node value discontinuity

sofien_73

I Victor
I have some trouble with internal force discontinuity see the two pictures. When you extract beam force axial value there's some there's discontinuities with nodal plot which it's not the same with element value. It maybe average value between both elements sharing the same node. Is there some tricks to have the same results as element value but with nodal value (maybe my claims looks to have no sense but It should be much more easier to automate design).
Regards.

Victor

It's not possible with the same mesh since a single node can only have one value for each variable.

You can disconnect the members at the connections, keeping the nodes at the same location and then join the nodes with constraint equations (all 6 DOFs equal for each node of the pair).

sofien_73

Thank you Victor, in my model there's a lot of connections between beams.
Is there a way to spot nodes which shares the same position?
How do you manage constraint equation with these nodes?
Regards

Victor

You can use View -> Open cracks which separates coincident nodes.

Another thing I sometimes do is Mesh tools -> Merge nearby nodes and check the total node count to see if it went down, then undo. Doesn't show you where they are but does show how many.

The GUI isn't very convenient for coincident nodes so constraint equations on them are probably best generated externally if you have more than a handful.

sofien_73

Thank you Victor

sofien_73

Hello, Victor, I've performed the connection between nodes with constraint equation this way for exemple on the liml file(nodes 61 which is the master and 82 the slave):

























Something goes wrong because my file doesn't complete solving stage and the software send a message saying that there's a problem with the constraint equation.

May I've done something wrong? I can send you the file if necessary

Regards

sofien_73

sofien_73

Another question arise, how to deals with multiple nodes to constraint?
For exemple 4 elements can share 4 nodes at the same position (x,y,z). How to deals with constraint equation in that case? We have to choose a master node to link with the 3 others? maybe the answer can solve my problem if it's not a syntax issue.

Regards.

Sebastianmaklary

@sofien_73 Tying all others to one or tying them to each other in series could be a common method. When, in CAD software, I apply constraints such as equal size, parallelism or similarly to multiple selected entities, the software will apply the constraints in series such that the second entity is constrained to the first, the third is constrained to the second and so on. It means that deleting one entity may break the chain of constraints but then it is just one constraint that needs to be added whereas all of the constraints needs to be reapplied if it was tying to a master entity and that was the one entity that was deleted. Thus, I'm not entirely sure which of these are preferred or is most robust but the commercial CAD softwares apply constraints in series in those cases.

Victor

@sofien_73 What you posted looks OK. A likely problem is that the node-dof pair that's the first term in each equation is the condensed DOF and is not allowed to appear in any other equation, nor various other constraints.

For more than 2 nodes, this means you can't connect them in a chain like @Sebastianmaklary suggested. However, you can use one node of the nodes as a master entity which all the other nodes are set equal to. This turns out to be a special case of Node-surface coupling - rigid (RBE2). So it could be easier to use that instead. Apply it to the end faces of 3 beams and use the node of the 4th beam (or some extra unconnected node) as the reference node.

sofien_73

Thanks Victor, in order to be sure I send the model once again with constraint equation and hinges. With or without hinges the issue is the same with this error message from MW when I run the case 1:
00:00 Start 18:33:39 .
00:03 Allocating matrix
00:03 Error: Incompatible constraints on nodes 61, 152, 243, 284, 304, 324, 365, 375, 385, 395, 415, 425, 456, 466, 476, 486, 506, 516, 587, 628, 638 ....
00:03 Failed

those nodes are actually triple (3 nodes / 3 elements / one position (x,y,z)) and all these nodes are linked with constraint equations for all dofs (for example node 61 is the master of the two others 82 and 1655). I really want to stay on the constraint equation method if it's possible because using end face of beams will be impossible to script in a iterative approach. Could we stay on a node approach?
Regards

Victor

Yeah, it's the condensed DOFs appearing in multiple equations problem. For example, x displacement on node 61 is the condensed DOF in both these equations:

  <constraintequation>
    <term coefficient="1 1/m" nid="61" dof="ux" />
    <term coefficient="-1 1/m" nid="82" dof="ux" />
  </constraintequation>
...
  <constraintequation>
    <term coefficient="1 1/m" nid="61" dof="ux" />
    <term coefficient="-1 1/m" nid="1655" dof="ux" />
  </constraintequation>

Change the order so the 1st node isn't the common one like this. Now node 61 becomes the single independent node and the other two (82 and 1655) are both condensed.

  <constraintequation>
    <term coefficient="-1 1/m" nid="82" dof="ux" />
    <term coefficient="1 1/m" nid="61" dof="ux" />
  </constraintequation>
...
  <constraintequation>
    <term coefficient="-1 1/m" nid="1655" dof="ux" />
    <term coefficient="1 1/m" nid="61" dof="ux" />
  </constraintequation>

sofien_73

Thanks you Victor, it worked perfectly. One last question, the beam releases can be managed by two methods :
-using hinges with the flexible joint on beams methods
-using contraints equation only on ux/uy/uz which means that the other dof are free to move in rotation
The second method are much more easier to compute but I want to be sure that these two methods produce the same effects on the global behavior of the frame.
Regards.

Victor

They are supposed to have the same effect globally, yes.

sofien_73

Thanks a lot Victor, for the future version of the software maybe another method for the beam release for the beams which are not compliant with the global axes for these one we can't use constraint equations.
Regards