Skip to main content
J
JI_107154871-Visitor
1-Visitor
July 11, 2023
Solved

Creo Simulate Radial Expansion

  • July 11, 2023
  • 1 reply
  • 2627 views

I am attempting to run a rather simple finite element analysis on a stainless steel rod with a moment (0.1 Nm) applied on one end and a fixed constraint on the other end. The displacement result is not what I had expected and I do not believe it to be realistic (please reference the images). The end of the rod that has an applied moment expands radially. I am attempting to replicate a benchtop test and I know that the rod does not expand radially, instead, it simply rotates and the other end deforms. Am I missing a constraint somewhere? Should I be opting for a nonlinear analysis with large deformations? 

 

Software: Creo 8.0

 

P.S.: I am much more familiar with ANSYS and am a new Simulate user so any help will be greatly appreciated.

 

Best answer by ilyachaban

It is correctly shown. You are running linear analysis and this is how deformation works. If you apply moment on a circular object it will have tendency to move in tangential direction. This is what you see on a picture. If you want to see diffrent results i would like to recommend running LDA (Large Deforamtion Analysis). This way your driver will be twisted the way you have expected it. 

Looking at your analysis your boundary conditions could be defined better so there is no tension in material. And if you correctly interpret result of your analysis you will be able to do it with simple small deformation analysis.  

1 reply

I
ilyachaban16-PearlAnswer
16-Pearl
July 12, 2023

It is correctly shown. You are running linear analysis and this is how deformation works. If you apply moment on a circular object it will have tendency to move in tangential direction. This is what you see on a picture. If you want to see diffrent results i would like to recommend running LDA (Large Deforamtion Analysis). This way your driver will be twisted the way you have expected it. 

Looking at your analysis your boundary conditions could be defined better so there is no tension in material. And if you correctly interpret result of your analysis you will be able to do it with simple small deformation analysis.  

    3
    346gnu13-Aquamarine
    13-Aquamarine
    July 31, 2023

    Yes it is correctly shown but the actual reason is as follows.

     

    The default post processor scaling for small deflection (linear) is making the largest calculated movement equal to 10% of the model size with all smaller movements scaled accordingly. This is so that we can actually see the movement because the real movement will be microstrain and otherwise invisible.

     

    Your loaded end moves more and therefore scaling makes it look like it is 'exploding'.

     

    The X&Y components of the tangential movement become exagerrated.

     

    Careful interpretation of such images is required with this 'limitation' in mind.

     

    Check. Measure the movement X & Y of any point on the circumference*

     

    Set the deflection scaling to '1' and deselect '%'. This will give you actual movement and is likely invisible to the eye.

     

    I suspect the strain is small enough that small defelction (linear) is ok initially.

     

    *Sadly we cannot combine X&Y in the post processor therefore we must measure and manually calculate the numbers we want. With such models it is always prudent to put a radial csys in BEFORE running such that the results can be shown it the radial csys rather than the cartesian. Unfortunately Simulate throws the solution away when the solve is completed and the addition of another csys after a solve means a complete re-run.

     

    Using a radial csys will not change the visual scaling; the end still 'explodes'

     

    LDA & contact default (which can be changed by the user) post processor scaling is '1' absolute (and not '10%' model size). 

     

      Terms & ConditionsAccessibility statement