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

i want any tutorial for it

- 177 Views
- Last Post 17 October 2018

submero
posted this
04 October 2018
- Last edited 04 October 2018

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

i want any tutorial for it

submero
posted this
05 October 2018

akhemka
posted this
05 October 2018

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.

submero
posted this
06 October 2018
- Last edited 06 October 2018

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
06 October 2018

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

submero
posted this
06 October 2018

Peter thank you

peteroznewman
posted this
06 October 2018
- Last edited 06 October 2018

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.

submero
posted this
09 October 2018

thank you Peter

but i have error

i make face sizing by t/4 = 0.5mm

step

10

10

100

submero
posted this
09 October 2018

i want to attach the wbpj file to fix this problem

but i can't

"file extension not allowed"

peteroznewman
posted this
09 October 2018
- Last edited 09 October 2018

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
09 October 2018

what about error ?

I'm so sorry for my repeated questions

peteroznewman
posted this
09 October 2018
- Last edited 09 October 2018

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
11 October 2018

thank you for your replay and your help

but still error exist

i will attach the file please help me

peteroznewman
posted this
12 October 2018
- Last edited 12 October 2018

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
12 October 2018
- Last edited 12 October 2018

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.

peteroznewman
posted this
12 October 2018

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
16 October 2018

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
16 October 2018
- Last edited 16 October 2018

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

peteroznewman
posted this
17 October 2018
- Last edited 17 October 2018

Hello submero,

You have a nonlinear model with Bolt Pretension in step 1 and a tension force in step 2. The bolts are clamping two parts together that have frictional contact. The clamp force is a normal force that is multiplied by the coefficient of friction to calculate a limiting shear force can be supported by the frictional clamped joint.

In step 2, when the applied force reaches the limiting shear force, the joint suddenly slips. The solver is gradually incrementing the applied force and finds a static equilibrium as long as the applied force is less than the limiting shear force. There is no static equilibrium beyond the limiting shear force, so the solver stops.

If the model was changed from applied force to applied displacement, the displacement would be able to slip the joint and keep going.

If the purpose of this model was to find the applied force when the joint slips, then it has done its job. If the purpose of this model is to know the stress in the assembly at the applied load, then the model should be reconfigured to achieve this. The current model has shown that the joint will slip before the full load is applied. After a joint slips, the side of the hole in the parts comes to bear on the shaft of bolts clamping them. However, **this model does not have a contact between the side of the hole and the bolt shaft.**

Even if that contact is added, a model with an applied force can fail to converge on the way to the full load. The reason is a significant distance between the initial location of the beam in the model and the slipped location of the beam. The solver is not able to jump that distance using an applied load, however it may be able to using an applied displacement.

In the Geometry editor, you can locate the beam in the slipped location at the start of the solution. That means the two holes of the two parts are tangent to opposite sides of the bolt shaft (shank) in the direction that advances the beam in the Y direction. That way, there is no sudden displacement as the limiting shear force is reached. *I strongly recommend you relocate the parts to achieve this configuration.*

As I look at the size of the holes and the size of the bolt head and nut, there is very little overlap. I wonder where is the washer?

Regards,

Peter

- rwoolhou 51
- abenhadj 49
- peteroznewman 26
- Abubaker 20
- tsiriaks 13
- jj77 10
- Abhi1311 8
- Astro45 5
- btingthewind 5
- seeta gunti 5

- 1 Need to help with dimension and changes, since it seems I am not able to do diff. in SpaceClaim 19.2
- 2 Ansys 19.2 student version installation problem
- 3 Wrong results for lift force every simulation
- 4 Installing the new version of License Manager
- 5 Another Work bench only opening a grey window [RESOLVED]

John2153 is a new member in the forum

umang is a new member in the forum

mohdaliff is a new member in the forum

daveberutu is a new member in the forum

Mdijo is a new member in the forum