Jump to content
lambefr

Rubber shell in Radioss

Recommended Posts

Hello, I am trying to model the correct bending stiffness and rebound and damping behavior of a rubber plate.  My plate is meshed with 3mm shells adn 6mm P1 property.  I tried with Mat Law2 and Law69 and in both cases my model "explodes" on the rebound.  See images below and both model files attached.  Any help in figuring out what I'm doing wrong?

 

Thanks!

 

image.thumb.png.b53b461c161db76cb8f6589a9314fde9.png

image.thumb.png.d584be53ef33ede1680039f273a3a076.png

image.thumb.png.844fd558a97f57a314d3defb7ceabf74.png

law69.zip law2.zip

Share this post


Link to post
Share on other sites

Hi,

 

when the shell element size is small compared to thickness it loses validity.

0.jpg

Quote

When h/L is large, shear deformation is at its maximum importance and the user should use solid elements. When h/L is small, transverse shear deformation is not important and thin shell elements are the most effective choice.

https://www.linkedin.com/pulse/shells-vs-solids-finite-element-analysis-quick-review-kuusisto-p-e-

 

Solid elements are more appropriate and the simulations runs fine.

law2_solid_edit_0000.rad

Share this post


Link to post
Share on other sites

Thanks for your input Hyperman.  I was hoping to be able to pull it off with shells but was expecting the large h/L ratio of my elements to be a problem.

 

Spin off question for rubber in Radioss; how can I introduce damping in the material?  As it is 100% elastic with Law2, it just "flaps" around indefinitely, which my real part does not do!

law2_solid_edit.gif.07d044adc6dab2b30bb3a6a8c31b4d61.gif

 

Can damping be introduced "directly" in the material properties with another material law?  Or must it be externel (ex. Rayleigh, DYREL, etc.)?  If external, which is best to use?

 

Keep in mind that I will have many rubber plates like this one moving at relatively high speed (100+km/h) impacting stationnary objects.  I don't want the external damping to affect the overall correctness of the simulation but I need to properly represent the "internal" damping of the rubber.

 

I would have access to a physical test to calibrate the damping of my model.

 

Thanks

Share this post


Link to post
Share on other sites

Glad to help.

 

Damping can not be defined in the material properties (like in Optistruct). Rayleigh damping /DAMP and dynamic relaxation /DYREL/1 can be applied to a group of nodes to avoid damping the whole model. Use the damping type that achieves primarily a better correlation to the experiments and secondarily better computational efficiency.

Share this post


Link to post
Share on other sites

The issue with LAW2 is that it is linear elastic.  For Non-linear elasticity, you can use one of the hyper-elastic materials like LAW42, LAW69, LAW92, or LAW94.   Example "RD-E: 5600 Hyperelastic Material with Curve Input" shows more details about these materials. 

 

To viscous (rate) effects to the material you can use the viscous input in LAW42 or add /VISC/PRONY to the other materials.  However, data for the viscous input is difficult to determine.  So then maybe Hyperman's suggestion of  Rayleigh damping /DAMP would be easier.

 

Thanks,

Andy

Share this post


Link to post
Share on other sites
On 11/2/2019 at 1:01 AM, Hyperman said:

I am solving plate for modal ansly with

 

two sides clamped two sides free

And

 

One sideclamped three sides free

 

How to apply two constraints in a single model

It says specify bc=n ... Which I don't know

 

 

Share this post


Link to post
Share on other sites
  On 11/2/2019 at 1:01 AM, Hyperman said:

I am solving plate for modal ansly with

 

two sides clamped two sides free

And

 

One sideclamped three sides free

 

How to apply two constraints in a single model

It says specify bc=n ... Which I don't know

Share this post


Link to post
Share on other sites

Hi @Sony Dhotre


create a separate load collector for each set of boundary conditions. For example, create a load collector with all DegreesOfFreeedom fixed and a second load collector fixing only translational DOFs.  Create only one load collector if you need to constrain only one set of DOFs.

 

Share this post


Link to post
Share on other sites
3 hours ago, Hyperman said:

Hi @Sony Dhotre


create a separate load collector for each set of boundary conditions. For example, create a load collector with all DegreesOfFreeedom fixed and a second load collector fixing only translational DOFs.  Create only one load collector if you need to constrain only one set of DOFs.

 

 

3 hours ago, Hyperman said:

Hi @Sony Dhotre


create a separate load collector for each set of boundary conditions. For example, create a load collector with all DegreesOfFreeedom fixed and a second load collector fixing only translational DOFs.  Create only one load collector if you need to constrain only one set of DOFs.

 

 

MultiBC.bdf

Share this post


Link to post
Share on other sites

here is the bdf file

i am getting error as

 USER FATAL MESSAGE 9073 (SUBDMAP PHASE0)
 MULTIPLE BOUNDARY CONDITIONS IN NORMAL MODES ANALYSIS REQUIRES THE BC=N COMMAND IN EACH RESIDUAL STRUCTURE SUBCASE.

Share this post


Link to post
Share on other sites

The solver deck you shared is a Nastran bdf file and that error was reported by a Nastran solver. Nastran issues should be posted on Nastran forums (this is Altair forum). 

 

Optistruct can import bdf files and I was I able to run your model without issues- see attachments.

multiBC.out multiBC.pch multiBC.h3d multiBC.fem multiBC.hm multiBC.op2

Share this post


Link to post
Share on other sites

sir also i want to apply simply supported boundary conditions for plate on all four sides.

 

plate will have only rotation not translation on all the edges is it correct, if not correct me.

 

 

thanking you 

 

 

Share this post


Link to post
Share on other sites

Good Morning Sir,

by accepting your advice, i want to convey to you that.

i am getting some different results than expected.  

 

as I am executing a model referring a paper.

the material for face and core is aluminum.

 

i am using MAT1 for face and MAT9 for core.

                   PSHELL                    PSOLID

 

i am suppose to get the frequency 20<=  f  <=  30  in Hz

i am getting 1.36Hz for 25 element size

                       0.7809 hz for 20 element size

 

 

Geometric Details

A             =1828.8mm

B             =1219.2mm

Tc            =6.35mm

Tf            =0.4064mm

a/b         =1.5

                                                Material Properties

Face Aluminum                                                                                 Aluminum Core

E=           68.94 GPa                                                            G23         =             51.71 e-3  GPa

 G=          25.92 GPa                                                            G13          =            134.45 e-3 GPa

V=          0.33                                                                       

P=           3.05E-09 tn/mm3                                                                p             =             1.34 e-10  tn/mm3

                                                                                                                             121.8318  kg/m3

                                               

                                                  Cards Used

MAT 1                                                                                                   MAT9

PSHELL                                                                                                  PSOLID

SSS         Boundary Condition

 

 

correct me if anything is wrong

 

thank you sir

287ssss44directdensity20mmelement.bdf 287ssss44directdensity25mmelement1.bdf

Share this post


Link to post
Share on other sites

There is an issue with the material property matrix (Gij)- it fails the material check:

 

Quote

*** ERROR # 1551 ***
 for material id = 1 referenced from property id = 1.
 Material coefficients Gij on MAT9 card produce material matrix with negative eigenvalues. This violates material stability conditions.
 Eigenvalues of G: -1.440511e+02 1.956294e-15 1.440511e+02
                   0.000000e+00 0.000000e+00 0.000000e+00

 

If the material check is disabled (PARAM>CHECKMAT>NO) I get the same results. 

Material Property Checks for MAT9.pdf MAT9.pdf

Share this post


Link to post
Share on other sites

Good Evening sir,

 

i really thank you for the support that i am having from you. it means a lot.

 

i want to get clarity, is this the problem of material property value input G13 , G23 ......or else.

 

i don't find any checkmat in hypermesh v9.0   as i am using in conjunction with nastran.

 

 

thank you sir

 

Share this post


Link to post
Share on other sites

Glad to help. You can show appreciation by liking the content.

 

Yes, the issue is with the G13 , G23 parameters. Are you sure you are not confusing the material property matrix parameters (Gij) with the shear modulus? If material data is specified with the Engineering Constants E1, E2, E3, NU12, NU13, NU23, G12, G23, and G13, then use the MAT9OR data.

 

Analysis>control cards>PARAM>CHECKMAT>NO, but it is possible CHECKMAT is not supported in HM 9.0. It will not solve your problem as mentioned before.

Sony Dhotre likes this

Share this post


Link to post
Share on other sites

yes sir i got it,

its there in hmv9.0 also.

i tried but its giving different results.

 

 

There is an issue with the material property matrix (Gij)- it fails the material check:

 

  Quote

*** ERROR # 1551 ***
 for material id = 1 referenced from property id = 1.
 Material coefficients Gij on MAT9 card produce material matrix with negative eigenvalues. This violates material stability conditions.
 Eigenvalues of G: -1.440511e+02 1.956294e-15 1.440511e+02
                   0.000000e+00 0.000000e+00 0.000000e+00

 

Quote

If the material check is disabled (PARAM>CHECKMAT>NO) I get the same results.

 

 

can you send me the results

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.


×
×
  • Create New...