Learning Forum

[fniessen]

Hi, 

I would like some help with importing data from an Abaqus *.inp file through the external model in ANSYS Workbench into ANSYS Mechanical. My aim is to read in nodes and elements with local coordinate systems associated with certain groups of elements to implement anisotropic materials behavior.
I succeeded in importing nodes and elements with named selections of element groups. I also managed to import local coordinate systems that I need for each named selection to define anisotropic material properties.

Here is one of the local imported coordinate systems:

This is one of the named selections, that groups a number of elements:

 

I would like to be able to assign an anisotropic material to the entire plate (that's easy) and then use local coordinate systems to define the orientation of element groups. This does not seem to be possible.

 

In my Abaqus input file I defined the coordinate systems with the orientation command:

 

*ORIENTATION, NAME=CS-56, DEFINITION=COORDINATE

0.,0.89872,-0.39135,0.19785,0.42697,0.67810,-0.59823,0.09996,

0.62212,0.77652

 

The element sets were then associated to the coordinate system as follows:

*Elset, elset=Grain-56, ORIENTATION=CS-56, MATERIAL=BetaTi_r, RESPONSE=TRACTION SEPARATION

8789, 8790, 8934, 8935, 8936, 9079, 9080, 9081, 9082

9226, 9227, 9228, 9229, 9230, 9371, 9372, 9373, 9374

9375, 9376, 9377, 9378, 9379, 9380, 9381, 9382, 9383

I was unfortunately not successful in importing local coordinate systems that are directly associated to the named selections in ANSYS Mechanical.

But even worse, the named selections in ANSYS Mechanical do not seem to be useful either. If I, for example, want to do a material assignment to a named selection, the dropdown window is empty even though I have all the named selections from the element sets. 

Does anybody have a clue on what to do about this situation? Any way forward or alternative approach would be great. I am currently generating the *.inp file in MATLAB and could formulate it differently if there was any merit to it.

Thanks and best wishes
Frank

[Aniket]

Hi I am not much of expert in the area, but how much work will it require to redefine the element coordinate system in Mechanical using element orientation in Mechanical?

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v195/wb_sim/ds_element_orientation_o_r.html

-Aniket

Guidelines on the Student Community

How to access ANSYS help links

[fniessen]

 Hi Aniket, 

thank you for the suggestion. Against all my expectations that seems to work. However, I would need to define the element orientations manually for my 83 areas. 
Is there a way of automatizing this?

Also, there seems to be a way of importing element orientations from an ANSYS input file directly.
https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v191/wb_sim/ds_import_ext_model_eo_o_r.html
I wonder why my files only get imported as coordinate systems and not element coordinate systems?

[Aniket]

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/wb_sim/ds_external_model_import.html

The link above seems to mention the following limitations does your model bumping into one of those?

The link you have mentioned seems to state that element orientations are supported, but doesn't strike anything from your description that might be causing this.

-Aniket

Guidelines on the Student Community

How to access ANSYS help links

[fniessen]

Hi Aniket,

I do define a part, but only one, which should be fine? All my data is within the *Part *End Part region. I do not use the *NGEN keyword. This is the file in case you want to have a look at it.

https://www.dropbox.com/s/qd5sd9ou3ub5rt8/ebsd.inp?dl=0 

[fniessen]

I finally figured out how to import Element Sets with a local coordinate system with an Abaqus *.inp file:

Define the local coordinate system:

 

*ORIENTATION, NAME=CS-50, SYSTEM=RECTANGULAR, DEFINITION=COORDINATES

0.,-0.02357,0.85587,-0.51665,-0.98928,0.05454,0.13547,0.14412,

0.51431,0.84541

 

Define the element set:

*ELSET=Grain-50

2698, 2699, 2769, 2770, 2771, 2772, 2773, 2774, 2841

2842, 2843, 2844, 2845, 2846, 2847, 2914, 2915, 2916

2917, 2918, 2919, 2987, 2988, 2989, 2990, 2991, 2992

3060, 3061, 3062, 

 

Define a shell section, linking the element set to the local coordinate system:

*SHELL SECTION, ELSET=Grain-50, ORIENTATION=CS-50

Finally, the element orientations can be imported with the external model and will show up in the Geometry tree:

 

Thank you all for your help.

 

[fniessen]

There is one issue remaining. I do not seem to be able to import anything other than isotropic elastic material properties. I summed up the problem in this example *.inp file that can be imported with the External Model and connected to the Engineering Data block:

**PARTS

**

*Part, name=SAMPLE

 

*MATERIAL, NAME=TestMat_Iso

*DENSITY

4506, 20

*ELASTIC, TYPE = ISOTROPIC

2.8000e+11, 0.3, 20

 

*MATERIAL, NAME=TestMat_Ortho

*DENSITY

4506, 20

*ELASTIC, TYPE = ORTHOTROPIC

2.8000e+11, 1.5000e+11, 2.8000e+11, 1.5000e+11, 1.5000e+11, 2.8000e+11, 1.2500e+11, 1.2500e+11,

1.2500e+11, 20

 

*MATERIAL, NAME=TestMat_Aniso

*DENSITY

4506, 20

*ELASTIC, TYPE = ANISOTROPIC

2.8000e+11, 1.5000e+11, 2.8000e+11, 1.5000e+11, 1.5000e+11, 2.8000e+11, 0.0000e+00, 0.0000e+00,

0.0000e+00, 1.2500e+11, 0.0000e+00, 0.0000e+00, 0.0000e+00, 0.0000e+00, 1.2500e+11, 0.0000e+00,

0.0000e+00, 0.0000e+00, 0.0000e+00, 0.0000e+00, 1.2500e+11, 20

 

*End Parts

All three materials are imported with the correct name and Density property. However, only the isotropic elastic data is imported, none of the orthotropic or anisotropic data.

I followed the instructions to define the properties in the *.inp file from here
https://classes.engineering.wustl.edu/2009/spring/mase5513/abaqus/docs/v6.6/books/usb/default.htm?startat=pt05ch17s02abm02.html

and here
http://dsk.ippt.pan.pl/docs/abaqus/v6.13/books/key/default.htm?startat=ch05abk03.html#usb-kws-melastic

and here it confirms that ANSYS should be able to read in these properties
https://support.ansys.com/staticassets/ANSYS/Initial%20Content%20Entry/General%20Articles%20-%20Products/ICEM%20CFD%20Interfaces/abaqus2icem.htm

Could anybody point me to the issue I am facing? Thank you so much,

Best wishes
Frank