Bolt modeling in Workbench

[arm100]

Guys, I am having a problem using the bolt feature in Workbench. I have defined all contacts as No Penetration, but the solver gives a "Rigid Body Motion" error. Can you tell me what is wrong. I have made a simple model of two L brackets clamped together by a single bolt to test out the bolt feature,and am getting the same error.

 

[sdra2]

Is the bolt going through a clearance hole (it needs to)?

Do you have a discrete cylindrical surface 'free in space' that you have applied your bolt load to, or have you applied it to the whole bolt shank?

Is there a nut on the other side of the grey bracket, or is it a blind hole you're threading into?

It's probably a good idea to spell out loads and constraints, as well as post the key solution file information. Also, a mesh indication might help - specifically the hole edges, and the contact surfaces. Do you have the Newton-Raphson contact convergence tools in your level of Workbench?

Cheers

 

[arm100]

Thanks for your comments,

The hole and the bolt are exactly the same size.I have applied the bolt force to the top circular face of the bolt head (maybe that is the problem).The nut, bolt shank and head are one solid part.I will have to check to see if I have N-R conatact convergence tool.

 

[sdra2]

Well, I would start off with some small clearance around the bolt and ensure that there is no contact here. I'd then make sure there was a "split cylindrical surface" on the bolt shank where it is clear, and put at least 2 or 3 mesh elements lengthwise on this split surface. For your load apply the Workbench supplied "bolt load" to this split surface.

You will still need to remove rigid body motions somehow I suspect, but just ground one of the bracket faces to start with to make sure that it not the contact that is giving you issues. If it is the contact, try putting a finer and more uniform (matching) mesh on the contact surfaces to start with.

 

[arm100]

Thanks for the tips. I will try them and let you know.

 

[PriamEngineering]

I have applied the bolt force to the top circular face of the bolt head (maybe that is the problem).


Yes it is.


have you any additional boundray conditions? It might ne flying off into space!!!!

workbench is a bit different from ansys classic. in that when you preload a section it places the cut plane in the middle of the section. Which may (in some cases) be in the engaged threads of your model.

http://www.priamengineering.co.uk

 

[arm100]

I do have constraints on one of the brackets and load on the other. I have applied the preload to the shank and have made sure that mesh is compatible between hole and bolt shank. The results look reasonable (both stress and displacements) but the error is still there. I will next try these on the actual problem (a cylindrical shape device 14 ft DIA X 50 ft long in 3 sectios) to see if the error continues. This geometry is more constrained than my test.

Thanks for all the help.

 

[PriamEngineering]

how many load steps are you using? Normally for what you are doing you need 2.

1. first to tighten the bolt
2. second to apply the load and extract the axial bolt force

http://www.priamengineering.co.uk

 

[sdra2]

What is the "rigid body motion error"? I think Workbench adds what it calls weak springs to remove rigid body motions and I seem to remember it doing this for bolted joints more often than many other types of analysis. If it has done this, I think (from memory, not used Workbench for a while) you can look at the reactions (forces, moments) at these springs. If these are low in comparison to the reactions at your applied constraints, it MAY be that the analysis is okay as is.

 

[arm100]

According to what I read, the two steps are done automatically within workbech. The springs were added and the forces as you had guessed did have very small forces on them, so I am becoming convinced that the results may be Ok eventhough the software issues this error. I thank you guys for the timely and valuable responses.

 

[sdra2]

If you look at your "solution output" or "solution convergence" graph (can't remember the exact terminology, sorry) you should see two traces. These overlap when the solution has converged. For a bolt load analysis, the two traces have to converge twice: once for solving the bolt preload, and a second time for solving the other loads afterwards. There will be a dashed vertical line (blue?) somewhere on this graph at the first convergence point and this is the best check to see if Workbench has applied your loads in two steps automatically as you suspect.

 

[arm100]

Solution Information does indeed show convergence of both steps. Thanks a lot guys.