Connect two midplane surfaces(shell elements) with rigid beam elements to get reaction forces?

[autodesk428JLG]

Hi!

I would like to get some help with connecting two planes with each other with rigid elements for example so i can get reaction loads in that element that connects the two surfaces, someone know how to do this, please? The planes consists of shell elements. There must be a way to achieve that in Nastran In Cad im hoping. In Ansys i once was selecting certain nodes/elements and was connecting those to a singel point etc making those rigid, i was hoping that i somehow could do the same in nastran.

Best regards, Daniel

[vanderson.mapdata]

Hi Daniel

Take a look attached video creating rigid elements between two surfaces. You have to choose 2 faces and select Point at center to create independent node at center between them.

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[John_Holtz · Accepted solution]

Hi @autodesk428JLG 

Vanderson's reply about using the rigid connector is part of the answer to your question. However, it does not eliminate the problem with getting the force transmitted from one plate to the other. The force at the center of a rigid connector is zero because the forces on the top plate are equal and opposite to the forces on the bottom plate.

Whether you use a rigid connector, contact, or some other means, you need to sum the results from the nodes on the plate that are connected together. The Inventor interface does not have a convenient way to sum the results. You will need to inquire on the nodes individually and add them together, or use a third-party tool. (FNO Reader comes to mind. Version 1.58 is the current version.)

• For a rigid connector, you need to output the MPC result.
• Contact forces are output automatically, but the moment that is created by offset bonded contact is not output. (In other words, contact would only work when the gap is zero.)

Now that I look at a test model, one way to simplify it is to use two rigid connectors (one on the top, one on the bottom), and connect the two rigid connectors with a rigid spring. Since there is only one spring connecting the two faces (instead of N spokes in a rigid connector), their is only one element where you need to get the forces and moments.

John

[autodesk428JLG]

Hi John! Thank you very much! What values did you use for the spring? Because no matter how much stiffeness i use it falls thru alot, see pic below. Also i wonder, how do i extract loads from the spring?

[John_Holtz · Accepted solution]

Hi @autodesk428JLG 

You may not be entering the spring stiffness properly because the interface makes it more difficult than it should be.

1. Click the "Advanced Options" button to show all 6 directions for the spring stiffness.
2. Click the "Stiffness" checkbox so that you can enter the stiffness values.
3. Enter a stiffness for all 6 directions. By definition, spring stiffness = force/deflection. Based on an estimate of the force to be transmitted, and choosing a reasonable amount of compression (something larger than 0!), you can get a good estimate of the required stiffness.

If you have requested to output the force results ("Analysis > Edit > Output Controls > Force"), you can view the force in the spring using the result type of "Other > BUSH Force-Y". (I do not know why Nastran calls a spring "BUSH", but BUSH means spring. Maybe Google will come out with a translator for Nastran to English and other languages 🙂.)

Let us know if you have any other problems.

John

[autodesk428JLG]

Hi John!

Thanks alot!

Best regards, Daniel