How can I find stress on a node/point in ANSYS workbench?

You can make a named selection containing the node(s) you are interested in.

Then, in result, you may ask for the specific term (stress, strain, etc.) on the named selection that you have created.

In order to create the named selection you have to specify at Scoping Method -> Worksheet. Then, in the window that appears on the right, you must right click in the row below Action and choose Add Row. In the column Entity Type you must choose Mesh Node and in Criterion you may choose what ever suits you more (Location X, for example).

If this is not enough you can go back at Action to create a second (filtering) criteria.

And so on.

Or you may use an snippet command.

Hope that this is of any help to you.

Victor 

IMT Bucharest

Thank you so very much for your answer,

i am not very familiar with this software

i have tried doing what you have advised but could you please explain how the criterion and operator thing works because i have tried inputting the crierion as location x and the value as 1

and then pressed generate but that makes no diference

thanks in advance

Hello again,

First thing that you should do is to verify that it exists a node at x=1 and also take a look at the units. 1 could mean 1 mm or 1 m. the difference could play you a trick.

After specifying Location X you must go to Operator and make a selection (let's say Range). Two more option are to be made: Lower Bound and Upper Bound. Let's say you choose for lower bound 0.9 and for upper bound 1.1. If you pay attention you will see that the units are automatically specified, so you must adapt the values to the displayed unit. Press Generate and if everything is OK you will observe in "Details", below Scope, the number of nodes that are selected.

Then, hopefully, it will work.

Good luck,

it does not work if i specify location x, however if i select node id as criterion and operator as 1 it shows me one node in geometry under scoping method

is there a way to find out where this node exists, like its dimensions? 

as i need to compare the stress on this node with the calculated theoretical values on that nodes length

Thankyou!

Try this other method:

Coordinate System -> Insert Coordinate System (Rename it if you want) 

Now, in Details you must change Geometry Selection with Global Coordinates, specifying Origin X and Origin Y to your desired location

Then go to Solution -> Insert probe ->Stress

In details you must change Location Method from Geometry Selection to Coordinate System. Also you must choose for theLocation -> Coordinate System (or the name you gave it)

Then Evaluate All Results and you should see below the main window in the right "Tabular Data" containing all that you want.

Thank you very much for your help !

Hey Ali Khademi please can you tell me how to get the graphic annotation after selecting the probes manually. I am using Ansys 16 and I am not able to see the graphic annotations after I select the probes manually.