Hi to all!
Here I come with another problem for which I didn't find any discussions in this forum. It is concerning the PLOTEL elements. As the documentation says, they should help doing post processing. You will find some explanations there, but unfortunately no example and no explanation of the exact features.
My problem is described as follows:
I have a running simulation using the solver SOL101 linear statics. It is a simple analysis where I examine the deformation caused by a given load on a structure. For this setup I got some measurement data of a sensor at a particular place. Since I want to do several calculations and compare the information of the sensor, I added a PLOTEL element via a "node to node" 1D connection in the FEM-file. In advance, I createt a PLOTEL 1D collector and furthermore a group with the corresponding PLOTEL element and the two nodes.
Keeping in mind that the PLOTEL elements do not influence the model and are only used for post processing actions, I created an Output request for only the PLOTEL group. I chose, displacements, stress, strain and forces. Any other output requests have been removed.
What I realized so far is, that I only get displacements and rotations for the PLOTEL group. Is there a possibility to get more data?
What I want to do:
Let's imagine the sensor is a simple strain gauge. Then I want to have a fast possibility to compare the measured strains to the analysis.
My current work around (without the PLOTEL element):
I added a CBEAM element at the same place (connecting the same nodes as the former PLOTEL), with a 1x1mm cross section and a weak material (E=10MPa, nu=0). For some reason, I have to use the parameter BAILOUT=-1 to get the simulation running. But nevertheless, I can use the beam resultants (forces or strains) to compare with the measurements. My hope is, to do this comparison without adding (even very small) stiffness or material to the structure.
I ran some searches regarding PLOTEL elements in Simcenter, but I didn't find any good hints or tips. So I think this forum here is the right place to start a discussion.
Thank you in advance for all the help!!!
Solved! Go to Solution.
As you mention, PLOTEL elements do not influence the structure - they don't have any area, mass, stiffness, etc.
They are inherently a very simple/basic entity. The only thing that they "do" is follow the motion of the grids that they are connected to to show displacements. There is no possibility to report any other type of results output.
Thank you very much JimB for your quick answer.
OK. I'll have to deal with that. It would have been a nice feature, if these PLOTEL elements could act as some kind of measuring connectors. Just to evaluate some results which are already accessable like relative displacements between connecting nodes.
However, this one is solved and I am happy with my workaround so far.
Have a nice day.
In Simcenter 3D, relative displacements can be obtained via a Result Probe
Another alternative, in Simcenter Nastran, you can define a MPC between 3 grids - the two that you want the relative displacement measurement between (one with a +1 coefficeient and one with a -1) and a third, unconnected SPOINT or GRID. The first two grids will move with the structure and the displacement output at the unconnected grid will be the difference between the two.
1. I believe that PLOTEL are only for visualisation. That means the will only show a nodal result without elemental context. That means, only nodal displacements can be shown with PLOTEL elements. Stresses and so on are results with elemental context for which you need in most cases stiffness and elasticity. That's not existing for PLOTEL elements.
Therefore, the method to get strains by means of beam and bar elements are the right way.
2. As not all elements connect to all degrees of freedom of global grid points sometimes the model remains singular for parts of its meshing:
- All solid elements connect only to the displacement DOFs of grid points,
- ROD elements connect only to the displacement DOFs of grid points,
- BEAM elements connect to the displacement AND rotational DOFs of grid points,
- shell elements connect to to the displacement DOFs of grid points and to parts of the rotational DOF of grid points as mostly the rotational DOF at normal direction of face remains uncoupled.
So if you create a mesh made of solid elements all of rotational DOF of grid points are unset and yield ZERO stiffness. Here the AutoSPC functionality is coping the problem => All rotational DOFs are eliminated (if they have no stiffness value at main diagonal of stiffness matrix).
So, now you create a beam element coupled with two of these SOLID grid points. Now the elasticity of beam is introduced into stiffness matrix at displacement and rotational DOFs of grid points. Now the rotational stiffness values of main diagonal of stiffness matrix is not ZERO. But its not constrained for rotational torsional DOF. Therefore, the stiffness matrix is singular and not solvable.
You can check it by means of eigenvalue analysis to get as many rotational eigenforms as you have separated beam areas in your model.
"Bailout = -1" will introduce a stiffness value additionally for all DOFs at main diagonal of stiffness matrix. But that is the wrong way. Solution: Constrain all free DOFs in your model (here the rotational DOFs of beams) which are uncoupled to already existing constrains by means of elemental stiffness.
But keep in mind, you can destroy the model too when you introduce stiffness values which are to large.
(see MAXRATIO and EPZERO)
Best wishes, Michael
Thanks again JimB,
I will have a look to the result probe thing. I must confess, I didn't get the point of some of the options envelope, result probe ect. So, this I will focus on a little bit more.
The second point you mentioned, I will have to try. Am I right that I will create a MPC and define some kind of constrained equation? Best practice for me would be to test it with a minimodel. Thank you for the tip.
these are some good points. Actually, I expected something like that when messing around with the BEAM element. Now, I completely understand what's going on. So, from my point of view I can try three different things to get the simulation work without the BAILOUT:
1st: I use a ROD element rather than the BEAM, because the ROD will not "activate" rotational DOF and no singularity will occur.
2nd: I can pretend the BEAM to be a ROD by working with the PIN END FLAG options. I guess, if I deactivate all rotational DOFs in the definition card, the resulting BEAM will only connect the translational DOFs. Am I right?!?
3rd: I change nothing, use the BEAM element, but add a constraint to fix the rotational DOFs at both nodes forming the BEAM element.
Please correct me, if I'm wrong on that. I will try this using my minimodel.
Thank you very much. I really appreciate your help. Kudos on the way!
to 2. I'm not sure if a PINFLAG suppresses the definition of stiffnesss of beam element, as it is possible to set pinflags only at one end. I assume pinflags will introduce some kind of MPC coupling between the beam grid point and the solid grid point in focus. Then the problem is the same, as a beam coupled to a solid grid point behaves like a hinge joint. Pinflags introduce the same which is redundant.
to 3. That's the way I use. Keep in mind that you only have to constrain one side of beam as the other side is coupled by means of elemental torsional stiffness. Additionally, if you want to couple a beam with a shell element mind the orientation direction of beam. If the beam follows an edge of the shell, that DOF will bind the rotational DOF of beam automatically.
Best wishes, Michael