problem with modeling plate bending using Ansys

[hask]

I having been having trouble modeling plate bending using Ansys 8.0. I am trying to simmulate what happens to a plate when it is bent in a brake press. I have made a 2D model of a simply supported 3 foot long 2 inch thick plate. The plate is to undergo multiple bends to obtain a 6 inch bend radius. The problem that I am having is that the supports are ten inches apart and the plate will not deflect more than 1/2 inch per bend (if I try to get more than that ansys says the plate is unconstrained and ridged body motion has occured). This 1/2 inch is not enough for me to get a 6 inch bend radius.

The elements that I am trying to use are Plane 82 with the plane stress with thickness option on (the plate is modeled as 6 inches thick). The element size that I am using is 0.2 inch squares.

Does anybody have any idea how to get a larger deflection so that I can obtain a 6 inch bend radius?

 

[TGS4]

PLANE82 would seem to be the wrong element type. If it were me, I'd go with either SHELL93 or model it with SOLID95's. (To better understand my rationale, take a look at the help for PLANE82 and check out what the DOFs are...).

Furthermore, what are you using as your plasticity model? Have you set nlgeom to on?

 

[hask]

I am using nlgeom and plasticity for modeling structural steel. The plasticity is inputed as nonlinear inelastic, rate independent, isotropic hardening plasticity, mises plasticity, multilinear.

I have tried using the Shell93 elements but it seems to take up alot of disk space. The files get extremely large for just one load step (100MB). Is this normal and if not how do I correct it?

 

[TGS4]

Large files for SHELL93 are typical. I suspect that you are referring to the .rst file. The size of that file will be directly proportionate to the number of substeps in the load step. If you are undergoing a large amount of plastic deformation (such as your case), and the even with auto timestepping, I would expect to see a large number of substeps.

On a separate note, I wouldn't consider 100MB to be a large amount of disk space. I regularly (every two to three weeks) fill up a 20GB partition on my HD and need to archive to DVD.

 

[hask]

Thanks for your help this has been giving me problems for a long time. I hope your suggestions fix it.

 

[hask]

I have tried to run the plate with Shell93 elements with the meshing 0.2 inch squares. The plate is 6 inches wide and 30 inches long and 2 inches thick. The simple supports are ten inches apart and I am trying to deflect halfway inbetween the two supports 0.5 inches. The model will not converge and says that some of the elements change in thickness to much for that iteration. I have tried to increase the number of substeps and I have tried to decrease the amount of deflect but the model will still not converge. Any idea how to make the model deflect and still converge.

 

[TGS4]

How are you applying your supports? Are they restraints on the nodes, lines, or areas?

It would also help if you posted your non-linear material properties, because there may be problems there as well.

 

[hask]

The left support is applied to a single node on the plates surface fixing the x and y displacement to 0, and the right support fixes the y displacement to 0.

In ansys to define the supports I go to define loads-apply-structural-displacement-on nodes.

My material properties that I am using are for A36 steel that is at 1100F. It is put in ansys using the mises plasticity multilinear option the values are:
The linear isotropic properties are: EX = 30800
PRXY = 0.288

Multilinear Isotropic Properties are:

Strain Stress

0.000415 10
0.002 15
0.005 18
0.01 20
0.02 23
0.03 24
0.04 25
0.05 25.2
0.06 25.4
0.07 25.6
0.08 25.8

 

[TGS4]

I suspect that the problem that you are seeing is related to your supports being applied to single nodes. What your analysis is demonstrating is something akin to the St. Venant's effect. Try spreading the restraint over several nodes. You may have to increase your mesh density in the vicinity of the support points for this to work.

Good luck!

 

[CESSNA1]

HASK: You should make sure you are within the limits of the software assumptions. If you are looking at bending a plate you are into large deformations, and the plastic range of the material. You will get answers but they may not be correct. most FEA programs assume small deformaitons.

Regards
Dave

 

[hask]

Well what about the fact that I have the large displacement option (on) and I use the inelastic materials option?

Where does it say the limits of ANSYS 8.0?

thankyou for your help.

 

[TGS4]

CESSNA1: hask had already stated that he had large-deformation and non-linear material properties on.

hask: as far as limitations go - check out the help regarding the specific element type.

 

[hask]

TGS4: I still am not able to get the model to work with the increase in the number of supports (could it be that as the strain increases the slope of the stress strain curve decreases, to nearly nothing, and the model when it reaches a certain point will just collapse).

One problem I have in increasing the number of elements is that the file size and run time increase and were I work I am limited on the amount of disk space and run time. Is there anyway that I can increase the speed of the processor without hurting my results.