Non linear incompressible elastic analysis

[men0wjv]

Hello all,

Someone in our department decided to change all our machines to run Ansys instead of Abacus. This isn't really a problem in itself, however all our experts don't have any knowledge of the new package and rather stupidly our extensive library is missing the manual. I've been bashing my head against a brick wall for some time now and with the deadline looming I'm in desperate need of help.
The problem is a bit difficult to go through on this board, so I'll point to "VM201: Rubber Cylinder Presses Between Two Plates" which can be found in the help. Could someone go through how they applied a series of step displacements and how they got Ansys to produce the Force vs Displacement graph?

Very Grateful regards

Will

 

[hwong]

Did you look at the VM201.DAT file and look at the simulation code? It will provide steps to the 3D modeling, material modeling and such.

 

[men0wjv]

Cheers, that's the best suggestion I've heard so far. The dat file certainly looks very useful although a little cryptic; my fea skills are not the best. Anyway I'll see what I get and I'm sure I'll be back soon Thank-you for your reply

Regards

Will

 

[men0wjv]

Ok You can find it at the following address, should you not have an ansys machine available.

http://dmt

http://www.epfl.ch/ims/micsys/ANSYS/verif/vm201.dat

could you explain whatthe purpose of coupling the top edge in the UY direction was and
/POST26
/AXLAB,Y,FORCE ! Label Y
/AXLAB,X,DISPLACEMENT ! Label X
NSOL,2,NCEN,U,Y
RFORCE,3,NCEN,F,Y
PROD,2,2,,,,,,-2
PROD,3,3,,,,,,-2
XVAR,2
PLVAR,3 ! PLOT DISPLACEMENT VS FORCE
PRVAR,2,3 ! PRINT DISPLACEMENT, FORCE
what this means? I have a rough idea but it keeps going wrong

 

[juzz]

Hello, men0wjv!

I hope this could be useful for you:

1) The model represent 1/4 from entire section
That means the top edge is axe of symmetry and will be over entire process. Applying displacement on this edge (which simulates the displacement applied on top of the cylinder) will preserve the symmetry so this is the reason to couple all nodes from that edge on y direction.

2) About the commands listed:

/POST26
--> start time-history post-processor
/AXLAB,Y,FORCE ! Label Y
--> establish the label for Y axis in graphs as "FORCE"
/AXLAB,X,DISPLACEMENT ! Label X
--> establish the label for X axis in graphs
as "DISPLACEMENT"
NSOL,2,NCEN,U,Y
--> store in variable no. 2 the Y displacement of ncen
node (ncen node is the node at the intersection of
symmetry axes - see the command
*get,ncen,node,,num,min from vm201.dat file)
RFORCE,3,NCEN,F,Y
--> store the reaction force on Y in the same node in
the variable no. 3
PROD,2,2,,,,,,-2
--> in fact the displacement that will be used in graph
is the difference between vertical diameter before
and after the deformation
PROD,3,3,,,,,,-2
--> from symmetry condition about XZ plane the real
value of reaction will be twice than that
calculated and is used in absolute value
XVAR,2
--> establish that the plot will be f(variable no. 2)
(the time history post-processor use the TIME
(stored by start in variable no. 1) as default
variable of every function stored in variables from
2 up).
PLVAR,3 ! PLOT DISPLACEMENT VS FORCE
--> plot the variable no. 3 versus variable no. 2 it
means "force" versus "displacement"
PRVAR,2,3 ! PRINT DISPLACEMENT, FORCE
--> lists the variable no. 2 and 3

I believe that could be easy understood from ANSYS documentation.

Best regards,

Juzz
----------------------------
Justin Onisoru
Researcher
Romanian Academy,
Institute of Solid Mechanics
----------------------------

 

[men0wjv]

Nice one Juzz, that's pretty useful thank-you very much for taking the time to reply

Grateful Regards

Will

 

[men0wjv]

OK Juzz or anyone else,
I think I can draw the graph with all the relevant, but I don't get a line drawn, which I feel might be attributed to a lack of applied static displacements. I've applied a 4mm displacement at the moment, but want 0 - 4mm applied at 0.5mm increments, any ideas?

Regards

Will

 

[juzz]

Hello, men0wjv!

You are already adviced how to do that. I intended to answer you but I see my mails first and I think now that is pointless.
We are both members of the same group of yahoo (xansys).

Best regards,

Juzz

----------------------------
Justin Onisoru
Researcher
Romanian Academy,
Institute of Solid Mechanics
----------------------------