4 Replies Latest reply on Aug 15, 2013 7:44 AM by Yordan Venev

    Inability to set SECTION=ELBOW for elbow elements in Abaqus CAE 6.11-3

    Yordan Venev

      Hello everybody,

       

      That is probably not the most proper place to ask for assistance for Abaqus (I appologise for that) but I hope that the people here have experience with it as well.

       

      I would like to model a simple pipe structure with any of the elbow elements available in Abaqus, for instance the beam element ELBOW31. In the Mesh module I successfully assign ELBOW31 as Element Type but it is also needed to assign an elbow section in the Property module. The problem is that when I create a Beam section in the list with the profiles I do not see "Elbow". In the Abaqus manual for Beam Section it says "Set SECTION=ELBOW for elbow elements, which are available only in Abaqus/Standard." (http://mse-license1.mse.drexel.edu:2080/v6.7/books/key/default.htm?startat=ch02abk06.html#usb-kws-mbeamsection). In my version Abaqus/ CAE 6.11-3, Abaqus/Standard is the product employed in the simulation process so I don't understand why I can't see Elbow as an available cross section profile for beam elements?

       

      Can you give me a clue how could I employ the elbow elements in my analysis?

       

      Thank you for the help in advance!

       

      Regards,

      Yordan Venev

        • Re: Inability to set SECTION=ELBOW for elbow elements in Abaqus CAE 6.11-3
          Jerry Steiger

          Yordan,

           

          You will probably have a better chance of getting an answer if you move this to the SolidWorks Simulation/Simulation forum, using the button in the Actions box to the upper right. Some of the folks there may have Abaqus experience.

           

          Jerry S.

          • Re: Inability to set SECTION=ELBOW for elbow elements in Abaqus CAE 6.11-3
            Jared Conway

            probably best to take this to the 3ds swym forums

            • Re: Inability to set SECTION=ELBOW for elbow elements in Abaqus CAE 6.11-3
              Yordan Venev

              Hello again,

               

              I got to know the solution for the problem I had.

               

              An Elbow section cannot be specified in /CAE. That’s why do so: specify the beam as a pipe-section in /CAE. Then you have to write out the inp-file from /CAE using:

              Job -> Write input

              Then you get a inp-file that you can edit like:

              ** Two, or more, asterix give a comment line.

              ***Beam Section, elset=_PickedSet2, material=steel, temperature=GRADIENTS, section=PIPE

              *Beam Section, elset=_PickedSet2, material=steel, temperature=GRADIENTS, section=elbow

              Data line 1

              Data line 2

              Where according to the Abaqus 6.11 keyword manual *Beam section:

              Data lines for ELBOW sections:

              First line:

              1. Outside radius of the pipe, r.

              2. Pipe wall thickness, t.

              3. Elbow torus radius, R, measured to the pipe axis. For a straight pipe, set .

              This value is not written for the Pipe-section so it have to be added.

              Second line:

              Enter the coordinates of the point of intersection of the tangents to the straight pipe segments

              adjoining the elbow, or, if this section is associated with straight pipes, the coordinates of a

              point off the pipe axis. The second cross-sectional axis will lie in the plane thus defined, with

              its positive direction pointing toward this off-axis point.

              1. First coordinate of the point.

              2. Second coordinate of the point.

              3. Third coordinate of the point.

              ( Also use:

              *Preprint, echo=NO, model=YES, history=YES, contact=NO

              So that you can look in the dat-file that all detailed input that is written there is what you specified. )

              After you have made these change save the inp-file under a new name and then run Abaqus using:

              abaqus job=new_name

              or:

              abq6113 job=new_name

               

              Best regards,

              Yordan Venev