Hi
I have modeled pipes and elbow (picture below) using *ELEMENT_BEAM_ELBOW using LSDyna. My model converged but somehow the results are not making sense. The von misses stresses are way larger than what is expected. When I check the d3plot, I found that the elbow elements are separating badly (picture below). It happens for the second elbow as well. My *ELEMENT_BEAM_ELBOW definition is as below:
*ELEMENT_BEAM_ELBOW
1 1 1 4 3 (element ID PID N1 N2 N5 and the row below is midpoint N3)
2
2 1 4 8 3
6
.............................................
*INTEGRATION_BEAM
1 0 0.0 9 2
0.161925 0.159125 0.0 0.0 0.0 0.0 0.0 0.0
*SECTION_BEAM
1 14 1.0 -1 2 0.0 0.0 0
0.0 0.0 0.0
Could anyone help me in this regard by giving me some suggestions what I am doing wrong? I did not get much help from manual and online. Thanks again.
Hi @mmia1,
Your elements are not actually separating, it's just a visualization of the beam cross section thickness. Prepost just displays offsets for each beam which end up looking disconnected (but they aren't).
It looks like you are attempting to define a tube (similar to a in the figure from the manual) but you are defining k=2 which would correspond to c in the figure. Maybe that's your problem? I'm unfamiliar with this definition specifically but doing a quick check, it looks like you have everything else defined correctly.
@negativevolume Thank you for the reply. I ran with your suggestion by putting k = 0 and ICST = 9 (tube section) in the *INTEGRATION_BEAM definition like below:
*INTEGRATION_BEAM
1 0 0.0 9 0
0.161925 0.159125 (D1 = outer radius and D2 = inner radius in m)
*SECTION_BEAM
1 14 1.0 -1 2 0.0 0.0 0 ( -1 indicates that user-defined integration will be used)
0 0 0.0
*DATABASE_EXTENT_BINARY
10 10 3
0 0 3 (3 integration points were considered, I chose it based on trial and error basis)
The model ran completely but my stress results are still high by ten times. I am attaching the .k file here. Below is the screenshot of beam von misses stresses.
@mmia1 when you say your results are x10 expected, which part are you referring to? And how are you sure of the expected stress? Did you do a hand calculation?
Also, have you looked into your material property?
@negativevolume thank you for the reply. I have model of this pipe-elbows as shell element instead of beam elements. Also, I modeled three straight pipes (no elbow) with beam elements. Both of these models give me about similar results. However, beam element model with elbow giving me 1.99e9 stress compared to 2.34e8 from shell and beam element with no elbow model.
I am using *MAT_PLASTIC_kinematic and all of these models had same properties.
@mmia1 I see. Have you attempted to model the same shape with standard beam elements instead of the specific *element_beam_elbow? Could just be a problem with that type of element in particular.
@negativevolume If I understand you correctly you are asking to use regular beam element (ELFORM 1) not *ELEMENT_BEAM_ELBOW for the elbow parts. I did not try that.
Do you think it is okay to use regular beam elements in the curved portion instead of available element in LSDyna *ELMENT_BEAM_ELBOW?
@mmia1 yes it’s 100% okay and probably the recommended way to model something like this. Beam elements can be used to define structures of all shapes, not just straight lines.
I’m honestly not sure what the purpose of the *Element_beam_elbow is. I’ve never seen it used.
@negativevolume Thank you for the suggestion. I will try to use regular beam elements. Let’s see what happens. I will post the update here soon.
just one last thing to confirm with you if possible. We know for beam element we have to define third node (n3) which defines the vertical axis of the beam or the beam face. In my case, should the n3 be chosen so that all pipes and elbows are pointing in same direction their vertical axis or beam face? Please take a note that I am considering hollow tube section for modeling the pipe. Thanks again.
@mmia1 I suggest reading through the link below and the section in the manual that goes over *Element_beam and when you need to define a N3 orientation node. I believe you should be able to use ELFORM=1 and define your inner and outer diameter of your tube and make sure CST=1. In this case, you won't need to define N3 for your beams.
https://www.dynasupport.com/howtos/element/beam
@negativevolume Thank you so much for your help. The model with regular beam elements (ELFORM 1) for both straight pipes and elbows gave me the expected results. It seems it is better not to use *ELMENT_BEAM_ELBOW.
Thanks again.