×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Modeling Simply Supported Members

Modeling Simply Supported Members

Modeling Simply Supported Members

(OP)
Hi,

This is my first post on these forums, but I have been lurking for awhile and find them very informative.  On to my question.

I've been asked to perform a preliminary FEA of a simple structure which consists of a frame with primary beams connecting to the columns, and secondary beams connecting into the primary beams and columns.  The beams support the deck, and the superimposed gravity loads on it.

So far, I have been using beam elements to model the frame (BEAM44 & BEAM188 specifically).  My question is this.  How does one go about modeling the connections as being simply supported?  I have tried many things, and anything short of making the connections completely rigid causes my model to be improperly constrained.

Thank you in advance for your help.

RE: Modeling Simply Supported Members

Got a picture to help visualise?

RE: Modeling Simply Supported Members

(OP)
Here is a quick MSPaint picture.  It's not the exact layout of the structure, but it is the same idea that I have come across on something else I have been working on.  The Secondary beams (blue line) connect to the primary beams (black line) and to the columns (red squares), while the primary beams are connected to the columns directly.  I hope this clarifies things.

RE: Modeling Simply Supported Members

you need to restrain your beams for rotation about the member y axis, if you don't the beams can rotate without resistance, hence the ill conditioning

An expert is a man who has made all the mistakes which can be made in a very narrow field

RE: Modeling Simply Supported Members

(OP)
That is something I already explored.  I should perhaps go through some of the thought process that led me to this point.  

Essentially, on a previous analysis I had worked on, it was the case where it was impossible to restrain both the primary and the secondary beam in their torsional directions since the column, the secondary and primary beams have coincident nodes where they meet.  So what I had done was to cut the beam a short distance away from the column, and applied my restraint against translations, and rotations in the torsional direction of the beam and about the z-axis, while ensuring the column remained rigid.  This technique seemed to work at the time.

I have tried doing the same thing in this case, and I have made sure to restrain the rotations about the y-axis for the secondary beams, and the rotation about the x-axis for the primary beams.  But doing this originally seemed tedious, but now that it didn't worked, it has made me me think that I was on the wrong track, and made me wonder if there is a much simpler way to achieve this, especially for the two beams that connect to the columns.

RE: Modeling Simply Supported Members

Not sure of the system your using, but have you any pin-flag options?

RE: Modeling Simply Supported Members

(OP)
I'm not exactly sure as I am relatively new to ANSYS.  But I have seen something like joint or mpc elements which might be similar to what you're talking about.  

RE: Modeling Simply Supported Members

For BEAM44 look at keyopt(7) and keyopt(8), which allows you to release rotational and or translational stiffness.  For BEAM188 you can use the ENDRELEASE command.

RE: Modeling Simply Supported Members

(OP)
TERIO,

When I contacted roi, that is what they suggested I do.  However, it did not have the desired effect.  All the commands do, if I recall correctly, is separate the different elements and assign a separate end node for each component (primary beam, secondary beam & column), then it couples them, which takes me right back to the initial problem where the model is ill-conditioned.  

rowingengineer,

What I have done now was apply a rotational restraint at the node closest to the ends of the beams, and I no longer get the error.  Is that what you meant by applying a restraint in member y-axis?  I did hand calculations for the deflections of the beam to compare with the FEA deflections, and the difference between the two was negligible.  

RE: Modeling Simply Supported Members

sure was

An expert is a man who has made all the mistakes which can be made in a very narrow field

RE: Modeling Simply Supported Members

(OP)
Thank you for your help. This was exactly what I was looking for. The analysis runs, and the results are looking good.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources