Learning Forum

[tumulpurwar]

Hi peter

Below is door assembly made of woven Carbon fiber material, when i apply fixed constarid over Solid meshed body,i see RIGID BODY MOTION in modal analysis.

Can you please suggest, what to do , have checked grounding procedure also, i feel its grounding problem, how should i solve.

FYI: In static structural, Weak Spring alraedy on

 

Figure-1 , showing fixed constraint

 

Figure-2 Modal analysis, with 2 zero HZ frequency

[mjmiddle]

You can make deformation results of the first 2 modes, and play the animation to see how the rigid parts are moving away from the rest of the model.

The 3rd mode frequency is pretty small too. Check that too.

I noticed hinges on this model. If you have used frictionless contacts or revolute joints, it allows the door to swing open in rigid body motion. If this modal analysis is just a check for rigid body motion but you intend to use a static structural analysis, then consider frictional contacts in the hinge pivots if there is force against the hinges to cause friction or consider another means to hold the door.

[tumulpurwar]

Hi @mjmiddle

I have used Frictional contact for hinges, i am just doing static analysis, i am not trying revolute joint.

As with photo attached in last post of modal analysis, you can see complete assembly is moving, and shows zero frequency for first two modes.

I want to know, it means my body is not fixed in relation with ground.

Thus instead of using Fixed Constraint, i should use Fixed Joint constraint, Am i correct in understanding?

 

[tumulpurwar]

Hi @mjmiddle

I am unable to get convergence for above model for static stress analysis, So i simplified model, model is below:

The Force applied on top face of Silicone rubber, as can be seen with red color in photo, purple color is Fixed boundary condition.

The rubber is sitting inside grooved cut area of door.Door is Carbon fiber composite material

Frictional contact applied (plaease see 2nd photo in exploded view).

It taking so much time to run, its just ever running, what to do.

Note: For rubber non linear adaptive mesh technique i applied with tetra element

[mjmiddle]

The fixed support must hold down the body it is set on at least. I would not trust the result from the modal analysis it if shows all bodies moving, and you should diagnose by other means. Do both of the zero modes show the same behavior?

I am confused about the simplified model. It seems to show 2 bodies, but you have frictional contact set up on what looks to be all surfaces of one body where there are no other bodies contacting. Are the other bodies just hidden? Or are they suppressed?

Are there any substeps converged? If even one substep is converged you can view a deformation result to see what is happening. You may be able to get a converged substep by specifying a very small initial time step, and then view its behavior. Also, set some nonzero value for newton raphson residuals, and view the problem locations.

I do not know the mesh sizes you have used but you may need to set some smaller mesh sizes.

The noninear adaptive region can be tricky to use and will make convergence problematic if not understood and applied well. Try it without the adaptive region first. You may get some converged substeps and you can view the model behavior at a time far before your end time. You can make sute the model is behaving properly for a time before the deformation gets too large, causing high element distortion error and requiring a remesh.

For the nonlinear adpative region, you need a body with enough bulk volume.  Thin bodies may not allow enough room to refine the mesh. Your model looks to have thin bodies. Have it remesh early and often, before the body gets too deformed, or else it may not remesh with an acceptable quality. The purpose of nonlinear adaptive region is to repair a distorted mesh in order to overcome convergence problems caused by the distortion. It is effective only when the mesh distortion is caused by a large, nonuniform deformation. Nonlinear adaptive region cannot help if divergence occurs for any other reason such as unstable material, unstable structures, or numerical instabilities.

Check to see if your hyperelastic material properties are a cause of the problem. Choose a simpler material model to see if convergence is easy and the model behaves correctly. You could try the neoprene rubber material from the hyperelastic materials library.

Also, consider taking a section cut through the model and creating surfaces to analyze in 2D first. Rubber gaskets with high deformation can be very difficult models to get to converge and behave correctly. Make sure you know how to get it to run and behave reasonably in a 2D model first. 2D models have a quick turnaround time to run and make changes for another run. Symmetric contacts work better in these kind of analyses. You can lower the normal stiffness factor, and choose an option for the update stiffness frequency, such as update each iteration, or the agressive setting.

[tumulpurwar]

Question:Do both of the zero modes show the same behavior?

Answer: Both zero mode shows complete assembly moving , one moving in x direction, other moving in diagonal of y and x axis.

 

Question: I am confused about the simplified model. It seems to show 2 bodies, but you have frictional contact set up on what looks to be all surfaces of one body where there are no other bodies contacting. Are the other bodies just hidden? Or are they suppressed?

 

Answer: Here are the contacts with images below:

1) 

 

2)

3)

Question:Are there any substeps converged? If even one substep is converged you can view a deformation result to see what is happening. You may be able to get a converged substep by specifying a very small initial time step, and then view its behavior. Also, set some nonzero value for newton raphson residuals, and view the problem locations.

 

Answer:

I let that simplified geometry to run over night, now in morning i got some results, offcourse it didnt converged complete, but it is taking quite a long time, i am using 4 core distributed .

[tumulpurwar]

 

Question:I do not know the mesh sizes you have used but you may need to set some smaller mesh sizes.

 

Answer:  Silicone Rubber: Currently 8 mm global size, Linear, Non linear mechanical

Door : 8 mm global mesh size, element order: Linear, Non linear mechanical

 

I have used earlier upto 1 mm global mesh size, but it still never converged, so now for fats running, i increased to 8 mm

 

[tumulpurwar]

Question :The noninear adaptive region can be tricky to use and will make convergence problematic if not understood and applied well. Try it without the adaptive region first. You may get some converged substeps and you can view the model behavior at a time far before your end time. You can make sute the model is behaving properly for a time before the deformation gets too large, causing high element distortion error and requiring a remesh.

Answer: I agree on this, but when i was not using Adaptive grid refinement,it ever gave Identify Element Violation every time i ran mesh for more and more finer mesh, thus i got tired and switched to Adaptive grid refinement.

 

Offcourse my door geometry is taken from online free CAD models avaialble on internet, and thats why i think i should had bit simplified the more before running it for simulation, but now as skiped that part and directly jumped to do simulation, i dont know how to move forward, i cannot ever refine mesh below 1 mm, it will tan run for several days, as i have only 4 core license. Tell me what to do?Also let me know,whether my time step is correct or should go with other values?

 

[tumulpurwar]

Question: 

For the nonlinear adpative region, you need a body with enough bulk volume.  Thin bodies may not allow enough room to refine the mesh. Your model looks to have thin bodies. Have it remesh early and often, before the body gets too deformed, or else it may not remesh with an acceptable quality. The purpose of nonlinear adaptive region is to repair a distorted mesh in order to overcome convergence problems caused by the distortion. It is effective only when the mesh distortion is caused by a large, nonuniform deformation. Nonlinear adaptive region cannot help if divergence occurs for any other reason such as unstable material, unstable structures, or numerical instabilities.

Check to see if your hyperelastic material properties are a cause of the problem. Choose a simpler material model to see if convergence is easy and the model behaves correctly. You could try the neoprene rubber material from the hyperelastic materials library.

 

Answer: Silicone rubber have high bulk modulus and as i am using non linear adaptive meshing only for Rubber, so i think this should not be a problem.

As earlier when i was not using non linear adaption mesh for rubber, i was ever getting, elements in "identify element violations",so thus got tired and switched to "nonlinear adpative region" for rubber.

I have checked cvomplete door aseembly when i assumed rubber as steel,it had no problem in simulation, but as soon as i convert to rubber or can say hyperelastic material, it ever run, and never converge completely, even for simplified model of real assembly its not converging(which hardly contain 2 structural items, one is rubber other is door.

`

[tumulpurwar]

Dear 

 

If you see photo below on true scale, it shows uncoverged maximum deformation point of rubber, but if you see second photo, a side view of deformation contour, it shows rubber coming out of composite door, how it is possible? it in non physical? what do you say?

[tumulpurwar]

FYI

 just reiterating gain ,For simplified model, force applied was and boundary condition was

[tumulpurwar]

[mjmiddle]

This is getting too involved for a forum post. You should submit a service request and attach the archive of your workbench model.

I will only add a few more points, some of which are reiterating what I said previously:

1. Using linear tetra elements is definitely a problem. Set to quadratic.
2. There is also a message stating that the nonlinear adpative region will not apply because it needs to be scoped to a region with quadratic tetrahedral elements. So switching to midside node elements will allow the adaptive region to work. However, as I stated previous, see if you can get some substeps converged first to see how the model is behaving before using an adaptive region. The model has to behave as expected before you can reasonably apply the adaptive region for later substeps that have too much defrormation to use the original mesh. 
3. The unconverged solutuon is not reliable. It's usually just junk, so don't take anything from that. Don't try to look at the end time 1 sec. Did it even get one substep converged that you can look at?
4. Restatement: Your substeps are definitley not enough for a problematic model. As I said in my previous message set a small initial time step as this may get a initial time step to converge and you can view that result to see what's happening. Try 1000 initial substeps, 100 min, and a max of 1e5. If that can't converge the substep, try even more initial substeps. The model would probably take a long time to solve a few substeps and never make it to the end since it's not behaving right. But even if the model is not behaving right you can interrupt the solution after you get a converged substep and then look at a result to see what's happening. Or if it can't converge that 1st substep, you can quickly abort and change something in the setup, instead of waiting all night just to see that no substeps converged.
5. Restatement: I can not state this enough: large deformation gasket models (hyperelastic materials) may look simple but can be decievably hard to work with. For this reason, you should take a section cut and analyze as 2D model first. Get that to run the full time so that you can understand how the rubber is deforming, and this will help you set up the 3D model if still needed. Many times, you can undestand what you need just from this 2D model, and this will run faster and save you a lot of time.
6. Some of your contacts appear to have some of the same geometry selections. This may confuse it a bit. Make sure your face selections are unique for each contact. Also, I see you have a frictional contact with zero coefficient. Try setting this to frictionless.
7. Restatement: Symmetric contacts work better in these kind of analyses. To help convergence, you can also lower the normal stiffness factor, and choose an option for the update stiffness frequency, such as update each iteration, or the agressive setting.

Beyond these suggestions, this is getting too complex for a forum post. You should submit a service request with your model if you need further help. We cannot transfer files through forum posts.