Learning Forum

[Ankush2302]

hello,

I've been trying to do 1D simulation on a space frame structure with beams. However i'm facing problems with the solution. I get following error message:

Text: "An unknown error occurred during solution.  Check the Solver Output on the Solution Information object for possible causes."

Association: "Project>Model>Static Structural>Solution"

Upon checking the solution output I found following errors messages:

 "*** ERROR ***                           CP =       2.219   TIME= 15:23:46  A boundary condition has been imposed on node 552, degree of freedom 1    of the element 3304.  Currently, ANSYS does not support such a set-up.     Please avoid boundary conditions on nodes forming the joint element.     *** ERROR ***                           CP =       2.219   TIME= 15:23:46  A boundary condition has been imposed on node 552, degree of freedom 2    of the element 3304.  Currently, ANSYS does not support such a set-up.     Please avoid boundary conditions on nodes forming the joint element.     *** ERROR ***                           CP =       2.219   TIME= 15:23:46  A boundary condition has been imposed on node 552, degree of freedom 3    of the element 3304.  Currently, ANSYS does not support such a set-up.     Please avoid boundary conditions on nodes forming the joint element."   

I have tried a few things but nothing seems to work. Please help me in finding a possible solution.

[peteroznewman]

You will have to show images of your model, the boundary conditions, joints and loads so we can help you.

[Ankush2302]

can i send you the workbench file?

 

[jj77]

You can attach your model in your post - see here how to do this:

/forum/forums/topic/saving-sharing-of-working-project-files-in-wbpz-format/

 

Finally I have spent sometime helping civil engineers that analyse mainly frame strictures, and in most frame or general purpose FEA  software that do design also, there is no notion of joints - and hence they are not used.

 

Elements are connected directly since they share common odes - if we need some special features then one can use end releases to decouple dof between beams - so one never uses joints (in the ansys sense of joints) when modelling frames say buildings, because it creates unnecessary constraint equation which are not necessary in frames. 

 

So just get rid of them and model it in a simple way.

To connect all the members/beams/columns, just model them in design modeller and then create multi body part, or share topology in Space claim, and in that way they share nodes. If you need to have say a pin release just use end release in ansys, very simple.

[Ankush2302]

 I have attached the .wbpz file along with the post.

[jj77]

The message is clear - always read them through.

 

The problem is the constraint equations generated by the joints and the simply supported condition at the same location (say node 470).

 

Just take them away as I said and use end releases (pinned so ROTX/Y/Z or just ROTZ). Anything else is just complicating things, and I would never trust results 100 % when MPC and constraint equations are used on something as connecting simple beams.

 

Else try using remote displacement instead of normal disp. BC. Have in mind though that you have pinned it so the structure is not stable since you do not have any base supports to prevent it from spinning/rotating about that point. If it is fully fixed then this method works (remote disp.) - even though as I said to use MPC, and other constraint equations is not recommended. Keep it simple with end releases and all beams sharing nodes via shared top. or one multi body part. In that way we can eliminate the additional unknowns and complexity coming from all constraint equations which are not necessary, making it straightforward to interpret and verify results.