How to select points correctly in stress linearization?

[mike.cheng]

Hi everyone,

I am trying to use the stress linearization function to get the Pm and Pb value for a pressure vessel. In order to define the SCL I have to select 3 points, first point and last point to define the SCL line, third reference point to define the local coordinates system. Now I have a problem for define the last point which located inside of vessel shell, since I have a full vessel model (for many cases, I can created symmetric 1/2 vessel then it is easy to define any points, but this vessel I cannot create only half ). I tried to use section view function under plot option, then the model looks OK and it gives me the section view that I want. However, when I selected the point by clicking the node in the view, it still applied to the outside node point which has been turned off by section tool. 

What is the easiest way to define a node point inside of a pressure vessel?  Or easy way to define any points inside of the enclosed shell?  Are there any function like "show/hide elements" in ANSYS? 

Thanks!

[John_Holtz · Accepted solution]

Hi @mike.cheng 

Your options in the Stress Linearization are to select a node, type a node number, or type the coordinates.

Inventor Nastran works off of the CAD model (naturally), so your level of control ends at the level of the parts. You cannot hide chosen elements, but you can hide the entire Idealzation which effectively hides the nodes and elements for that part or parts. Then you can either use "Nodes > Query Display" to determine the node number on the parts that are still shown (and then type them into the Stress Linearization), or you can click the node in the Stress Linearization.

In other cases, you may want to split a big part into smaller pieces so that you can hide some of the pieces in order to access the inside of the vessel.

[mike.cheng]

Thanks very much for the reply.

[AndrewWeighell7348]

A neat way to create an SCL exactly where you want is as follows.

a) Decide where SCL should be based on stresses from your first run.

b) Return to Inventor. Create a plane on what should be the Stress Classification Plane SCP.

c) Create a sketch on the plane.  Project cut edges adjacent to the SCL.

d) Draw a line to represent the SCL as required.

d) Add sketch points at the beginning and end of the SCL.    

e) Constrain and dimension several equi-spaced points  along the SCL.  (Spacing equal to the desired mesh size along the SCL).

f) Add a sketch point off the SCL and on the outside surface of the model to set the SCP. 

g) Keep the sketch visible.  Return to Nastran.

h) Open a mesh control window.  Add all the sketch points created above to the "Vertex Data".  Set the mesh size equal to the point spacing above.  (All points are selectable through thickness so no need to section.  The sketch geometry and dimensions will "point" to the sketch points allowing them to be selected by guess.  i.e.  At the end of each dimension used to locate the sketch points along the SCL).  Set the mesh growth to a low number to prevent  localised area of small mesh.

i) Remesh.  Nodes will be created at the sketch points.

j) Rerun.  The surface nodes required for the SCL utility can be selected by going inside the model or sectioning slightly off the SCP. 

(Splitting the model into two bodies to make internal mesh visible on the SCP changes the stress pattern.  Not much but enough to look a bit odd to somebody expecting a smooth transition).

h) If you need to move the SCL.  Go back into the Inventor model and move the plane or line.  The mesh control might need to be reset. (I have not tested this).

The above process works really well.  The only problem is the SCL data does not seem to be saveable? 

[vmurugesh]

This method is only applicable when there is one load case, with a very text book data sets and fea parameters.

In reality, this method is not feasible as there would be heaps of load cases, multiples variations in fea parameters before and after verification, addition or modification of part geometry to meet code compliance, and different level of results extraction.