December 6, 2019 at 8:36 ammehdimechanicSubscriber
I have an assembly of parts which have some forces and supports on it. It is simulated to give me the results. The results are deformed geometry and some stresses which i export to text files to use in external model as initial stresses. I need to assemble the deformed geometry to another geometries ( in a CAD software) and after that, map the stresses to my first deformed geometry. How can i do these steps? Can it be done?
1. get deformed geometry of an assembly.(The stl file is attached).
2. map initial stresses of a deformed geometry to another assembly containing this deformed geometry.
December 6, 2019 at 11:59 ampeteroznewmanSubscriber
You can't attach .stl files directly. Put it in a .zip file, you can attach that.
There is an old thread on how to export Deformed geometry to bring into a CAD system. The tail end of the thread has the new method introduced since the thread was originally published.
It sounds like you need the deformed geometry to design another part in the assembly. Once you do that, you will have an assembly that has the underformed first part, the deformed first part and the rest of the assembly. Delete the deformed first part and bring the assembly into Static Structural. Support and load the first part to create the deformation in Step 1, then in Step 2, you can use the parts in the rest of the assembly. This will avoid the need to map stresses.
It might be the case where you use bonded contact to connect the deformed part to the rest of the assembly. You can define that contact in the model, but have it be Dead during step 1, then make it Alive in step 2 so the contact bonds "in place" on the deformed part.
December 6, 2019 at 12:51 pmmehdimechanicSubscriber
The file is uploaded. Now i have two main questions. First i want to know can it be done using the deformed geometry and mapped stresses or NOT.
My second question is how can make contact alive or dead in steps? Thanks for the help.
December 6, 2019 at 3:07 pmpeteroznewmanSubscriber
Yes, the stress can be exported and imported, but I don't use that functionality.
Here is how you make contact become dead and alive in different load steps.
December 6, 2019 at 3:20 pmmehdimechanicSubscriber
Which Ansys versions supports Contact Step Control?
December 6, 2019 at 3:23 pmpeteroznewmanSubscriber
I don't know when it was first added as a Workbench button, probably one of the 2019 versions.
The same functionality exists in older versions, but you have to use Command objects and write a line or two of APDL code.
December 6, 2019 at 3:43 pm
December 6, 2019 at 3:50 pmmehdimechanicSubscriber
actually all of the parts together will import to another geometry for assembly. there is three of geometries like this, i think i should import the deformed geometry. the main problem is the springs and the elastomer cup.
December 6, 2019 at 7:41 pmpeteroznewmanSubscriber
The springs are easy. Do not use solid model geometry. Insert a spring element and enter the spring rate, free length and preload data.
You don't want to mesh the elastomer cup in its deformed state. You will get highly faceted surfaces that will make a very heavy mesh. The undeformed geometry has very clean faces. You want to deform the few elements it took to mesh the clean geometry.
December 7, 2019 at 1:45 ammehdimechanicSubscriber
with the new method introduced, it is almost ok except when i export the geometry in design modeler as stp file, it exports faulty geometry.
could please help me on this? in design modeler i can not creates solids. But there is a good geometry with 8 distinct parts in the design modeler. mechanical model greatly do it. i can not just export a good geometry. could please help me on this?
December 7, 2019 at 4:02 ampeteroznewmanSubscriber
When I said you don't want to go down the export deformed geometry path, I implied that I don't want to go down that path either. I am curious to see how the deformed geometry exported using the "new method". Please attach an archive file so I can see how faulty the geometry is. I'm not going to fix it, I just want to see what kind of a mess was made of the geometry.
Exporting STL files of the deformed geometry is very easy and useful for visualization only, because it can be put in a CAD system to see other parts around the deformed part, but the STL facet body is not geometry and trying to convert it to geometry is to be avoided at all costs.
I suggested above that you do a multistep analysis.
A better idea is to replace the elastomer cup with a nonlinear spring. Use a model where there are no other springs except the cup. Move the shaft with a Displacement load. Copy the reaction force data and the displacement data to a spreadsheet so you have the nonlinear force-displacement data to paste into a nonlinear spring element (COMBIN39) in the larger model where you want three of these working with other parts.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.