Abaqus Assembly

[keulehans]

Hi guys,

I am quite new to Abaqus, so this should be an easy one I hope.
I have two different finished models in Abaqus. The one is an airfoil (without any analyzing) and the other one is a thermally cured fiber reinforced rectangular plate. I performed one analyze step on this plate, in which the plate is cooled down, which leads to residual stresses and Deformation of the plate. The model of the plate works well as the plate behaves as expected.
My Problem now is, that I dont know how I can put together the analyzed (deformed and with residual stresses) rectangular plate and the unanalyzed airfoil. My best guess yet was to import the deformed part from the odb file, but then I only get the deformed mesh without any residual stresses (Composite layup and material is also gone). Also I have to put further analyzing steps onto the model in which both parts are assembled.

Can anyone tell me how I can put together the unanalyzed airfoil and the analyzed rectangular plate, without losing the residual stresses and deformation of the plate?

Thanks very much everyone!

 

[Dave442]

Look up *IMPORT in the keyword reference manual. Its used to define the time in a previous analysis at which the node and element information is imported. There is an optional parameter STATE=YES that allows you to import the material state of the elements at a specific step, interval, increment, or iteration.

 

[keulehans]

Hey Dave,

thanks for the answer. I was not able to do it in the input file, because my syntax was always wrnog. However *IMPORT in the Abaqus documentation showed my eventualy the way how to do it in the CAE. In the analyzed modell I went to Step modul->Output->Restart Requests. There I put a 1 as frequency at all steps and then submitted the job for that model. I then went to the other model, into which I wanted to import the deformed and analyzed part. Here I imported the analyzed geometry with all its informations by first importing a part and chose to import the deformed geometry after the last increment of the last step. That will however give you only the deformed mesh. To add all the information from the analyzed part I then had to make a instance of the deformed part (name the instance exactly as the instance from the other model and if you want to translate or rotate the geometry DO IT NOW). Then I had to go to Load modul->Predefined Fields->Create. There I took Initial as step, Category Other, Type initial state. There I had to fill in the job name of the analyzed part and left step and increment as last.
Hope this can help other people and my future me if I forget the procedure again.