Skip to main content

Cyclic symmetry in ABAQUS

Submitted by NoeP on

Normal
0

false
false
false

EN-US
ZH-CN
X-NONE

/* Style Definitions */
table.MsoNormalTable
{mso-style-name:"Table Normal";
mso-tstyle-rowband-size:0;
mso-tstyle-colband-size:0;
mso-style-noshow:yes;
mso-style-priority:99;
mso-style-parent:"";
mso-padding-alt:0in 5.4pt 0in 5.4pt;
mso-para-margin-top:0in;
mso-para-margin-right:0in;
mso-para-margin-bottom:10.0pt;
mso-para-margin-left:0in;
line-height:115%;
mso-pagination:widow-orphan;
font-size:11.0pt;
font-family:"Calibri","sans-serif";
mso-ascii-font-family:Calibri;
mso-ascii-theme-font:minor-latin;
mso-hansi-font-family:Calibri;
mso-hansi-theme-font:minor-latin;
mso-bidi-font-family:"Times New Roman";
mso-bidi-theme-font:minor-bidi;}

____________________________________________________________________________

hi,

I'm trying to set up a cyclic
symmetry model of a bar with a changing radius.

The bar has moments applied at both of its ends in opposite
directions (through reference points which are constrained to the bar's end
surfaces). thus, the model isn't symmetric but cyclic symmetric.

I've created a part that is an 8th of the bar.

Though I've set up the cyclic symmetry interaction, the
results seem to show that the analysis is only done on an 8th of the model and
isn't simulating the whole bar.

I would appreciate any advice on this manner.

Here’s a link to the CAE model - http://files.engineering.com/getfile.aspx?folder=dbc3e55c-6ac0-4b12-9d6d-2ac289b7f2f4&file=Cyclic.cae

thank you,

Noe

Forums
Ask iMechanica
research
Free Tags
ABAQUS
Akumar

The cyclic symmetry means that the two nodes on symmetry face will follow same deformation. This means, if you rotate node 1 by an angle x (symmetry angle), you'll get the node 2.

In your model, you can do it two ways. However both will require you to be careful.

  1. Write equation constraint between symmetric nodes on two face.
  2. Use *MPC -> type Cysmm.

MPC type cysmm is supported only in keyword (no cae). Check abaqus keyword manual or analysis user's manual for this. However, this option will require you to write cysmm for each and every pair of nodes on symmetry planes.

For equation constraint, I would suggest you to do it in input file. Even though you can use node sets for each side of symmetry face, but there is no surity if the nodes will be ordered correctly. Equation constraint will constrain i-th node of node set 1 with i-th node of node set-2 if both of them are of same size (check manual for this more). However, if you create node sets such that i-th entry in each set are symmetric pair then you can use node set safely (that's why I suggested to do it manually). So if this is the case use the following equation:

U2 = T * U1

U1 and U2 are displacement vectors of Set-1 and Set-2, respectively. T is transformation matrix (expression below):

T = [ [C -S 0], [S C 0], [0 0 1] ] ---------3x3 matrix

'C' and 'S' are  cos(x) and sin(x) where x is the angle of rotation measured from set-1 to set-2 counter clockwise.Note that this T-matrix is valid only for your case, since axis of rotation is z-axis in your model.This is same is coordinate transformation .if nodes of your elements have rotational dofs, you can use the same equation to constrain them.

------
The world started with 0, is progressing with 0, but doesn't want 0.

Fri, 08/31/2012 - 17:29 Permalink
Akumar

I looked at your mesh, and something is not right...run mesh verification in mesh module

------
The world started with 0, is progressing with 0, but doesn't want 0.

Fri, 08/31/2012 - 19:41 Permalink
Akumar

any luck??? your mesh aspect ration is screwed up (sorry for this word :P)...always remember, the bad the aspect ratio is, the more the probability of  getting into shear locking phenomena (for continuum elements). Bad aspect ratio would trigger other things as well (obviously not the good ones)

------

The world started with 0, is progressing with 0, but doesn't want 0.

Wed, 09/05/2012 - 03:36 Permalink