## General Mechanical

#### Ploting results with only certain elements – APDL

Subscriber

I'd like to plot stress results of just a bunch of elements let's say of the elements no 10920, 10000, 10080. How can I write an APDL code with just these elements showing stress.

• Sandeep Medikonda
Ansys Employee

Hi, Are you looking for a contour plot or a history x-y plot?

Ansys Employee

Hi,

For this,

1) Create an Elemental Component of these elements using CM command.

2) Select this Elemental Component using CMSEL command.

3) Under /Post1, select last result set.

4) Plot above selected Elements (under elemental component) using EPLOT.

5) PLESOL,S,EQV for plotting stress results and PRESOL,S,EQV for printing stress results of selected elements.

Regards,

Samir.

Subscriber

I think I was not precise enough. I have a simulation with extreme stresses at the boundary when I plot the nodal solution. So what I want to do is to exclude these elements at the boundary. Therefore I want to pick some elements in the middle and plot these stresses. I coded Samirs suggestion like this

CM, MYELEM, ELEM
CMSEL, S, MYELEM, ELEM
EPLOT
PLESOL,S,EQV

Where I get all elements. Where can I get just my certain elements?

This code also doesen't function (as it is a violation to the CMSEL command):

CM, MYELEM, ELEM
CMSEL, S, 10920, ELEM
CMSEL, S, 11000, ELEM
CMSEL, S, 11080, ELEM
EPLOT
PLESOL,S,EQV

• Rohith Patchigolla
Ansys Employee

As Samir suggested, you would need to select the elements first before creating the component (step 1).

Without component:

esel,s,,,10920

esel,a,,,11000

esel,a,,,11080

plesol,s,eqv

With component (for reuse):

esel,s,,,10920

esel,a,,,11000

esel,a,,,11080

cm, myelem,elem

cmsel,s,myelem,elem

plesol,s,eqv

Also, may I ask, if there is any reason to do the modelling/post-processing in APDL instead of Mechanical?

Best regards,

Rohith

Subscriber

ah esel does the magic thx. The reason for APDL is that a similar script exists before I was dealing with this project in APDL and APDL turned out to be useful, using it in a parameter study where I write the the commands in Matlab and then hand it over to Ansys and then get back the data. I will implement this in my code and see if it runs.

Subscriber

Ok at the end I adjusted the solution to my needs and used a location approach based on nodes found on xansys:

NSEL,S,LOC,X,19.000000,21.000000,
NSEL,R,LOC,Y,13.000000,16.000000,
ESLN,S,1
PLNSOL,S,X,
NSEL,ALL
ESEL,ALL

The advantage of the location approach is that I don't need to know all element numbers. The disadvantage is that I need to know approximately where the elements are.