ANSYS WORKBENCH - BEAM ELEMENTS - PROBLEM 1

[Tiagomota]

Hi everyone!
I started a few days working with ansys, now I try to analyse a structure with many beams. I used the designmodeler to construte my model (I use points, lines and cross sections). When I use only 1 line with a few points and only 1 cross section I can obtain results, but when I modified my model and use a lot of lines to alow use more than 1 cross section and different orientations I can't solve de simulation. Ansys return:
"An internal solution magnitude limit was exceeded. Please check your Environment for inappropriate load values or insufficient supports. Also check that your mesh has more than 1 element in at least 2 directions if solid brick elements are present. Please see the Troubleshooting section of the Help System for more information."
*** ERROR *** CP = 3.728 TIME= 15:04:44
The value of UZ at node 13378 is 7.061632235E+09. It is greater than
the current limit of 1000000. This generally indicates rigid body
motion as a result of an unconstrained model. Verify that your model
is properly constrained.

In fact I use exactly the same supports and loads.

Another question: In connections ANSYS generate automatic and the state is "Fully Defined" but I can't visualize the connections in field "geometry" why?

Thanks a lot!

Best regards

 

[davemechuk]

"This generally indicates rigid body
motion"

When ever you get an error like this it means that you have not constrainted your model enough, ie something is being displaced at an infinite distance and so has aborted the job, make sure you have applied your Boundary conditions correctly and/or check your beams are tied/connecting to each other.

Note that I don't have much experience using Beams in the Workbench UI (I always use APDL for beams), so I can't be of any more help.

Dave, Msc(Eng), AMIMechE
Graduate Stress Engineer
(3 Years left for Chartership!)

 

[Tiagomota]

I check many times the boundary conditions, I will continue search the solution for this problem.
Thanks a lot.
Best Regards

 

[Hurricanes]

In design modeler, try using 'join' to connect all the beams to each other.

 

[Tiagomota]

Hello Hurricanes.
Where's the option "join" in designmodeler? I have ansys workbench 14.5 and I tried locate this option in help and I only found "joint".
In another way I was able to solve my first question... in design modeler I make a new part from every line body... this solution works....
Thanks a lot.

Best Regards

 

[davemechuk]

Ah sounds like you hadn't setup your connections with your beams.

You must have done the following in Design Modeller:

Highlight selected parts under the part tree, RMB 'Form new part'.

What this does is create a 'mulit-body part' what this means is that the new part at the interfacing points/edges/faces share nodes, meaning that effectively ansys recognises it as a single body. Allowing loads to transmit from one body to another through these shared nodes.

If you don't create a multi-body part the beams will have their own nodes at this single conincident point meaning the beams are floating in space and are not connected to each other. Another way to stop this from happening for shell/solid bodies is by creating connection constraints in Mechanical (Bonded contact for example).

Just remember to surpress the original beams as they will still exist in the parts list.

Dave, Msc(Eng), AMIMechE
Graduate Stress Engineer
(3 Years left for Chartership!)

 

[Tiagomota]

Thank you a lot Davemechuck. You help very much!

I understand what you mean but at this momemnt I'm working in the same structure but in this case is a 3D model instead 2D. I proceed the same way (create points and beams) and in the final I create a multi-body part with all beams but ANSYS return exactly the same error that I receveive in the initial problem. In 3D structures I need create different multi-body part? for example I nedd create a multi-body part with the beams who are in the same plane?

Thanks a lot!!

Best Regards

 

[Tiagomota]

Davemechuck when you say in another way I can create connections constraints in Mechanical in this case I can't create a multi-body part in design modeler correct? Only transfer the line bodies to Mechanical and add the connections have I right? Another question: The best way to meshing beams are use mesh control ---> Edge sizing?
Thanks!

Best Regards

 

[Hurricanes]

Sorry I left the 't' off, joint. Use joint to 'weld' all the beams together. To form a single body as davemechuk says, select all your like line bodys from the lefthand list, right click and create a new part.

 

[wchaiane]

I am actually having the same problem. I tried the "form new part" option, but than an error occurred in solution (although I tried different meshes). I also have no valid option for "joint" in Design Modeler in this case (Ansys 13).

I think the question might also be: how can we unite line bodies with contacts?

 

[rb1957]

it sounds like you have beams that you want to join together. i'm assuming that each beam has it's elements created as an individual so that at a junction between two beams there are two coincident nodes ... yes?

a simple way is to have the same node at the end of both beams ... there should be some way to do this automatically but maybe you edit one element changing the co-incident node ... yes?
beam 1 ... node 1 to node 2
beam 2 ... node 3 to node 4
these join so that node 1 is coincident with node 3
to "weld" the beams together change beam 2 to ... node 1 to node 4

Quando Omni Flunkus Moritati