What is the support or constrain condition for cure shrinkage of polymer?

  • Last Post 04 May 2019
  • Topic Is Solved
Guangqi posted this 03 May 2019

What is the support or constrain condition for  a disc shape polymer putted on a plane(like desk)? I want to know the shrinkage of thus polymer after heating and cooling. I use the ACCS extension 

some problems always happen

Order By: Standard | Newest | Votes
peteroznewman posted this 03 May 2019

Open the Geometry editor DesignModeler, assuming the disc is centered on the global origin, select the Tools > Symmetry > and set it to 2 planes and pick ZYPlane and XZPlane for the two planes and Generate.  If Symmetry Plane 2 remains yellow and doesn't accept the pick,change Model Type to Partial, then it will accept the input, and you can change it back to Full. This is a defect in the software. 

You will be left with a quarter of the circle. You may need to reattach the Convection BC in the Transient Thermal model (or not).

Refresh the project, then open the Model. The only BC you need in Static Structural is a Displacement on the table-touching face of Z = 0 leaving all others Free.

The part is now fully constrained by the two planes of symmetry and the one Displacement BC.

Guangqi posted this 04 May 2019

Thank you it works. But why? It seems that I just add a symmetry, and I think the result is supposed to be the same, right?

Besides, And there two another problems.

1. the result seems not symmetic in the corner. I think the result is supposed to be symmetic in the whole body.

2. It warns that "for a  linear analysis newton raphson type has been activated. The solution may not converge. For better results use program controlled." Where should I use program controlled? I tried use time step as the program controlled, but the warning is still there.



peteroznewman posted this 04 May 2019

Did you apply Convection to the Symmetry faces? There should not be Convection on those faces.

I don't know if the Composite Cure Simulation code has been written to respect Symmetry. You have to check that.

The dialog box is only a Warning, which you can ignore since the solution did converge.

You should rerun the simulation with 1/2 size elements, and then with 1/4 size elements to see if the results change a little. Maybe the non-uniformity is evened out by using smaller elements.

Guangqi posted this 04 May 2019

Thank you, I tried different size element, the results are same. I think that may because my meshing is not symmetric.

Besides, I still do not understand why adding a Sysmmetry condition could avoid error that I mentioned at the beginning? 

peteroznewman posted this 04 May 2019

A solid body has six degrees of freedom that must be supported for Static Structural to solve.

Each plane takes away two degrees of freedom and since all three planes are orthogonal, all six degrees of freedom are constrained.