Beam element stress output question

JRP

Hello,

I have one simple question about stress output on beam elements in static 3D analysis. Attached is the example with simple enclosed ring. This is just one more analysis simplified, so top and bottom curved remained full bar steel and side are steel tubes.

Check attached hand check calculations. Because local coordinate system of elements is antisymetric, we get different stress outputs. On one side we have bending stress added to normal stresses and on the other side substracted because of moment sign. I hope I'm clear enough...

Is it possible to simplify stress output on beams, so one stress plot would show maximum stresses in elements (normal + bending) in absolute values?

Thanks for help...

Victor

Do you want to show the maximum value of normal+bending stress over the cross-section of the beam? I can't think of a way to do that, but you can at least see both sides simultaneously using any of the 4 "point #" stresses in the older version of your screenshots or "stress UU" in version 9. That doesn't require you to know the orientation of the element axes and doesn't have the discontinuity at the ends.

JRP

Ok. That's good. But that is possible only graphicaly. I can't select a node and check stresses there, because we have 4 possible points.
It would be great if it could be possible to sum normal + bending stresses and show them as maximum plot. That is sometimes needed for simpler presentations.

What about maximum stress range for selected components. If I have all components selected in solution, then stress range is set from min to max over all of these components. If I select one component, stress range stays the same. Sometimes it is nice to show maximum and minimum stresses for just one component.

Victor

Version 10 will probably have max and min functions added to the formula tool so you'll be able to create a new plot that way.

To set the contour plot range to fit a selected component, right click one of the selected elements and choose Fit contour plot max/min to selection

JRP

Ok. Good again. Thanks. But as I can see it is only possible for point 1, 2, 3 and 4 and not for "stress UU".

Do you have any examples for manipulating with plots with formula tool for beam elements?

Victor

That's a limitation that it doesn't work when it's displaying multiple variables together, sorry.

Here's an example of a formula for absolute value of longitudinal stress in MPa.

JRP

Ok. Thanks. I will check it out and see. Talk back soon...

disla

Hello JRP,

Something strange here.
Stress on the beam should not depend on axis orientation. It is an invariant under rotation.
Something is not properly represented when we see two different values of bending on the plot.

I do not think you are completely right or at least I would not say it this way when you say, "Because local coordinate system of elements is antisymmetric, we get different stress outputs".

From my point of view, you are getting different stress outputs because you have defined the Stress recovery points V=6mm and W=6mm for both sides the same. One side should be recovered at V=-6mm W=-6mm in order to compare apples with apples as local axis are as you say antisymmetric.

See attached files. There are two options. You can fix the axis to be the same at both sides or you need to define different recovery points to take care of axis different orientation.

Oh and by the way Victor , ¿has the option to propagate axis orientation to the neighbours disapear in version 9? I don't see it in the experimental tools.

JRP

@ Victor: Ok. I've checked the formula definition. That will be useful in the future. I will try and see what other options can I get out of that. Thanks...

@ disla: I agree, but it is not practical to have so many materials defined in complex calculations. Too much things to look for. I like second option more - with axis orientation. It's also better and more clean to use and read results.
But what is the simplest way to turn element axis after it is defined?

disla

In Mecway 8 there is an option in Tools/Labs/Propagate axis orientation to the neighbours. Very useful and it normally works pretty well.
This option has disappeared in MECWAY 9 and it is replaced by the option to automatically set the axis orientation to your elements as a constrain/New element orientation.

Victor

For beams, you might also want to reverse their longitudinal (U) axis, which is Mesh tools -> Invert.

JRP

That doesn't work for me. What am I doing wrong?

Victor

Select some elements, then click Mesh tools -> Invert. It might be hard to see the axis lines but the red ones (U) are reversed. One of the others will be too to retain the right handed coordinate system.

JRP

I see now. But disla showed me reversed z axes of elements, so that they are all pointing out of the ring. With inverse command we inverse only x and y axes, z remains the same.

Victor

Sure. The node connectivity (changed with Invert) defines the U axis while "orientation" defines the other two axes.

An easy way to make them all point out is with Loads & Constraints -> New element orientation like the attached picture.

JRP

Ok. I will check it out and see... Thanks.

Is there anyway to define axes during element definition? Something like which node is selected first?

Victor

The U axis is defined like that, yes. If you make the element using New element then it's directed from the 1st node to the 2nd. The other axes only have a fixed default orientation until you specify a new one.

JRP

Hello again with one question regarding stress output in beams.

I attached a LIML file and few screens from Mecway. I'm doing stress calculation for a simple tripod and I question the maximum stress output.

1) If I understand correctly UU stress reports axial + bending stress in 4 predefined points on a beam?
2) Points 1 to 4 under UU stress are then graphical representation of these four points? Why are the maximum values not the same as in UU stress that graphicaly shows all four points togehter?
3) With this tripod modeling, beam orientations are predefined and are different for all of the three main legs, so reading stresses is hard. How would you recomend to orient bemas in this kind of calclculation, so that maximum stresses are not overlooked?
4) Why do I get larger maximum stress in user defined point than in any of five previous outputs (UU, points 1-4)? I defined my points on the edge of the element and if I understand correctly they should be coincident with two of predifined points.

JRP

Forget question number 2. I checked again and I saw that maximum under UU are the same as under points 1 and 3.