Learning Forum

[Rahima Ummi]

Hello,

I'm trying to run a non-linear analysis for a simple bolted connection in Ansys 18.2, however the analysis is not succesful.

 

It displaying the error : The solver engine was unable to converge on a solution for the nonlinear problem as constrained.  Please see the Troubleshooting section of the Help System for more information.

 

I have tried refining the meshing around the bolt hole and also try to incrementally increase the load.

 

Please let me know how I can fix this issue and complete my analysis. Thank you.

Attach bellow is the model for my analysis.

 

Regards,

Rahima Ummi.

[peteroznewman]

Hello Rahima,

Are you on the Student license with node and element limits, or on the Research license without limits?

1) In either case, open Inventor and delete the chamfers on the top of the bolt head and the bottom of the bolt shaft. Those faces are unnecessary for the analysis and create more nodes and elements which slows down the analysis, or on the Student license, forces smaller elements to be used without any benefit. While you are in Inventor, split the face of the bolt at the plane of the nut. That way, you can have one face to bond to the nut, and a second face to have frictional contact with the plate holes. The second face can also be used to add a Bolt Pretension load that tightens the nut and bolt and squeezes the parts in between.

2) Delete the Patch Conforming mesh controls and replace it with the Sweep method for all parts except the Nut and Bolt and set the sweep to have Number of Divisions to 2.  Put another sweep on the Nut and number of division can be 3 or higher. Use Multizone on the simplified bolt. You should always have a minimum of two elements through the thickness.

3) Insert a Contact Tool under the Connections folder and Generate Initial Contact Results.  Any Frictional contact in the direction of the bolt axis must be closed. Any that are not closed, you need to go to that contact, and under Geometric Modification, Interface Treatment, select "Adjust to Touch".

4) Under Analysis Settings, change Number of Steps to 1 and turn on Large Deflection. You have 30 initial and 30 minimum substeps. That is okay for now if your mode converges.

5) Delete your Displacement constraint. That does not simulate reality.

6)  Change the force to a Constant value of 1500 N in the X direction. The Step controls above will ramp the force up from 0 to 1500 in at least 30 steps. If you want results to view for a minimum of 50 steps, then set the initial and minimum substeps to 50 instead of 30.

7) On the Geometry tab, right click and Edit in DesignModeler. This will cause the geometry to be saved in the archive so I can edit it later. I will recommend that you add a centerplane through the center of the bolt, along the length of the plates so you can use Symmetry to cut your model size in half. This will save some time solving, but also allow a finer mesh while staying under the Student license limit. I can help with that if you can't figure it out.

Save the project and follow these directions to Archive the project and reply with the .wbpz archive file attached. You don't need to zip that, it will attach. After I receive that file, I can show you how to apply a bolt pretension load (and Symmetry if you didn't do that yet).

Another observation is that the bolt shank diameter appears to be equal to the hole diameter in the plates and washers. More realistic geometry would have a clearance hole, but then you have to do more work. In Inventor, stagger the parts so that the bolt shank is tangent to each side of each hole where it would make contact under the tension load, so the two plates are making contact on opposite sides of the shank. The washers would get an even larger clearance hole and you could leave them concentric on the shaft. For now, do the geometry you have with equal sized holes and bolt shank.

 Regards,
Peter

[Rahima Ummi]

Hello. Thank you for replying to my question. I will adjust it like your instruction. But i have a question, when I try to archive my file, the archive size is very large. Its up to 6 GB. Do you know what can I do to decrease the size?

[peteroznewman]

To minimize the archive size without losing a solution that is saved with the project, do the following:

1) In Workbench, Save As to a new name. I usually append the word Cleared to the existing name.

2) Now that you are in the Cleared file, right click on the Model cell in the system and select Clear Generated Data. This will delete the mesh and the solution.

3) Save the project.

4) Archive the project.

You now have two projects, but only use the Cleared one to send small archives.  As you edit the original project and make changes, you can repeat the process above, and overwrite the project with Cleared appended to the name.

If that file size is still over 120 MB, that may be because you have a lot of geometry in ANSYS. If you imported a large CAD assembly, but are only analyzing a few parts and suppressing the rest, make a new CAD assembly with only those few parts in it for import into ANSYS.

You didn't say if your license was Student or Research, but I'm going to guess it is Research.

[Rahima Ummi]

i'm sorry. I forgot to tell you about the licence. Yes, it is Research license. Based on your instruction, ANSYS successfully run the analysis for the model. Thank you so much for your help.

But when I tried to analyse the model when it have the clearance hole, it did not successful. So, I have a question about the part where you said that the geometry should have a clearance hole.

'Another observation is that the bolt shank diameter appears to be equal to the hole diameter in the plates and washers. More realistic geometry would have a clearance hole, but then you have to do more work. In Inventor, stagger the parts so that the bolt shank is tangent to each side of each hole where it would make contact under the tension load, so the two plates are making contact on opposite sides of the shank. The washers would get an even larger clearance hole and you could leave them concentric on the shaft.'

I do it like the picture I attach below. But I think the model is not correct. And about the washer, is the washer hole should be the same size as the bolt hole on the plate or is it larger?

Also attached below is the archive file of the model.

[peteroznewman]

Here is what I mean about holes that have a lateral load that puts them in contact with the shank of a bolt.

The washer is typically larger than the clearance hole, but it depends on the part chosen for the design.

[Sreenath1994]

Respected Sir, 

I am having a similar issue (non-convergence) when trying to carry out the non-linear buckling analysis of two rectangular plates (10mm and 20mm , simply supported on all 4 edges. As soon as the material gets fully yielded (250MPa) the solution has problems converging. Material plastic behaviour was defined as bilinear isotropic hardening. 

The load stepping was set to program controlled.

Can somebody please explain why the solver can't converge on the solution as soon as the entire material gets yielded although I have defined the tangent modulus.

I am on student license.

Thank you

This is the case for the 20mm plate.

[peteroznewman]

Sreenath, please create a New Discussion in the Structural Mechanics section to post this question. This is not your Discussion. Also, you can attach a Workbench Project Archive .wbpz file of your model to let me see what went wrong.