properly without the need of weak springs?

Sergio · May 2016

Maybe you can try appliyng a displacement and not a load. Then do a plot of reaction force vs displacement in Excel to know in which displacement you have reached the desired force.

max · May 2016

Thank you for your suggestion Sergio! I will give that a try for now. However, do you know the reason for not being able to simply just apply a force load in place of the displacement? Previously I have tried to apply forces ranging from -1E-11N to -1N but the analysis does not show any stresses. Which leaves me with the conclusion that I cannot just apply a force load onto the faces that I have previously done the displacement as load. Ultimately, I would like to be able to apply a force load instead of a displacement.

Sergio · May 2016

Maybe what is happening is that with such small forces the part still is penetrating so no reaction/stress.

I'm not sure, but what I can tell you from experience, is that is always easier (less time to solve, is a math thing) for the solver apply a displacement than a load, even more for contacts or nolineal material/big displacements.

What I have in my mind is that you could have the upper part completly separate from the bar, and you ask for apply -XX load. How the solver would know in what direction he must move the part (apply the load) if he has no force reaction? He could apply a small displacement and then check the reaction...no reaction, then what next? Increase the displacement, reverse the direction??? On the other side, if you ask for doing a displacement, you are telling not only the magnitud but also the direction, so there is no doubt for the solver in which direction he must move the part.

Guess that the low stiffness spring trick is to circumvalate this undetermination and give the solver a small reaction force to determine the direction of the loading, but to me, is more easy to apply directly a displacement than setup the springs, and you have the gain in time also during the runtime due to displacement and not load.

Victor · May 2016

I've managed to get force to solve OK, but as Sergio said, it's a lot harder than displacement. I did it by seeing what kinds of incorrect displacements the non-converged solutions gave and constraining them:

- Merged some nodes of the top roller with the beam at the point where you'd expect them to never move relative to each other.

- Added a constraint equation between two ends of the beam to prevent it from rotating about the Y axis. Any part of the beam can rotate, but the two symmetric sides now have to deform symmetrically. Caution: If you change the mesh in any way, you'll probably have to change the node numbers in this equation.

Sergio · May 2016

Víctor, for this kind of test normally I use a simmetry plane (in fact here we could use two planes), adding a displacement restraint (normal to the simmettry plane) to take in count this simmetry. This constraint also limit the rotation as we can see in the complete model, so there is no need to use equations. But could it be that this simmetry representation is too artificial?

Regards

Victor · May 2016

Oh yes, that would be more sensible. The equation is really ugly.

Jack · August 2016

Hi Victor,

I am new to Mecway and FEA and have been working on a similar project. Thanks for all the comments above and I learned a lot. But I still have to questions:
a) Looks like Laminate is only available to tick for Mechanical Tab of Material Properties of Plate/shell/membrane. Is there a way I can choose Laminate for hex20 elements so that I can input each layer's data like thickness, angle, etc.?
b) After I changed the coordinate system(z' = x, x' = y, y' = z) and moved the origin to the center of the laminate, the part deformed abnormally after solving. Can you explain why it didn't work?

Victor · August 2016

No, it doesn't allow laminate materials on solids. You'll have to do what you're doing, though you can make it a little easier by reusing the same material definition on several components, even if they're oriented differently. Material(1)-Material(4) are the same so you could delete 3 of them.

Everything looks OK so all I can think of is that the material properties might be incorrect. Where did you get them from? Some innocuous looking sets of orthotropic properties can represent exotic or impossible materials which lead to strange results or a failed solve. There are also two widely used definitions of orthotropic Poisson's ratio so make sure it's the same one Mecway uses - nu_xy/nu_yx = E_x/E_y, not nu_xy/nu_yx = E_y/E_x.

The deformed shape looks OK if you set all the Poisson's ratios to 0 or increase the shear modulus WU, but of course this isn't the same material anymore. Notice that your material has almost no shear stiffness even though it has a high bending stiffness due to the longitudinal Young's modulus. Do you expect it to deform mostly by shearing rather than bending?

Jack · August 2016

Hi Victor,

Thanks for quick reply. The same material definition are reserved for future work when each component is in different material.

I have tried to correct nu_WU values for the orthotropic properties and it works. Now the shape looks normal after solving. Cheers.

Jack · September 2016

Hi Victor,

I am trying to do the same analysis with shell element and displacement load. When displacement load is -2 mm and -3 mm, the results look normal. But when displacement load is -1 mm as per the attachment, penetration occurs. I have tried to adjust the k value (in range of 2000 to 1000000 GPa) of contacts, etc, but no luck. Can you have a look and advise?

Regards,

Jack

Mecway

Forum

Three Point Bending Constraints

Comments

Howdy, Stranger!