Reproducing a compressive test, load control

[MaurizioMilani]

Hi everyone,

I have a "piece of cilynder"-like geometry (something like a wheel) having 2 different material, a central nucleus and surrounding ring. Both are "soft" material

I want to load it superiorly in compression pinning the inferior part. The free faces (superior and inferior) are not perfectly in a plane and below I have 2 different material as I wrote

But I want to reproduce a compressive test, so, have the same displacement for all the superior nodes with a given load, as it happens during the test

I found not worth to use a contact approach, so:

- I created a shell superiorly with very high modulus, and loading one node --> singularity problem

- I tried with *kinematic constrain but I have convergence issues

- *rigid body, tying nodes of the shell seems not work as well

perhaps the shell is not necessary, or perhaps I should thy with a different approach

Any suggestion?

Thanks

[Nicholas Fantuzzi]

Hi Maurizio,
I modeled some contacts with ABQ in a friction case. You can try drawing the
2D plane unlike a rigid body but with a very high elastic modulus. Next you
should apply a uniform load on it (the distributed load must have the same
resultant of compression's component). Of course you have to use another 2D
plane in the lower part as a fix table.

I hope I can help you

Nicholas

p.s.
if you prefer you can write me in private in italian :), and next we can
report here in english


[Non-text portions of this message have been removed]

[Dave Lindeman]

Try using *EQUATION to couple the relevant degree-of-freedom on your
surface, the apply the entire load to the retained DOF.

Regards,

Dave

-------------------------
Dave Lindeman
Lead Research Specialist
3M Company
3M Center 235-3F-08
St. Paul, MN 55144
651-733-6383


MaurizioMilani wrote:

>  
>
>
> Hi everyone,
>
> I have a "piece of cilynder"-like geometry (something like a wheel) having 2
> different material, a central nucleus and surrounding ring. Both are "soft"
> material
>
> I want to load it superiorly in compression pinning the inferior part. The
> free faces (superior and inferior) are not perfectly in a plane and below I
> have 2 different material as I wrote
>
> But I want to reproduce a compressive test, so, have the same displacement
> for all the superior nodes with a given load, as it happens during the test
>
> I found not worth to use a contact approach, so:
>
> - I created a shell superiorly with very high modulus, and loading one node
> --> singularity problem
>
> - I tried with *kinematic constrain but I have convergence issues
>
> - *rigid body, tying nodes of the shell seems not work as well
>
> perhaps the shell is not necessary, or perhaps I should thy with a different
> approach
>
> Any suggestion?
>
> Thanks
>
> --
> View this message in context:
> http://www.nabble.com/Reproducing-a-compressive-test%2C-load-control-tp26110587p26110587.html 
> <http://www.nabble.com/Reproducing-a-compressive-test%2C-load-control-tp26110587p26110587.html>
> Sent from the Abaqus Users mailing list archive at Nabble.com.
>
>

[pine]

sounds like an idea application of kinematic coupling. when you say you have convergence issue, did you constrain the rotation DOF of the reference node in the kinematic coupling. this is typically the problem of convergence.

Hansong

---------
Hansong Huang
Senior Research Engineer
Modeling Group, Saint-Gobain Northboro R&D Center

>
> MaurizioMilani wrote:
> >  
> >
> >
> > Hi everyone,
> >
> > I have a "piece of cilynder"-like geometry (something like a wheel) having 2
> > different material, a central nucleus and surrounding ring. Both are "soft"
> > material
> >
> > I want to load it superiorly in compression pinning the inferior part. The
> > free faces (superior and inferior) are not perfectly in a plane and below I
> > have 2 different material as I wrote
> >
> > But I want to reproduce a compressive test, so, have the same displacement
> > for all the superior nodes with a given load, as it happens during the test
> >
> > I found not worth to use a contact approach, so:
> >
> > - I created a shell superiorly with very high modulus, and loading one node
> > --> singularity problem
> >
> > - I tried with *kinematic constrain but I have convergence issues
> >
> > - *rigid body, tying nodes of the shell seems not work as well
> >
> > perhaps the shell is not necessary, or perhaps I should thy with a different
> > approach
> >
> > Any suggestion?
> >
> > Thanks
> >
> > --
> > View this message in context:
> > http://www.nabble.com/Reproducing-a-compressive-test%2C-load-control-tp26110587p26110587.html 
> > <http://www.nabble.com/Reproducing-a-compressive-test%2C-load-control-tp26110587p26110587.html>
> > Sent from the Abaqus Users mailing list archive at Nabble.com.
> >
> >
>

[MaurizioMilani]

Thank to everybody for the replies

Hansong is right, constraining the rotation DOF of the reference node (both kinematic approach I think and rigid body approach, which is that one I tested) convergence was no more a problem

Finally I solved like this: adding a layer of element (3D, but I think also shell will work) in the top part, defining this new layer as a rigid body, applying the load in the desired direction and constraining all the other DOF (translational and rotational)

The only curious thing i have to remark is that when a rigid body is defined from an element set Abaqus asks for a *solid section (with a correspondant material defined). I didn't understand this, because rigid body is infinitely rigid, namely. Perhaps no matter what material properties you define, it is just a "dummy" section...

Bye, and thanks again

pine wrote:

sounds like an idea application of kinematic coupling. when you say you have convergence issue, did you constrain the rotation DOF of the reference node in the kinematic coupling. this is typically the problem of convergence.

Hansong

---------
Hansong Huang
Senior Research Engineer
Modeling Group, Saint-Gobain Northboro R&D Center


>
> MaurizioMilani wrote:
> >  
> >
> >
> > Hi everyone,
> >
> > I have a "piece of cilynder"-like geometry (something like a wheel) having 2
> > different material, a central nucleus and surrounding ring. Both are "soft"
> > material
> >
> > I want to load it superiorly in compression pinning the inferior part. The
> > free faces (superior and inferior) are not perfectly in a plane and below I
> > have 2 different material as I wrote
> >
> > But I want to reproduce a compressive test, so, have the same displacement
> > for all the superior nodes with a given load, as it happens during the test
> >
> > I found not worth to use a contact approach, so:
> >
> > - I created a shell superiorly with very high modulus, and loading one node
> > --> singularity problem
> >
> > - I tried with *kinematic constrain but I have convergence issues
> >
> > - *rigid body, tying nodes of the shell seems not work as well
> >
> > perhaps the shell is not necessary, or perhaps I should thy with a different
> > approach
> >
> > Any suggestion?
> >
> > Thanks
> >
> > --
> > View this message in context:
> > http://www.nabble.com/Reproducing-a-compressive-test%2C-load-control-tp26110587p26110587.html 
> > <http://www.nabble.com/Reproducing-a-compressive-test%2C-load-control-tp26110587p26110587.html>
> > Sent from the Abaqus Users mailing list archive at Nabble.com.
> >
> >
>