Unconnected regions with analytical rigid components

[blckwtr]

I get a warning about unconnected regions in the assembly, but so far I think I have put it all together as it should. There are 4 analytical rigid parts which now are connected to its reference point, and within these 4 components, there are a rubber "seal", which are modeled as a deformable. I have initiated the inetaractions between parts, I have constrained the reference point to the respective analytical rigid part, and also BC'd the reference points with an encastre. Could anyone help me?

 

[Mustaine3]

The warning does not mean, that it is a problem. So if everything works fine and the results look plausible, then you can ignore it.

 

[blckwtr]

Well, the analysis seems to me like it is assembled as it should, but the solution does not converge at all. I get an error that "the solution is not likely to converge", and "solver problem. numerical singularity". I have, as I said, connected the reference points to the analyticla rigids. I have initiated contact with the master surfaces (the analytical rigid). When it complets one step, it also seems like the moveable instance is rotated in-plane, and it does not have support from the elastomer part contained in the volume. I have checked over and over again, but still I can't find anything faulty in the model..

 

[Dave442]

check the .msg file to see whether you problem is an issue with contact convergence, force convergence or displacement convergence. Then look at the nodes associated with the issue and check where they are located in your actual model. This can help identify issues. Also, are there any additional warning/error messages in the .msg file? Does the second step run at all or does it just cut back five times and terminate?

 

[blckwtr]

The force applied at reference point on the moveable instance seems to be the problem, but I have also checked this several times. There seems to be more problems... Can I send you the inp. file?

Teh problem cut back after 5 incomplete iterations...

 

[Dave442]

if you post attach your .inp file here someone might take a look at it

 

[blckwtr]

I think there may be something in the way I have connected the analytical rigid components to the reference point. So far I have constrained the components to the reference point via a rigid body constraint. Then I have, for the static components, used an "encastre" for the reference points. I want to move the moveable component via a predescribed force on the reference point for that component. Is this wrong?

Q:
- can i prescribe a load to a reference point on an analytical rigid on a 2d axisymmetric analysis
- How do I coreectly define BC on reference point on a 2d axi?

 

[Mustaine3]

The problem is, that you don't know what the reason for the missing convergence is. You just assume it is the rigid body.

It sounds like the rigid body definition is correct. Maybe you have no active contact situation when you apply the load, which leads to a singularity and to nonconvergence. Open the .msg file and check what's written in there.

 

[blckwtr]

I have no contact initially... there is a gap around 0.2-0.3 mm which I need to close when applying load. But is it OK to "encastre" the referenco point, and to load it? I assume I load it with load equal to the complete model...

The error messages are as follows;

***WARNING: THERE ARE 5 UNCONNECTED REGIONS IN THE MODEL.

NUMBER OF EQUATIONS = 4292 NUMBER OF FLOATING PT. OPERATIONS = 1.17E+07

USING THE DIRECT SOLVER WITH 8 PROCESSORS

CHECK POINT START OF SOLVER

CHECK POINT END OF SOLVER

ELAPSED USER TIME (SEC) = 0.60000
ELAPSED SYSTEM TIME (SEC) = 0.10000
ELAPSED TOTAL CPU TIME (SEC) = 0.70000
ELAPSED WALLCLOCK TIME (SEC) = 0


***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE
UPPER_AXD-1.1 D.O.F. 2. THIS NODE HAS NO STIFFNESS IN THE
SPECIFIED DIRECTION AND IS NOT COUPLED WITH THE REST OF THE MODEL.


***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE
PACKER-1.71 D.O.F. 2 RATIO = 14.2973E+12 .

ASYNCHRONOUS TRACKING ELEMENT LOOP STARTED

 

[blckwtr]

I tried to close gaps with an additional step, and the analytical rigid body see no contact with the deformable, so here is something worth checking... I have defined the AR components as the master surface and the deformable elastic part as the slave surface with a penalty friction.

 

[Mustaine3]

1. Having a load on a node the is fixed (encastre) makes no sense. The load isn't doing anything then.
2. A gap is a problem when applying a load in a static step. A static solution means equilibrium. What is the opposite force against the load? Nothing. This leads to a singularity and usually nonconvergence.
3. When you have contact penetration and no stress at all, then you should check your contact definition.

 

[blckwtr]

Thanks, I have found the problem now. As you say, it gives no meaning to apply load when a gap need to be filled, so I enclosed it with a movement, then applied the load. Also, I needed to divide the moveable reference point in two, since three steps are involved, one with initial closure of gap, and deactivate it afterwards. Then I needed to hold the rotation and x-direction during all three steps. And I have also forgot to move the BC's to the left when I applied the additiional enclosure step. So everything is working fine now...