January 3, 2023 at 8:33 ampcSubscriber
I am doing hydrodynamic analysis in Ansys Aqwa. In a semisubmersible sturcture, I have to use surface bodies for cylindrical columns and line bodies for cross braces so that a hybrid approach using potential flow and morison equation will be used in analysis.
I created the said braces using line from sketch option and later applied a circular cross section to get the cross braces. Now, my question is about the area where the brace and cylinder meet.As of now, they are different bodies in a part. Should I perform the analysis as it is or should I do some joint operations or share topology operations for cylindrical surface body and cross brace line body.
January 4, 2023 at 6:47 pmmjmiddleAnsys Employee
This is a common question customers often ask. How do I connect beams and shells? And what is the best method? There are a couple methods and I can’t asy that either is best. You need to make a preference choice. There are pros and cons to each method.
Method 1. Connect with shared topology in CAD system
Shells and beams are meshed with 6 DOD elements by default. Solids use 3 DOF. So you cannot easily connect solids and shells/beams by mesh nodes. But shells and beams should be able to connect. However, DM doesn’t do this when you “Form New Part.” If you open the model in SpaceClaim, you can connect the surface body and beam with shared topology.
pro: Simpler model setup in Mechanical. No need to joints or contacts. Faster running analysis because of this
con: Extra task connecting bodies in CAD modeler (SpaceClaim) which could cuase extra user time if beams shells have gaps/overlaps. A one-node connection of beam end to shell may not be rigid enouh to represent a beam whose entire cross section is attached (welded) to the surface.
method 2: Connect with contacts or joints in Mechanical
A mentioned above, for a DM model, you must connect beams to shells in Mechanical since only SpaceClaim will do it in the CAD system. If you use a contact, set formulation to MPC. A joint should be set to fixed joint in most cases. Select the beam end vertex for contact/reference side. Select face for target/mobile side. In either case set a pinball radius on the side with the face selection. This connects constraints only within that pinball radius (red lines below):
Thse constraints stiffen the model a bit in this locationm but may be more approiate to represent a beam welded at the cross section perimeter in this case:
Scaled result on the cylindrical surface:
Here is the same model setup using the share topology in SpaceClaim that connects only the one node at the beam end to one node on the surface:
This may be appropriate in some models, but I don’t think it’s as good for this one.
Note that you can project the beam end vertex to the surface to embed a point into the surface in DM or SpaceClaim. Then you can create the joint as vertex-to-vertex selection instead of vertex-to-surface with pinball. This will have a similar result to the one-node connection done in SpaceClaim with share topology. You won’t be able to do a vertex-to-vertex selection for a contact.
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- How to work with STL file?
- Using Symmetry in DesignModeler and Expanding the Results
- Rotate tool in ANSYS Design Modeler
- drawing a geometry by importing a table of points
- section plane
- material properties
- ANSYS FLUENT – Operation would result in non manifold bodies
- Geometry scaling
- Parameters not imported into Workbench 18.2 from Solidworks/Inventor
- Convert Surface body to solid
© 2023 Copyright ANSYS, Inc. All rights reserved.