How to connect a mid-surfaced shell element to a solid element

[mcook21VD9DL]

Hi guys,

As titled, I believe the solution for me lies in rigid body connectors however I don't think using points is sufficient (that or mid-surface everything). I have a large model in which has multiple thin bodies of long lengths, and I would like to maintain some solid surfaces such as end plates as it is a structure. It seems nastran is in agreement as it leaves them as solids when I run 'find thin bodies'. If I mesh the whole assembly as a solid at a relatively ok mesh, I get 5.5 million nodes. What I have done so far is I have taken one of the main assembly sub-assemblies, and turned it into a simplified model with solid bodies in tact, this seemingly decreased the time to create mid-surfaces. Now, when attempting to run the test on this sub-assembly, it gives me a 5004 error which means I am not getting that solid to shell element connection I need.

This is Nastran 2022

It would be fantastic if someone could help me out with some insight into how to best go about solving this.

Cheers

Sub assembly is as below

[John_Holtz]

Hi @mcook21VD9DL 

See How to set up automated contact with shell elements in Nastran | Inventor Nastran | Autodesk Knowled....

John

[matthew.cookXCL5S]

Hi John,

I am an avid user of solver contacts, but it still produces singularity errors when attempting to contact the shell to a solid. I believe it is because regardless of offset bonded or bonded (I always use offset bonded), the perpendicular joining of a vertical shell to a horizontal solid still creates a hinged/swing joint. In my case, I am simulating a large vertical column on a base plate, in which the column is a mid-surfaced shell element and the base plate is a solid. I managed to get it to run when I set everything (inclusive of gussets and base plates) to shells but I really would like to know how to run with shells and solids without needing to customise my model too much to suit FEA.

Please let me know if my understanding of the contacts are incorrect,

Thanks John!

[John_Holtz]

Hi,

There is something wrong. Offset bonded contact does create a moment connection, not a hinge connection. So if a flat plate makes a theoretical line contact with the solid, such as the following, the model is statically stable. (I had to increase the contact stiffness to reduce the rotation angle from 0.19 to 0.134 radians. The theoretical rotation at the free end is 0.129 radians.) The reaction force and reaction moment in my constraints match the expected load and moment, so there is no artificial stiffness or constraint occurring in the solution of this model.

The maximum activation should follow these criteria:

• Larger than 0. (Actually, I'm not sure if 0 means 0 or it means to use some default. Better to be safe than sorry.)
• Larger than the gap between the pieces. In your case, larger than the gap (if any) between the bottom edge of the shell column and the face of the solid base plate. (For another example, if there is a gap between the web and flange of a wide-flange beam, the max activation distance needs to larger than this.)
• Smaller than 1/2 the mesh size (if using parabolic elements) or smaller than the mesh size (if using linear elements). You so not want the mesh size to be so large that it creates contact between the "next node on the shell" to the base plate.

If the E5004 persists, you could run the analysis as a Normal Modes analysis. The part that has a displacement in mode 1 (or any mode with a frequency near 0) is the piece that is unstable.

If that doesn't solve it, feel free to zip your subassembly and the part files for the subassembly and attach it to the forum.

John

[matthew.cookXCL5S]

Hi John,

Thanks for that - I'll give it another go. Can you please tell me how am I to know when to increase the stiffness factor (or decrease) ?

[matthew.cookXCL5S]

Hi John,

Just wanted to touch on something else. The shells certainly contain less nodes, but when I complete the test and go to view the results, it's taking me 30 minutes to wait ( or more) for the results to show up, when the test itself takes 2 minutes to run. I have a considerable PC and it's not working very hard at all. Is there a way to fix this?

[hbhu]

Hi,  matthew.cookXCL5S.
          In order to turn our engineering analysis platform to Inventor Nastran, our team members have done a lot of research in recent years. The following experience with mixed element idealization hope to give you some help:
1. When the structure is simple, it should be manually create all mid-surface shell elements and solid elements, and then manually perform all offset bonding to complete the idealization;
2. When the structure is complex, a surface model and a solid model should be created in the Inventor environment, and imported into Inventor Nastran. , using the continuous mesh method to idealize the shell element, and then manually establish the offset bonding between the solid element and the shell element to complete all the idealization;
3. The conclusion is that, when the current Inventor Nastran deals with practical engineering problems, the hybrid element idealization methods are impractical. For engineering structures with a large number of thin shell structures, the solid part should be simplified out, and all shell elements are used for idealization.