Learning Forum

[Arzzack]

Hello everyone !

 

I am currently trying to simulate the following sequence:

- Pressurization of a thin Aluminium pressure vessel to strain harden the material (plastic deformation)

- Wrapping with CFRP on top of the aluminium skin

- Simulation of the finalized tank under pressure and thermal load

 

I know how to do every sub-tasks separated but I don't know how to use the deformed shape as a surface for the composite modeller (I end up with a dead surface without edges). I must also simulate the final tank with the remaining plastic strain in the Aluminium to account for the hardening.

I included a screenshot of my workbench

Can someone help me on this ?

 

Thanks in advance !

[Wenlong]

Hi Arzzack,

A very interesting topic. I am testing a small model and will get back to you soon.

Regards,

Wenlong

 

[Wenlong]

 

Hi Arzzack,

Here is what I came up:

1. To transfer you deformed shape to ACP(Pre), you can simply link the "solution" of System A to "Model" of ACP(Pre).

2. After you generate you composite in ACP(Pre), you can create another Static Structural, then link your Setup of ACP(Pre) and Setup of System A to the "model" of the new Static Structural Analysis. If you open it, you will see two parts: one is the metal, one is the composite (see below). You may want to adjust the offset of the metal sheet so that these two layers don't overlap each other. 

3. To transfer the equivalent plastic strain, there are several steps:

3.1 In System A (the first static structural analysis), plot the equivalent plastic strain, then right click on it --> Export --> to Txt file. 

3.2 In the same environment, insert a user-defined output, name is as locx, and type the expression as "loc_defx", it will plot the deformed x-coordinate. Do the same export again. 

3.3 Repeat until you export all the three deformed coordinates.

3.4 Open these txt files you just generated, edit them so you have the following format:

3.6 In Ansys Workbench, insert an "external data" component. Then double click on it, and choose the txt file you just modified. (You may need to manually modify the node number because after you generated composite, the node number may be shifted, which is my case)

3.7 Modify the settings so Workbench recognize the meaning of each column, as shown below:

3.8 Link the External data to the setup of system C (Static Structural), open it. 

3.9 Right-click on the imported data, then insert an initial strain, as shown below. You can see the Eqv plastic strain is added.

4. The Eqv plastic strain is just an example, you can add other variables as you need.

Hope this helps. If you want to see the full resolution image, please see the following link.

Regards,

Wenlong

 

---

Useful Links

---

• How to show full resolution image

 

 

 

[Arzzack]

Wow that's what I called a detailed answer, thanks a lot !

 

I implemented it and it mostly worked very well. However I had problems when applying the pressure during the last analysis with the composite added: