Transforming Axisymmetric Results To 3D Model

[mhajinaw]

Dear Members,

I have an axisymmteric model that undergoes forming process. In this axisymmetric model, I have a rigid body and a deformable body. I can run the simulation and obtain the results.

The next thing that I want to do is to use the results from the axisymmetric model and transform it to 3D. This require some transformations. I have already looked at the keyword *Symmetric Model Generation and *SYMMETRIC RESULTS TRANSFER. The problem is my current axisymmetric model contains quadratic element (CAX8R) for the deformable body and linear element for the rigid body (RAX2). The symmetric keywords do not work with both elements (linear and quadratic at the same time). I have also tried changing the CAX8R to CAX4R and it works. However, this forming process involve significant bending and I prefer to use quadratic elements since it gives better approximations. This means I am still stuck.

So, do you have any suggestions to resolve this problem?

I know that it might be possible to create a script to transform the nodes from 2D (CAX8R) to 3D (C3D20R) but I require some guidance and example.

Cheers.

 

[mhajinaw]

I have figured out how to do this. In case someone else wants to know how, here's how I do it:

1. Run the initial forming process.
2. Create a new model by importing only the deformable part from the ODB of previous completed simulation. Right-click on part --> import --> select odb file --> select the part and the final deformed shape
Also remember to also include predefined fields (e.g stress components from previous simulations). From the previous simulation, you can create XY report of stress components and include that in your new model. This step can be a bit tricky and you probably needs to play with the input file. What I do is to request the stress components from the centroid instead of the integration points. And for each element I also create a set. This way it'll be easier to assign the stress components of each element by defining it through set. There's also another options to define the stress states from ODB output file. But I'm not familiar with this option.
3. Just run a simple static case without any loading. The idea here is to assigned the stress components to the deformed part. It is also a good idea to make sure that you also deactivate the option to use parts and assemblies in input files. Model --> Edit Attributes --> Unclick the option to use parts and assemblies in input files
4. Once you've completed the job, just check the results (deformed shape and stress states). If everything seems good, you can start to transform the results into 3D using *Symmetric Model Generation and *Symmetric Result Transfer.

Let me know if there's another method of doing this.

Cheers and success!