Calculate Contact Area Using APDL in Workbench 1

[bgrz]

Hi everyone,
using a few examples from forums, I wrote a APDL script for the Workbench (Release 19.1) postprocessor that calculates the area of contact:

SET,LAST !select results from last loadstep
ESEL,R,TYPE,,3 !select contact elements (target elements would be 4, see solver information)
ETABLE,ESTAT,CONT,STAT !store contact status
ESEL,S,ETAB,ESTAT,2,3 !select element in contact (stat=2 sliding,stat=3 sticking)
ETABLE,C_AREA,VOLU !select contact element area (volume is calculated for unite thickness for 2D elements)
SSUM !sum area
*GET,T_AREA,SSUM,0,ITEM,C_AREA !store result in parameter
MY_AREA_1=T_AREA !print area as result

This works fine, BUT if I use symmetric contact definition the calculated area is doubled, because ANSYS finds contact elements on both contacting bodies.
Does anyone have an idea how to make the script convenient for both symmetric or asymmetric contact? Can I somehow select only the contact elements on one volume?

I am thankful for any advice or tips.

 

[Petr Vymlatil]

Hi,
try to create named selection containing bodies (volumes) on your contact side, you can name it "contact_side".
Then in APDL Comamnd Block you can select the elements via cmsel commad.

Your code will look like this:
SET,LAST !select results from last loadstep
! added code
cmsel,s,contact_side
nsle
esln
! end of added code
ESEL,R,TYPE,,3 !select contact elements (target elements would be 4, see solver information)
ETABLE,ESTAT,CONT,STAT !store contact status
ESEL,S,ETAB,ESTAT,2,3 !select element in contact (stat=2 sliding,stat=3 sticking)
ETABLE,C_AREA,VOLU !select contact element area (volume is calculated for unite thickness for 2D elements)
SSUM !sum area
*GET,T_AREA,SSUM,0,ITEM,C_AREA !store result in parameter
MY_AREA_1=T_AREA !print area as result

This should work. After command ESEL,R,TYPE,,3 only one side will be reselected.


Petr Vymlatil (

http://www.designtec.info)

 

[bgrz]

Hi Petr,
I tried your addition to the code, it works beautifully.
Thanks a lot!

 

[struclearner]

When we give the command of SSUM, !Sum Area, the summation is done for the Contact Area of the Contact Elements based upon the Contact Status of Sliding and Sticking of the Contact and for the Element Table created for the Contact Status, what the SSUM for the Contact Status represents and how it is calculated?
For the static analysis, where the analysis is started at the contact closed state for the computational efficiency, what the contact sliding represents, and why that sliding occurs, is this due to insufficient friction force, not making the forces sum equal to zero.
Thanks for the input.