Assign a moment release in a specific location of the beam modelled as a single part in ABAQUS

There's a *RELEASE keyword that can be used for this purpose. Its usage is described in the documentation chapter Constraints --> Element End Release.

Thank you so much, FEA way.

When I tried to implement the *Release feature, I received the error messages below.
----------------------------------------------------------------------------------------------------------------------------
When I tried this:
*RELEASE
4, S2, ALLM

Error message: Degree of freedom 3, 4, or 5 has been specified on the model. Beam elements in space should be used with the *release option
----------------------------------------------------------------------------------------------------------------------------
When I tried this:
*RELEASE
5, S1, ALLM

Error message: An invalid element end identifier 0 has been specified on the element

Degree of freedom 3, 4, or 5 has been specified on the model. Beam elements in space should be used with the *release option
----------------------------------------------------------------------------------------------------------------------------
I would be grateful if you could also help me solve this issue. Best regards,

For 2D beam elements you may have to use M1 instead of ALLM. Otherwise, you should use 3D beam elements.

I tried it with M1 but I received the same error message " An invalid element end identifier 0 has been specified on the element
Degree of freedom 3, 4, or 5 has been specified on the model. Beam elements in space should be used with the *release option"

I suppose it should be very simple and I try to do it as the documentation describes. Element 4's end node will be released by M1. So I try as follows
*RELEASE
4,S2,M1


Sometimes I also receive this message " An invalid element end identifier 0 has been specified on the element A release has been specified on element 0 but this element has not been defined
Analysis Input File Processor exited with an error." It is so strange either because all the elements with their id are available in the inp file as seen in the second pic above. After meshing the part, the elements are automatically defined with no effort. I don't know if I miss something.

Have you ever tried it with a simple beam model as I have? I would appreciate it if you have any samples, or if you can guide me on how to solve it.

Thanks

You can find some example files for this feature in the documentation chapter Verification --> Miscellaneous Options --> Miscellaneous modeling options --> Release rotational degrees of freedom.

Hi again.
I need further help to solve one more issue. I am using the 2d Beam (b21), and it works perfectly when I use *Release, no matter if I use either M1 or ALLM commands. I conducted eigenvalue analysis and static analysis, and both worked well. In the further step, I need to define a surface-to-surface contact in the interaction module(the top of the beam appearing as magenta will be the master surface, and a reference point will be a slave surface). When I only define the surface, run the same analyses as I did before, I receive the error message "Degree of freedom 3, 4, or 5 has been specified on the model. Beam elements in space should be used with the *release option" I think somehow Abaqus converts the model to a 3d problem when the surface interaction is added, and I think it contradicts the current model where the 2d beam is actually used. Or do you think there is another problem? Do you have any idea about what could be generating this error?

Best,

What did you do to get rid of this error before ? It can be important for the resolution of the current occurrence of the error.

When I got that error the first time, I was trying to apply moment releases in my actual model (complicated one) that has a surface-to-surface interaction, assigned point mass, rigid body etc. Then I decided to model the bridge from scratch without adding any of those features simply as seen in the picture. So My bridge model worked well with moment releases. Following this, I decided to add the features one by one and check the results in eigenvalue analysis. I have just figured out the problem causing that error message. When I add a point mass to the model in the interaction modul (btw surface interaction is not tested yet in static analysis), the analysis is just aborted before starting to run. It gives the same error message. Assigning point mass somehow converts the model to a 3d problem, and it contradicts the use of the *Release command applied in the 2d beam. I also tried to use the anisotropic mass option to define it, like in a specific direction M11, M22 etc. The problem still exists.

Edit: adding the surface to surface interaction also causes the same problem. If I decide ok Abaqus creates blood incompatibility somehow, lets change the 2d beam to 3d beam, then I will not be able to use the surface-to-surface contact because 3D beams cannot be used as the master surface in a surface-to-surface contact interaction. If I say Ok no problem, I can use general contact, then another issue will come out that surface pairs will not include reference points where they are used as slave nodes in my 2d beam for moving load/mass analysis.

I see. You could use a different approach to apply a moving load (like we discussed in your previous thread) but I see no reason why the current approach wouldn't work. Can you share the file ?

I have just shared it. Thank you!

Additionally, you can also check this attachment to see the same error message when the point mass is added to the beam in eigenvalue analysis.

There might be some bug with the *RELEASE option. You could try replacing it with equivalent MPC constraints (REVOLUTE + PIN). If it doesn't help, you may have to use 3D beams and change your approach to make use of contact.

Is it possible to assign both the revolute and Pin to the beam without using two separate parts and connector assignment like assigning moment *release? If two parts are necessary, I am concerned that the resulting two surfaces could create numerical problems (contact chatter problem creating acceleration peaks) as I have experienced before when a moving mass passed from one part to the other.

You need two separate nodes to apply those MPC constraints so two parts of the beam will be necessary.

Thank you for your support. I decided to use the 3D beam model because *release command works with no bug. In this 3D space, How would you simply model the half-car model as shown in the picture, providing a surface-to-surface interaction between the beam and contact point? That model works well in 2D. I don't know how to simulate this car model that will move over the 3D beam.

Something like a rigid beam perpendicular to that bridge model should work. General contact will handle this interaction.