Modeling Simply Supported Members 1

[STpipe]

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.

 

[40818]

Got a picture to help visualise?

 

[STpipe]

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.

 

[rowingengineer]

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

 

[STpipe]

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.

 

[40818]

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

 

[STpipe]

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.

 

[TERIO]

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.

 

[STpipe]

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.

 

[rowingengineer]

sure was

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

 

[STpipe]

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