Learning Forum

[venkyvenkatesh374]

Dear All., Am trying to do a structural analysis of Aircraft. I have done the composite skin in ACP pre, then imported model in static structural. 

when am soliving am getting an error message related to constraints. I'll post an error message here, also enclose the archive file of complete setup. I need to understand whats the error and how to resolve it. 

*** ERROR ***                           CP =      16.891   TIME= 10:43:22
 The value of ROTY at node 11266 is 378238423.  It is greater than the  
 current limit of 1000000 (which can be reset on the NCNV command).     
 This generally indicates rigid body motion as a result of an           
 unconstrained model.  Verify that your model is properly constrained.  

 *** ERROR ***                           CP =      16.891   TIME= 10:43:22
 *** MESSAGE CONTINUATION ---- DIAGNOSTIC INFORMATION ***               
 If one or more parts of the model are held together only by contact    
 verify that the contact surfaces are closed.  Also make sure that      
 there are constraints (or friction) in the sliding direction even if   
 no load is applied in that direction.  You can use the CNCHECK command 
 to check the initial contact status in the SOLUTION module.        https://drive.google.com/file/d/1Q8GIiKO4gOEY2ZNF6tdJRxHo_d1BwwWq/view?usp=sharing

[venkyvenkatesh374]

I want to understand how to close these contacts , Like adjusting the value or repairing the cad file. if its adjusting the value, how do i do it??

[peteroznewman]

Open the Geometry in SpaceClaim.  On the Workbench tab, click the Share button then the green check.  Now all the edges that touch surfaces will be connected to shared nodes in the meshing of the ACP/Pre block. I opened the Model cell and suppressed all the Contacts. I added a Modal analysis to the Model cell of Static Structural to show that all the parts are connected. What you can see is there is a need for a contact on the trailing edge of the wings.

[venkyvenkatesh374]

Hello Sir, Kindly appreciate the effort. so modal analysis is the key to check if all the edges been connected to surface is it??.

I've shared topology in Space claim, and clicked green tick, few edges turned blue, which am assuming connection is being created between edge and surface. 

few being red only, which i argree there's no surface, so i'll have to edit the geometry or adjust in mesh to fill those gaps.

In ACP I've supressed all the connections, Now I can directly go to modal analysis to see if any connections aren't there right?? also in modal analysis any loads being given to see the frequency sir? Coz when i did, its showed zero frequency throughout and only tail fine was deforming away from the boom( Pic 2 reference), But In space claim the edge colour turned blue., so am bit confused here.

[venkyvenkatesh374]

[peteroznewman]

Modal analysis is a useful diagnostic test for checking that the mesh is connected or bonded contacts are working. There are no loads in a modal analysis.  You can run it with no supports, but if you do, the first 6 modes have zero frequency if there are no unconnected parts.  The default number of modes to compute is 6 so that is not very useful, so I always request 12 or 20 modes.  It a part is unconnected, you will see it float around when you plot the deformed shape of all modes.  Notice that I plotted mode #9 to show the flapping of the wing rear edge.

Your modal result shows that the tail fin was not connected to the other surface. I’m not sure why. What version of Ansys are you using?  I opened your model in 2025R1. You can Unshare the surfaces, then on the Repair tab, try extending the edge of the fin to the surface of the spar and redo the Share operation.  You can also use a larger tolerance on the Share operation.

 

[venkyvenkatesh374]

Hello sir, Sorry to reply late.

I have unshared the topology and shared with more tolerance value, In modal analysis i set the modes to 15, I see no floating surfaces. But under contact tool there's more warnings.I want to know if these warnings can be adjusted with pinball radius value, if yes i want to know how sir. 

Enclosed snips, can you please take a minute time and assist me with this sir.

 

[venkyvenkatesh374]

[peteroznewman]

The Share button should make all the mesh connections you need if the geometry is properly trimmed. After doing a Share operation in SpaceClaim, open the model in Mechanical and under the connections folder, delete all the contacts. Solve the Modal analysis and check animations of modes 7 and higher to verify that all the edges that should be connected are behaving properly.

[venkyvenkatesh374]

Hello sir, Sorry to reply late.Share option solved the problem patially. Also in modal analysis i was able to see unconnected edges. I deleted those connections and created manual connection between edge and surface which solved the problem.

My sincere thanks for your involvement and suggestions sir.