Possible error in rigid body connector

[Anonymous]

Hello I was running some tests with a toy problem to get a grasp of what can be done with rigid body connectors. This is a simplified problem of some more complex models that I've done.

The idea is to calculate this model:

This can be done easily simulating every piece. In the model the white and green bodies can rotate around the X axis. While this can be done, in some cases there is no information of the supports other than they should be much stiffler than the beam. The results should look something like:

 I have tried to do the same using rigid body connectors. For that I set two small bodies that I restrict completely. I connected a corner of those bodies to the surfaces that were in contact with the supports. I have tried conecting just the appropiated degrees of freedom without success. Therefore, I tried to run the same model with all restrictions and all connected degrees of freedom. It seems to me that rotational degrees are not connected or I'm missing something.

Here it is the model and the results. In this case it shows a rigid body rotation around X:

[AndrewSears]

Hi Alberto,

Can you attach the model so we can see your setup?  I will start working on my version.

Thanks,

Andy 

[Anonymous]

Sure thing

[AndrewSears]

Alberto,

The rigid connectors are working as designed and the issue is with the solid elements.  Review the attached model for my changes in the set up.  This will give you some ideas on how to use rigid connectors to simplify the model.  What you will notice is that I created two rigid connectors per pivot point.  The anchor points of the rigid connectors should be defined along the axis of rotation you are expecting.  You were almost there because you added the small blocks to the model to help define that axis of rotation.  Also, be sure to notice what I selected as the Dependent Entities as you can only define a surface/edge/vertex one time for all instances of Rigid Body Connectors.  

The reason you are getting the twist is that the solid element nodes have an unrestricted rotational degree of freedom.  To see this in a simpler way, create a block and apply a fixed BC to a vertex.  what you will see is that the model is only partially fixed.  This should also answer why the DOF View, for your model, is showing as fully constrained when it really has the ability to rotate.  

Hope that helps and let me know if I need to expand on anything or you don't see what I did differently with the attached model.

Thanks,

Andy  

[Anonymous]

I understand the solution. However, doing it this way, the result would be a function of what points are chosen on that edge. For this toy problem it is not an issue, but it may be for larger ones.

I understand that a node in a solid does not have rotational degrees of freedom. It seem counter-intuitive to me to use a point in a solid to reference a rigid connection for that reason among others. Also, what is the point of setting up an interface to translate a degree of freedom than can not be set? Allow me to elaborate, unless I'm mistaken, as the system stands right now the settings for Rx, Ry, Rz are useless if we can not connect points were those dof can be set. What is the point of transferring those dof if they can not be set? I imagine that it is there for future update. If not please consider doing something in that line.

I have not used Nastran in quite some time, but the interface with other solvers is normally based on defining dof of a node (here it could be an isolated point or a geometry point) and connecting setting other nodes as dependent (or the other way around depending on the type of connection). Those are the famous RBE, I seem to remember that Nastran used that terminology too. In Fusion, to do this we need to create a body that we are not interested in calculating (therefore meshing it and the rest) just to set up a point.

I mean no disrespect, but this seems like a hack. I think the simulation part of Fusion is looking better each iteration and I feel it is becoming quite complete. However, in this case I have to say that it feels weird. I understand that you are probably trying to make it as easier to use. I think this time it is not the case. Just trying to be helpful.

[AndrewSears · Accepted solution]

Alberto,

---

@Anonymous wrote:

Also, what is the point of setting up an interface to translate a degree of freedom than can not be set?

---

The rigid body connector dialog was created to work with shells, which support nodal rotational DOF.  As you guessed, we ran out of time for the latest update to support shells in Fusion and did not change the UI.  We agree this is confusing and we are discussing an option to hide Rx, Ry, and Rz until we get shell elements into the software.  It does currently seem like a hack to add the extra part and we are working on solving that problem also.  

Please do not ever think you are being disrespectful.  We have a great team making the simulation side of Fusion awesome, but we sometimes overlook items or in this case, set lower priorities on other items to focus on features we think you would find more important.  By you pointing this out, it lets us know where to focus for future updates and started a discussion internally on how to solve this.  We are going to try to get these hidden for the January update and change the behavior of the dialog so that when users apply rigid body connectors to solids, they will not see Rx, Ry, and Rz.  Once we add shells and line elements to Fusion the rigid body dialog will adjust and show what DOF's work with the element types defined.

My suggestion to you is to keep the comments coming and help us make it better!

Cheers,

Andy 

[David-Truyens]

Hi @Anonymous, @AndrewSears,

I would like to popup this thread. The rigid connector is very important to correctly define the DOF's in an analysis. The most common mistake I've seen made in all my years of FEA teaching is the pin constraint. If you do it using a pin you'll get something like this:

Instead a real pin would look something like this:

The usual way to do that would be using a rigid connector and a constraint to the central node of the connector. 

Now you have to do very crazy stuff (create a rigid connector to a vertex of a solid???) to try to get something done, but in the end it doesn't even do the job. 

Even better would be a button to create a real pin constraint in one go (and do the trick with the rigid body in the background).

Regards,

David