exporting model from WB to ansys classic

[unaisarriko]

Hi All,

I am working on a static simulation of a complex machine tool where I am using ANSYS Workbench 11.0. After importing the assembly from Solid Edge to WB and defining the basic contacts and supports, I need to export the model to the ansys classic environment. I have tried to load Ansys from WB, and it seems to export the model correctly. After saving it as .db I close Ansys workbench and try to load the .db archive from the ansys product launcher, but there is no information in it: no elements, no real constant... it’s empty!
Is there any suitable way to export all the info that has been defined in Ansys workbench to Ansys classic environment.

Any help is much appreciated

Thanks in advance

 

[kemosabee]

There's 2 ways that I use. If I plan to use classic environment to solve/make changes I do the following:
go into simulation, make sure you have a type of analysis setup, create a dumming analysis condition if need be. Then in the tree, select the solution, then goto to Tools->Write Ansys Input File from the Dropdown menu at the top. If it's greyed out, it means you don't have the solution selected.

The other, which is what I normally use. Solve you analysis like you would normally in workbench simulation, then goto the project page tab, click on that analysis you just solved, and then click on the the link called "Open containing folder".
This is the analysis folder with the results, the database is contained in the ds.dat file (ansys classic import using file->read input from). Just make sure you read the input in using a preppost license, or else it'll run the full analysis again.
I use this method to extract data, like path operations all the time.

 

[timkwan]

Note that the Workbench Simulation's DSDB file is not the same as the classic GUI's DB file.

Also note that only the FE model (nodes and elements) is transfered to the classic GUI. The solid model (volumes, areas, lines and keypoints) do not get transferred from Workbench to classic GUI.

 

[bagarbilla]

@unaisarriko First thing i note that is you wrote that, you used product launcher to load file, i don't think ansys load file from product launcher it only ask for name. you have to resume db to read the file.

i like the classical environment so i export geometry to ansys classic using the *.anf (ansys neutral file) and then play with it in ansys classic.