Penetration problem

  • 220 Views
  • Last Post 4 weeks ago
Junaid.Dand posted this 4 weeks ago

Hi everyone, 

Can anyone help me out with the penetration problem as shown in the image.

Thank you

 

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 4 weeks ago

Hi Junaid,

Maybe the contact definition needs a much larger Pinball Radius. That is a parameter in the Contact definition that you can change.

If you create a Workbench Project Archive .wbpz file and attach it to your post, it will be easy to show you what changes are needed to your model.

 

Regards,

Peter

  • Liked by
  • Junaid.Dand
Junaid.Dand posted this 4 weeks ago

Hi Peter,

Thanks for the reply. File size is too large, more than 120MB so cant attach to the post.

Is there any other way I can share the file?

Thank you

 

SandeepMedikonda posted this 4 weeks ago

Junaid,

Can you put snapshots of what contact settings you are using?

Any discussion/recommendations in this thread would help others facing similar problems in the future.

Also, check out the recommendations in these documents (1 & 2).

~Sandeep

  • Liked by
  • Junaid.Dand
peteroznewman posted this 4 weeks ago

Junaid,

If you click on Model and Clear Generated Data, that will clear the mesh and result in a smaller file size. After you save and archive, if that is still > 120 MB, then the other option is to put a link to your Google Drive.  If you tried to mail that file as an attachment to someone, Gmail would put it on your Google Drive and just put the link in the email.  You can paste that link into your response.

As Sandeep says, if you show the details window and the graphics window of the contact definition, we might be able to see what is wrong.

Regards,

Peter

 

  • Liked by
  • Junaid.Dand
Junaid.Dand posted this 4 weeks ago

Hi Peter,

As u suggested earlier, Please check the attached model file.

Looking forward to hearing from you.

Thank you

Regards

Junaid Dand

Junaid.Dand posted this 4 weeks ago

Hi Sandeep,

Thank you for your reply. Please check the attached model file.

Looking forward to hearing from you.

Thank you

Regards

Junaid Dand

SandeepMedikonda posted this 4 weeks ago

Junaid, 

Try the following:

  • Change the Normal stiffness from program controlled and use a factor of 5 or 10 even. If needed, change update stiffness to Each iteration.
  • Change the formulation from Augmented-Lagrange to Normal-Lagrange. This will eliminate nearly any penetration, but make sure that you are using the direct solver in the analysis settings.
  • Lastly, as Peter suggested, use a higher pinball radius by changing it from program controlled to manual and make sure that the contact regions are being properly closed by the blue transparent guide ball that shows up.

~Sandeep

 

  • Liked by
  • Junaid.Dand
peteroznewman posted this 4 weeks ago

Junaid,

In addition to Suneep's suggestions, one that may be the major cause of the failure is Trim Contact.  Turn it Off.

It is also very important to turn Large Deflection On.

I am running your model now with just Trim Contact turned off and a large Pinball Radius to see if that makes a big improvement.

I noticed that you had left Auto Time Stepping as Program Controlled.  Under Program Control, it automatically selected 5 substeps, but had two bisections before it initially converged. By changing to On and setting Initial Substeps to 20, it was able to achieve the first converged substep without bisections.

You have a Displacement 2 Boundary condition, but it has all 20 faces of the beam set to Z = 0.  That is not a correct way to constrain a beam. Yes, you need a Z = 0 constraint somewhere, but the best place of that would be to put a plane down the center of the beam and slice the model into a half model and put the Z = 0 as the Symmetry Boundary Condition.  When Z = 0 on opposite faces of the body that is experiencing tension and compression stresses along the X axis, the material wants to expand or contract in the Z direction due to the Poisson's ratio, and the constraints on both sides prevent that form happening. 

I changed to to just one set of faces in a Symmetry type of Boundary Condition, so the model is now representing a beam twice as wide.

Regards,

Peter

  • Liked by
  • Junaid.Dand
Junaid.Dand posted this 4 weeks ago

Mr Peter,

Thank you for spending your precious time and running the model.  

Is the penetration problem over when you made these changes in the model?

Thank You

Regards

Junaid Dand

peteroznewman posted this 4 weeks ago

Junaid,

I will repeat what I was adding to my note above in case you missed it, since your reply was already there when I was done editing: It is very important to turn Large Deflection On.

As I look more closely at your model, I see a Metal Strap that has two Steel "end blocks" and between them is a Beech wood block. You have used Bonded contact between the Beech wood block and the Metal Strap and the "end blocks" but it seems to me that the Beech wood block is placed into this steel assembly with no bonding between the faces.  I expect the Metal Strap is in fact bonded to the "end blocks". Is that correct?  If so, then there should be frictional contact between all the Beech wood parts and the steel parts.  Am I right?

Regards,

Peter

peteroznewman posted this 4 weeks ago

Junaid,

Thank you for the photograph, that confirms my assumption. There should only be frictional contact between the steel and the wood. That is what I have done in the attached model.

A better way to connect the steel end blocks to the steel strap is to put those three bodies into the same part in DesignModeler. That way there is no bonded contact required between those three bodies, they will be meshed and share common nodes at the coincident faces.

In the attached model, I created a multibody part for the steel parts. I also sliced the geometry into a half model and used a z = 0 constraint on the cut face.

I added planes and made slices to get a higher density of nodes over the contacts on the bottom supports.

The attached ANSYS 18.2 archive has run for a displacement of 6 mm and will run overnight to see how far toward the 46 mm final value it can get.

Regards,

Peter

Adisa posted this 4 weeks ago

Peter or anybody,  whether in this case can  use  the mesh nonlinear adaptivity  for the mesh control? And how much the results are accurate using the mesh nonlinear.

 

peteroznewman posted this 4 weeks ago

I added another slice to make it a quarter model instead of a half model. This makes the solution run faster, but the biggest benefit is it adds an X=0 constraint to the model, which was lacking in the half model. The half model only had X = 0 constraint once friction was established, making convergence difficult. Now getting started is much easier. Now the challenge will be getting to large values of displacement.

Below it is apparent that the thick steel plate shown in the photograph above that is not included in the model serves a necessary purpose.

Adisa, a large amount of plasticity can be accomodated without needing to turn on Mesh nonlinear adaptivity.

The attached ANSYS 18.2 archive had all steel parts, and no plasticity. See the next post for rev1.

Attached Files

Junaid.Dand posted this 4 weeks ago

Mr Peter,

Thank you for the attached file.

I am running the previous model now with the half model.

Thank you

Regards

Junaid Dand

peteroznewman posted this 4 weeks ago

Junaid, the half model has problems. Look at the quarter model attached here, which has the wood property with plasticity assigned to the block.  The image above is for a steel block without plasticity.  When slicing material in DesignModeler, previously assigned materials get replaced with Structural Steel, because it is assigned as a Default material. That leads to mistakes such as the one above, where I ran with the wrong material. There is a way to remove the Default material so that when slicing is done, the model gets a ? that demands correction, rather than a silent replacement of one material for another.  It is however a good practice to get a model to converge without plasticity before adding plasticity.

Here is how far that same model got with plasticity turned on before convergence failed after 205 iterations.

 *** WARNING ***                         CP =     774.670   TIME= 06:50:22
 Plasticity algorithm did not converge for element number 800 with      
 material number 7.                                                      

Regards,

Peter

Attached Files

  • Liked by
  • Junaid.Dand
Junaid.Dand posted this 4 weeks ago

Mr Peter,

Thank you for correcting the model, I will add the missing plates in the quarter model and will try to run it.

Thank You

Regards

Junaid Dand

peteroznewman posted this 4 weeks ago

Junaid, the missing plates are not the problem. Plasticity convergence issues are the problem. See above.

There may be a problem having Bilinear Isotropic Hardening with an Orthotropic material.

Try Bilinear Kinematic Hardening instead.  Or try an Isotropic Elasticity instead.

Regards,

Peter

  • Liked by
  • Junaid.Dand
Junaid.Dand posted this 4 weeks ago

Mr Peter, 

I am running the model with Bilinear Kinematic Hardening now.

Thank You

Regards

Junaid Dand

peteroznewman posted this 4 weeks ago

Junaid, that didn't get any further, but it stopped because it could not converge, not due to a Plasticity.  I used the NEQIT,50 command, and it looks like if I had given it a higher number, it would have converged, but it stopped at the 50 iterations mark. Bump that number up to 100.

Do you know how to Restart a solution from the last converged substep?

I looked at the Newton-Raphson Residual Force, and the max value is in the tail. That may require smaller elements to converge.

Regards,

Peter

 

Junaid.Dand posted this 4 weeks ago

Mr Peter 

Same thing happened with my simulation also. Should I increase the number of maximum substeps?

Thank You

Regards

Junaid Dand

 

 

peteroznewman posted this 4 weeks ago

Junaid, try reducing the element size along the tail as shown in the image above, and changing the command snippet from 50 to 100.

Regards,

Peter

SandeepMedikonda posted this 4 weeks ago

Junaid,

Here is a video that illustrates restarting an analysis:

 

Regards,

Sandeep

  • Liked by
  • peteroznewman
Junaid.Dand posted this 4 weeks ago

Mr Peter,

Unfortunately.I don't know how to Restart a solution from the last converged substep?

I will do that as suggested by you.

Thank You

Regards

Junaid Dand

Junaid.Dand posted this 4 weeks ago

Mr Sandeep,

Thank you for sharing the video.

Regards

Junaid Dand

peteroznewman posted this 4 weeks ago

Junaid,

Your original model had the displacement of the cylindrical body onto the flat wood sample defined by selecting all faces of the body. That has the effect of turning the body into rigid body. There won't be any stress or deformation of that body, though I note that it was defined with plasticity.

I continued that practice into the recent models. If you want the center pusher to deform at its tip where it makes contact with the block, you must pick the top flat face instead of the cylindrical face that is currently picked.  That does then expose another set of elements from failing to converge, so you might want to stick with the rigid body effect for a while until you have the flat wood block behaving the way you want.

The model is now at the point where element deformation errors are stopping convergence.

I have created a Named Selection called Element ID to find this element.

If you zoom into that corner of the wooden block, you can see that the Poisson's ratio is causing the wood to expand laterally, and the wood is starting to "fall off" the sharp edge of the cylindrical pusher.  This is going to cause the block element to deform and convergence to fail.  The corrective action is to make the pusher wider than the block so that the wood block doesn't fall off the pusher.  That assumes the pusher is much harder than the block (or rigid) otherwise, the same problem may show up on the pusher.

Actually, the element is on the symmetry side, but this model is missing some faces in the Symmetry Region, so once that is fixed, the problem will just show up on the other side.

At this point, you might consider a 2D plane strain model, since you can get some useful information in much less time and trouble.

Regards,

Peter

Attached Files

  • Liked by
  • Junaid.Dand
peteroznewman posted this 4 weeks ago

The attached model was making good progress when I stopped it.

Attached Files

  • Liked by
  • Junaid.Dand
Junaid.Dand posted this 4 weeks ago

Mr Peter,

Thank you for the attached file. I will run it.

Now I have made the change in the displacement direction as was during the lab test. I have applied displacement on the supports.

Regards

Junaid Dand

peteroznewman posted this 4 weeks ago

Junaid,

Are you saying that instead of moving the top center piece downward, you are moving the bottom side supports upward?  That makes no difference to the simulation.

Why are you not taking advantage of symmetry?  The solver will run for twice as long (or four times as long if you don't run a quarter model).

Update on the post above. The solver hangs at increment 337 as shown in the force-convergence plot above. The first time it ran, I clicked Interrupt Solution to look at the results, but it never stopped.  I restarted that computer and reran that model and the solver appears to still be running, but it got to that same increment and goes no further.  There is no error in the solver output file, and all the ANSYS.exe processes are still showing in the Task Manager, but I believe the solver has hung.  This is a very rare outcome. Let me know if that happens for you also.

Peter

Junaid.Dand posted this 4 weeks ago

Mr Peter,

Yeah, I mean bottom side supports moving upward. In order to avoid any deformation of the elements which caused errors when the symmetry condition was used earlier, I am using full sample along the longitudinal section. Below is the image of the model when it was simulated for 10mm displacement only for checking purpose.

 The same thing happened to me. But there seems no penetration when scaled 5x auto.

Regards

Junaid Dand

Close