simulate of thin walled bolted connection

  • 48 Views
  • Last Post 1 hour ago
submero posted this 2 weeks ago

plz help me to solve this problem. always the solve have errors for convergence 

i want any tutorial for it

 

Attached Files

Order By: Standard | Newest | Votes
submero posted this 2 weeks ago

akhemka posted this 2 weeks ago

Hi,

Looking at the image above - I am not able to see bisections before non-convergence. Can you please check what exactly the error is in Solver Output file. There is rigid body motion indication in the warning. Please see if the model is properly constrained. Also please turn on the Newton Raphson residuals to see the region of force imbalance. 

 

 

 

  • Liked by
  • submero
submero posted this 2 weeks ago

it is the same error 

but when i use smaller force like 10 N instead of 100000 N the error not occurred

" USE SPARSE MATRIX DIRECT SOLVER "

 

peteroznewman posted this 2 weeks ago

 You added the Newton-Raphson Residual Force plots to the Solution Information details.

Now there are 3 plots under that folder. Please expand that folder and show us an image of those three plots (or just one if they all look the same).

Regards,

Peter

  • Liked by
  • submero
submero posted this 2 weeks ago

Peter thank you

 

 

peteroznewman posted this 2 weeks ago

The location of the Max NR Residual Force is where you have to add Mesh controls to create smaller elements.

  • Put a Coordinate System near the location of Max NR Residual Force.
  • Add a Sizing Mesh control, and select the solid body as the Scope for the control.
  • For Type, select Sphere or Influence, then select the Coordinate system created in first bullet.
  • Enter a Radius that captures all the locations shown in the three plots.
  • Enter an Element Size that is at least half the current size or smaller.
  • Solve and repeat the process if it still does not converge, but also double the Minimum number of Substeps.

Guidelines for Posting

  • Liked by
  • submero
submero posted this 1 weeks ago

thank you Peter

but i have error

i make face sizing by t/4 = 0.5mm

step

10

10

100

submero posted this 1 weeks ago

i want to attach the wbpj file to fix this problem 

but i can't

"file extension not allowed"

 

peteroznewman posted this 1 weeks ago

You must create a Workbench Project Archive .wbpz file by following these directions. Then attach the .wbpz file.

The .wbpj file is not useful on its own.

submero posted this 1 weeks ago

what about error ?

I'm so sorry for my repeated questions

 

peteroznewman posted this 6 days ago

You have a sheet metal form that is currently represented by a solid model and being meshed with solid elements. This is a poor way to model the structure.

A better way is in SpaceClaim, create a Midsurface from the solid body. Then the solid body will be Suppressed for Physics leaving the Midsurface.  Apply the loads and supports to this surface body.  The surface will be meshed with shell elements that will have the thickness of the sheetmetal assigned as a property.

A shell model will not suffer from the convergence difficulties that you have with solid elements on a very thin solid.  The reason is you need four elements through the thickness of thin solids that see bending loads, while a single shell element can accurately compute bending stresses.

You can delete that really long post with the Solution Output. We don't need that anymore.

submero posted this 4 days ago

thank you for your replay and your help

but still error exist

i will attach the file please help me   

Attached Files

peteroznewman posted this 4 days ago

You were correct to put in the Contact Tool to find out the Initial Contact Status.
Unfortunately, some of the contacts are Near Open.

These contacts are only open by a tiny amount, but that is enough to prevent the solver from converging.
The corrective action is to select these four contacts and set them to "Adjust to Touch" to close them.  Here is Nut1.

Change the Interface Treatment to Adjust to Touch. Do that for all four Nuts. You can do four at once if you pick all four.

After you do that, the solver will fail to converge due to elements that are too large on Bolt 2.

The corrective action is to use smaller elements on the bolt head.

There is also a high N-R Residual Force on the beam end where the force is applied.

You could use a few more elements around the corner, but why is the force only applied to one edge?

Pick all the edges to apply the force to, not just one.

Regards,
Peter

submero posted this 4 days ago

Hello Peter,

Thank you for followup my problem but the error not solved

1- I changed four contacts and set them to "Adjust to Touch" to close them but still near open.

2- the solve not converge at time step 1.35 as before.

3- Also applied the force to all element at the top.

I will attach the file i hope you try to solve it, thank you again for the previews useful information.  

Attached Files

peteroznewman posted this 4 days ago

Hello submero,

I haven't looked at your model, but you didn't fix the problem that causes the model to fail at 1.35.  The elements in the bolt head are too large. You need to add a mesh control to create smaller elements on the contact face of the bolt head. Currently there are 2 elements across the contact face. Make sure there are at least 4 elements across the width of that face. Same on the Nut face.

After you make that change, if the solver fails to converge, please reply with the N-R Force Convergence Plot and the N-R Residual Force Plots and their details window to see where the solver is having difficult converging. Once you know which part and where on that part, the corrective action is to use smaller elements.

Let me know what you find.

submero posted this 6 hours ago

Hello Peter,

I meshed all contact parts with 0.5 mm although the model is shell element with thickness 2 mm, resulting in the time of solution reached to 66 hrs.

1- bolt and nut mesh

 2- I have the same error

3- I have 6 N. R all the same at this point

peteroznewman posted this 6 hours ago

Hello submero,

Nonlinear models can fail to converge for many reasons. In a model with plasticity that is loaded with a force, one reason the solver can fail to converge is that the solution has reached the ultimate load capacity of the structure and there is no static equilibrium at the next increment of force. If you plot the force-displacement curve and the slope is approaching zero, that is evidence that this is the reason for the failure to converge.

The corrective action is to change from a force loaded model to a displacement loaded model. While the solver will fail to converge as the force-displacement curve approaches a zero slope, the displacement loaded model can continue to increment the displacement to the next increment, but the reaction force will decrease.

Please plot the force-displacement curve and show the slope. Note: you have to require the solver to take small time increments by using a large value for minimum substeps to get many points on the force-displacement curve.

Clear the mesh and File Save As to a new file name that you can create a Workbench Project Archive .wbpz file to attach to your reply.

Regards,
Peter

submero posted this 1 hour ago

Attached Files

Close