Compression of Hollow Rubber Seal 1

[ConorWalsh]

hello all,

I am new to Abaqus and have used Ansys before but am having a bit of trouble adapting to it.

I am currently attempting to model the compression of a hollow rubber seal that is constained between two rigid surfaces and the upper rigid surface begins in contact with seal and then moves down via a dof constraint to comprerss it.

I wanted to model the rubber as a hyperelastic material by using the coefficeints C10,C01 as 80 and 20 respectively, I am not sure what bthe D coefficeint is for. Can you help.

Also I am unsure what element type to use.

Could someone who has encoutered a problem like this before give me some guidlines on the approach to take.

Thanks in advance

Conor

 

[jkapcoe]

Conor,

I think that you have done a good thing going from Ansys to Abaqus. We made the switch a couple of years ago and I haven't look back since...

As far as your coef. definition goes, it should look something like this:
------------
*SOLID SECTION,ELSET=<YOUR ELSET NAME FOR THE RUBBER ELEMENTS>,MATERIAL=<MATERIAL LABEL>
*MATERIAL,NAME=<MATERIAL LABEL>
*hyperelastic,polynomial,n=1
80.,20.
-----------

For the rigid surfaces you have to make sure that the normal of the surface is pointed in the direction of the contact. If your points for the rigid surface are 0,0 to 0,1 the direction would be up. If it went from 1,0 to 0,0 the direction would be down.

The surface call outs would look like this:
-----------------------------------
*SURFACE, TYPE=SEGMENTS, NAME=<<<RIGID SURFACE NAME>>>>
START, 0.,0.
LINE, 0.,1.
*RIGID BODY, ANALYTICAL SURFACE=<<<RIGID SURFACE NAME>>>, REF NODE=<NODE>
*SURFACE, NAME=<SURFACE NAME FOR RUBBER COMPONENT>
<NAME OF ELEMENT SET OF RUBBER COMPONENT>
*CONTACT PAIR, INTERACTION=<NAME FOR PAIR>
<SURFACE NAME FOR RUBBER COMPONENT>,<RIGID SURFACE NAME>
*SURFACE INTERACTION, NAME=<NAME FOR PAIR>
*FRICTION
<<FRICTION FOR CONTACT>>
.
.
.
------------------------

You would need two surface set callouts. One for the top and one for the bottom contact.

Also note that the rigid surface has to have a node associated with it (this is how you apply the displacement). Just create dummy nodes somewhere in space. Do not forget to constrain these in your boundary declerations (I sometimes forget to constrain the rotation ability of the nodes, which can give wacky results).

The type of element you use is up to you, but for a 2d axisymmetric analysis you could probably use the CAX4H. For 2d plane strain analysis you could use CPE4H. (I try to avoid midside nodes with hyperelasticity).

If you expect self contact you have to define that as well. Abaqus does not see it if you don't tell it.

I hope that helps!

John

 

[DickButkus]

D is the compressibility. Although some books refer to rubber as incompressible, it is about as compressible as water. In reality, rubber is far more compressible than something like steel, but it's shear modulus is so low that the incompressibility is relative.

The bulk modulus for rubber is around 100,000 or 200,000psi. Either of these values will make the problem converge easier, but will most likely, not have any effect on your results. It is very difficult to trap rubber volumetrically so that the bulk modulus will have a big effect on your results.

D is 1/K so 1E-5 would be a realistic value.

Best regards,
KF9RI