Too many attempts made for this increment

[EmilyHCH]

Hello!

Trying to model compression tube fittings but keep coming across the error of "too many attempts made for this increment" Our load is a uniform load applied to the surface as pictured in the attached file at about 4600 lbs. We've already looked at comments to try to fix this by changing increment sizing, applying a smaller load, making sure our materials are correct, etc. We've made everything a rigid body except for the two smaller components only visible by cross section in the assembly named, "rear ferrule" and "front ferrule". We've applied one boundary condition to the "cap" telling it to remain fixed in space. Any help you could provide to get us past this error and to a working model would be greatly appreciated. The .cae and .jnl files are attached.

 

[FEA way]

Boundary conditions and loads have to be applied to reference points of rigid bodies instead of their surfaces. Also there’s no contact definition in your model (only contact property).

When it comes to step settings, use step time = 1 and initial increment size of about 0.01. Enable automatic stabilization.

 

[EmilyHCH]

Thanks for the response! How do we apply the boundary condition to a reference point if we want the force applied to the entire surface? What would be a good contact definition?

 

[FEA way]

You can apply boundary condition to entire face via reference point assigned to kinematic coupling or rigid body constraint. And if you want to keep the whole body rigid then select all its elements for rigid body constraint.

When it comes to contact, you can use contact pairs or general contact. I suggest the latter approach. Just create contact interaction property and assign it to general contact definition. Abaqus will automatically detect contacting faces.

 

[EmilyHCH]

After adding a general contact and running a job it gives the error, "The user parameter is not available for the current license type". Is there a way to go about this error? I also added the load to a reference point on the ourside of the surface I initially wanted to the same job but I'm pretty sure the error is referring to the contact since we've seen this before when we tried it.

 

[FEA way]

This error most likely means that your input file contains a call for user subroutine. These are not available if you use student version of Abaqus.

 

[EmilyHCH]

What kind of load should we use in order to apply to a reference point? We've tried concentrated force. How do we avoid calling for subroutines if we just want to use a general contact condition?

 

[FEA way]

That’s right, you should apply concentrated force to the reference point. Or you can prescribe its displacement.

To set the general contact properly follow these steps:
- in the Interaction module select "Create Interaction Property" and choose "Contact" for Type
- add "Tangential Behavior" and/or "Normal Behavior" from Mechanical group
- select "Create Interaction", switch to Initial step and select "General contact (Standard)"
- in "Global property assignment" pick the contact property that you defined previously (by default it should be called "IntProp-1")

And that’s it. GC algorithm will handle the rest automatically.

 

[EmilyHCH]

We did that previously, we used a penalty global property with friction factor .577. Is that fine or do you think that's where our error is?

 

[FEA way]

That shouldn't cause any problems. Check your input file, maybe something else is set "User-defined".

 

[EmilyHCH]

Here's what we have so far with the added suggestions you made. Still getting the license error and are pretty sure that the only thing user defined we could potentially have is with our materials we added. Could you take a look? Thanks so much for your help!

 

[FEA way]

In the contact property definition you have Tangential Behavior with Friction formulation set to "User-defined". That's what causes the error. You should change it to Penalty.

 

[EmilyHCH]

Okay, now we're back to the too many attempts made even with your initial comments added in.

 

[FEA way]

I've noticed that Encastre BC is still applied directly to the part with rigid body constraint. You should apply it to proper reference point (like you did with force).

If it still doesn't work, enable automatic stabilization in step settings and consider using prescribed displacement instead of force control. What's more, there might be some rigid body motions that cause convergence issues. You may have to get rid of them (using boundary conditions applied to other parts or some form of artificial damping). Explicit solver may be better for this application.

 

[EmilyHCH]

I changed the encastre BC to the reference point but it still gave the too many attempts error. Automatic stabilization I believe was already on in the step settings. We did consider the displacement option under loads however this option in our case isn't ideal since the criteria given to us by our supervisor specifically provided force acting on the face.

What do you mean by rigid body motions? The encastre boundary condition was put on the rigid bodies we don't want to move but the other one rigid body we defined (which has the load on it) is expected to compress the non rigid components into the rigid bodies that don't move.

You suggested getting rod of these possible rigid body motions using boundary conditions, I don't really understand what you mean do you have an example? Thanks!

 

[FEA way]

Each part should be constrained somehow in all directions in the case of static analysis. Either by boundary conditions or by contact. In your model only one part is completly fixed. So the rest relies on contact for stabilization. To see what happens you should perform eigenfrequency extraction (modal) analysis. Just replace contact with tie constraints and remove load for this analysis. Modes at frequency close to zero will indicate any rigid body motions occuring in the model.

 

[EmilyHCH]

Where is the option to run this model/how do you.

Also what kind of boundary conditions or contact should we apply to our two non-rigid parts? I've attached an updated file with the additional fixed rigid body. The third rigid body with the load applied should compress the two non rigid bodies that are only visible by cross section. We thought that the general contact condition we added per your suggestion earlier would define a basic contact condition for all the parts? Is that not the case? Still getting the too many attempts error.

 

[FEA way]

You don't have to apply BCs to these parts but make sure that contact keeps them in position. General contact algorithm should take care of rigid body motions but it may not be enough if some parts are initially separated. You can use output variables such as CSTATUS, COPEN or CPRESS to see whether the contact is established properly or not. Maybe contact pairs with strain-free adjustment will be better option in this case.

If you want to run modal analysis to check for RBM's (which is highly advised) then follow these steps:
- copy the model and open the copy
- replace general static step with Linear Perturbation --> Frequency
- specify the number of eigenfrequencies for extraction (10 should be enough)
- disable general contact and define tie constraints between all parts (Find Contact Pairs tool can help you with that)
- specify density for materials used in the model
- disable concentrated force
- submit the analysis

 

[EmilyHCH]

We just made all the rigid bodies fixed with exception of the rigid that experiences the load which we made fixed in all directions except for the y direction. Because of this should we no longer have a risk of RBM? We also got the file to run with everything defined in this file EXCEPT the load. So now we know the load is the only thing giving us issues when it's added. Can you take a look at our new file and see why the load would possibly be giving us issues? We defined a concentrated load on the rigid body with a force in the negative y direction and we defined a 0 force for U1, U3, UR1, Ur2, and UR3. Thanks!

 

[FEA way]

Deformable bodies can experience rigid body motions too. But properly defined contact should take care of them.

Load control may cause convergence problems in simulations with contact. If you can, use prescribe displacement instead of concentrated force.

I think that you could simplify this model and make use of symmetry. This would not only speed up the analysis but also eliminate some RBM’s.