Beam model, error changing mesh size

[autodesk428JLG]

Hello!

I need some help cause im out of options here!

1) Im getting a error while changing the mesh size, from let say 50 to 10 mm. For 50 mm and 100 mm it works for a modal and a static analyse.

Is this an indication of what? Arent lines connected? I used split like everywhere i can find a possible error. And investigating a modal and a static anaylses, i cant find any loose ends.

2) I also getting an error when trying to change idealization from current to rigid for some reason. First i thought it was due to having different centroids defined for the joining beams, but it wasnt. See picture and attatched model.

Thanks in advance, best regards,

Daniel

[John_Holtz · Accepted solution]

Hi Daniel.

In the future, please list the errors that you are getting. Some readers do not have Inventor 2023 and cannot view your model, but all users have the ability to comment on what an E5000 error is, for example, since users can encounter that error with all versions of Inventor Nastran.

1) Your model gives an E5000 error when the mesh is changed from 50 mm to 10 mm. Technically, the error indicates the stiffness matrix cannot be solved. Something leads to a division by 0 after all the multiplication and subtraction is performed. Practically, it means

• A piece of the model is not statically stable. This creates a value of 0 in the stiffness matrix. (That does not appear to be the issue in your model.)
• The material properties are wrong. (The "RIGID" material in your model is the problem. A modulus of elasticity of 1.9E50 MPa is ridiculous compared to the other modulus of 2E5 MPa. Typically a range of 1000 or 10000 is what can be handled, so try E=1.9E9.)
• The mesh is distorted which "corrupts" the stiffness matrix and produces the same type of problem.

2) I am not clear what you mean by this (changing "current to rigid"). If you are referring to the rigid material property of E=1.93E50, the solution is to not do that.

Let us know if you have any other questions.

John

[autodesk428JLG]

Hi John! 

Thanks for your help as usual! And i will try to remember the error code to next time.

Yes, i found that out too just now, but if im allowed to geek out a bit here cause im interested: So, if im using an unreasonable high stiffness, the total strain energy will be so off when compared to the total applied work to the model and that are making the stiffness matrix zero? Is that correct theory understanding?

Best regards,

Daniel