## General Mechanical

#### Workbench Transient Analysis using Beam model

• byungchun
Subscriber

Hello,

1. I have made 2 sets of beam model using workbench for imposing transient loads.

2. How can I use gap element in workbench. Beam element seems not to be proper element for applying gap(contact element)

Actually I want to have gap element at each elevation.(see attached figure)

3. Is there any easy way to apply fixed joint at once at all each point?

In case of having many connection point..

I used user define when generating beam model

• jj77
Subscriber

I assume you refer to GAP as CGAP from nastran, which are old tech. point to point contacts (are ok to be used fro civil appl. like you show, but not for general contacts, e.g., large sliding).

The equivalent in ansys is a legacy element that is called contac12 (node to node contact). Never really used it. If you can use it then use it in apdl, not sure how to use it in wb.

Below is a small example to show how it works. Two beams are left and right (with an offset in height Y) and connected at their free tips with a contact element, thus when the top beam is pushed down it will contact and push the other one down (if force is reversed nothing happens as expected). The contact properties are defined via real constant (R command) - the first one is the number, the second some angle (contact surface), third the normal contact stiffness,... Look up contac12 and you will see what they all mean.

Good luck

/prep7

L1x1=0

L1x2=1

L2x1=1

L2x2=2

ET,1,BEAM188

KEYOPT,1,3,3

ET,2,CONTAC12

MPTEMP,,,,,,,,

MPTEMP,1,0

MPDATA,DENS,1,,7800

MPTEMP,,,,,,,,

MPTEMP,1,0

MPDATA,EX,1,,200E9

MPDATA,PRXY,1,,0.3

SECTYPE,   1, BEAM, RECT, , 0

SECOFFSET, CENT

SECDATA,0.1,0.1,0,0,0,0,0,0,0,0,0,0

R,1,0,1E9,0,0,1E5,0.5 ! Point contact element definition via real constants

N,1,L1x1,0,0

N,2,L1x2,0,0

N,3,L2x1,0.1,0

N,4,L2x2,0.1,0

TYPE,1

E,1,2

E,3,4

TYPE,2

REAL,1

E,2,3

/SOLU

ANTYPE,0

D,1, ,0, , , ,ALL, , , , ,

D,4, ,0, , , ,ALL, , , , ,

F,3,FY,-100

SOLVE