[Ansys Mechanical] Hide regions with stress concentration

[Staszkinson]

Hello,

I would like to ask about Ansys Mechanical Functions.
Is it possible to hide regions of my structure, where stress concentration (for shell elements) and bending moment concentration (for beam elements) are the highest?
Let's say that I would like to hide some finite elements with the highest values in the results window and adjust scale.

 

[rickfischer51]

Unselect the elements with NSEL,U,P.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[Staszkinson]

Thank you,
Did you mean ESEL command? (according to "elements" word).
I would ask about one more thing.
I don't exactly get formulation from APDL Help: "Item - Label identifying data, see Table 134: ESEL - Valid Item and Component Labels. Some items also require a component label. If Item = PICK (or simply “P”), graphical picking is enabled".

I use Ansys Mechanical but really don't know when should I pick the elements in graphical mode after ESEL/NSEL, U, P command.
How does it works?

 

[rickfischer51]

Yeah, ESEL,S,P. My bad. Yesterday was a bad day.

You can pick elements with a variety of methods. You chose the method based on what you know about the elements, you criterion for picking them, etc.

If you wanted to pick all the elements below the X-Z plane: ESEL,S,CENT,Y,0,-99999

If you wanted to pick all the elements with material number equal 3: ESEL,S,MAT,,3

If you wanted to unselect all the contact elements: ESEL,U,ENAME,,168,178

If you wanted to select all elements with a pressure load of 300 psi applied to it: ESEL,S,SFE,PRES,300

If you wanted to select all CONTA178 elements that are closed and sliding:

ESEL,S,ENAME,,178
ETABLE,STTS,CONT,STAT
ESEL,R,ETAB,STTS,2


Rick Fischer
Principal Engineer
Argonne National Laboratory