Bolted connection - your model may not be tied down enough warning .

[ssenbore]

Hi,

I have a large assembly of solids (using brick elements) and some components are connected to others by bolts.

- When I use 3D bolts, the setup runs smoothly.

- When I use the bolt idealization with a preload and surface contact between the bolted components (I need to get the force passiing through each bolt), I get Warnings that "your model may not be tied down enough or you may have a change in stiffness somewhere in your model which is too abrupt. Check DOF:25".  But at the end of all the iterations, it says "The solution has converged"

Problem is:

- The DOF referenced in the warning belongs to a solid part on which the General Fixed Constraint is placed (and its fixed in all directions).

- Material Properties are obtained from the Auutodesk Sim Material Library (A36 Steel.  So I didnt make up some arbitrary stiffness.

- The model is statically stable.  I think this because when I suppress the bolt idealizations and leave the surface contacts in, I get displacement of 3.5 e^9 inches (extraordinarily huge).  When I unsupress the bolted connections, I get displacements of 0.020 inches.

Can someone please explain why these warnings are there? How to make them go away? and/or If they are of any consequence and can be ignored.

Note If this helps, the solver used is the Sparse solver.

Thanks,

[AstroJohnPE · Accepted solution]

Hi ssenbore,

Here's what I remember about stiffness warnings. This is from a "long time ago", so I may not have the details 100% correct.

From what I remember, the stiffness warning can occur in two locations. One location is when forming the stiffness matrix, which looks like this in the log file. At this stage of the analysis, a warning may not be significant. (No warnings appear in this section from my sample model.)

**** Symbolic Assembly Using the Row-Hits Matrix Profile ...

 **** Number of equations                 = 50933

      Estimated maximum bandwidth         = 185

      Estimated triangle matrix nonzeroes = 3705371

      Symbolically assembled nonzeros     = 1768617

 **** Real Sparse Matrix Assembly ...

      in the upper triangle:

      number of entries in the profile    = 3705371

      number of nonzeros                  = 1768617

 **** Sparse Matrix Assembled

The other location where the stiffness warning is shown is when solving the analysis. That location would look something like this in the log file.  Ironically, the test model I opened to get these snippets from the log file is a contact model that gives the stiffness warning during the solution! In a contact model, the only warning that really matters is a warning on the last iteration (which occurred in my model!). The intermediate iterations are not a part of the final solution, so a warning on those iterations is not that important. Since my model was hand built and had weak 3D springs to provide stability, I know the elements are "perfect". My stiffness warning must be related to the stiffness of the contact (very low in my case) compared to the stiffness of the material (steel). The results look reasonable, but they may be less accurate than normal because of the stiffness warning.

**** Invoking Parallel BCSLIB-EXT Sparse Solver...

 **** Begin solving nonlinear equations of load case        1

       warning: your model may not be tied down

               enough or you may have a change in

               stiffness somewhere in your model

               which is too abrupt. Check DOF:50933

 ITER CLOSE OPEN frON fOFF    LOADFACT TOTALf CLOSED/TOTAL CRC-CHECK

    1  1922    0    0    0  1.0000E+00      0 1922/1922     D04394C8

      warning: your model may not be tied down

               enough or you may have a change in

               stiffness somewhere in your model

               which is too abrupt. Check DOF:50933

 **** Solution has converged.

In your model, the warnings may occur if the mesh has highly distorted elements in the solid parts. Or if you made the properties of the beam element bolt spokes too large, they could be causing the error. Be sure to check the displacements, stress, and reaction forces to convince yourself that the results are reasonable.

[ssenbore]

Thank you for your reply.

The warnings I get are in the 2nd case (when solving the analysis). And it shows the warning on the last iteration).

The beam element bolt spokes are 1.5 times the bolt size, and there are 24 spokes. Did I define this wrong?

The displacements seem off. (0.012 for a preloaded bolt idealization and 0.008 for a 3D bolt without preload).

If this helps, when I open the ldd file, I notice that there are 2 extra parts in there that I did not design. Both contain gap elements, and seem to be associated with the surface regions in the model.

Any advise on how to tweak the model? Also, when reviewing the stresses and reactions, what should I be looking for to convince myself of reasonable results?

Thanks.

Shayee Senbore
Technical Specialist
Boundary Systems
O: 440-274-0291x316 | C:216-538-3397
Skype: shayee.senbore
www.boundarysys.com
www.creoracing.com

[Description: Description: C:\Users\Ndarhinger\Desktop\Graphics\Facebook-Icon.png][Description: Description: C:\Users\Ndarhinger\Desktop\Graphics\Twitter-Icon.png][Description: Description: linkedin][Description: Description: C:\Users\Sales\Desktop\youtube.png]
[cid:image006.jpg@01CF225F.94DBBD20]

[ssenbore]

I was able to review the model, and determined that the results were very consistent and comparable to cases where I ran the simulations with 3D elements instead of idealized bolts (even though I was still getting the warnings with the idealized bolts).

The reactions, displacements and stresses checked out OK.

Thanks for your response AstroJohn PE