Go to tools>options>export>include nodal coordinates. Change the select option to select mesh. then select nodes/elements of interest. Make named selection of selected nodes/elements of your interest. Right click named selection to export the entity. Excel file will open with node no and their global coordinates. For elements only element no, type and connected nodes will be given.

Note-Selecting nodes and elements will take time if your model has high no of nodes and elements. Selecting and exporting interested nodes and elements is rather easy.

Hi Nikhil Patil,

Thank you very much for this. I have tried to export the nodal location and nodal connectivity of the undeformed model. It's success as expected. I wonder if this method works in case of the deformed model. I think that to export the nodal location of deformed model, I should export the UVECTORS by creating a "user defined result" using WORKSHEET. Then manually, I can derived the deformed nodal location just by summing the original location and UVECTORS.

Yes. UVECTOS will give you the component wise displacement value that you can sum up with original coordinate to get final node location. Also look in to the user defined results LOC_DEFX, LOC_DEFY and LOC_DEFZ for another way to export deformed nodal coordinates for each X,Y and Z component separately.

Alternate way is to insert command block as given in the enclosed link. You can follow the steps given in the enclosed link. But note- instead of converting CDB file to geometry, you can use the deformed mesh CDB file to extract the nodal coordinates by using mechanical model object or using CDB in APDL and issuing NLIST command.

The procedure given in the link is for use of deformed geometry for further analysis.

https://caeai.com/resources/generating-geometry-deformed-shape-using-ansys-workbench-v12

Yes, I'm also curious why ANSYS WORKBENCH does not support exporting LOC_DEFVECTORS. It will be more convenient in exporting the location of deformed model.

The article is very interesting. Although I don't know the meaning of these command anymore, I try the COMMAND (APDL) in Ansys Workbench and It works. However these command only export the mesh of un-deformed model. Is it right? Do you know the code to export those of deformed model.

No. This code primarily used to export deformed model. I should have told you to omit UPCOORD command to use it to get node coordinates of non-deformed mesh. UPCOORD command actually updates the coordinates of the non-deformed nodes to that of deformed nodes and WRITE command writes the CDB file with updated mesh. You should use this command block in solution after solution is achieved. If you use it in the setup, the coordinates will not update as model is not deformed. 

I dont know why it doesn't work. In your link above, it is said that the method may not work for complex geometry. I think this is the case.

OK. I will check it more later. Now I will use the manual method to find the deformed nodal locations.

Thank you very much. You have saved much time and effort for me.