Convergence Issues - Highly Distorted Elements

  • 122 Views
  • Last Post 2 weeks ago
jonnyflowers posted this 2 weeks ago

I am having issues attempting to get a model to converge as I am getting the highly distorted elements error.

I have tried increasing the time it takes to apply the load and tweaking a couple settings within Ansys.

If someone could give me some advice on how to overcome errors like this I would really appreciate it.

 

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 2 weeks ago

Hi Jonny,

Use Symmetry
Cut the problem in half by using a symmetry plane down the center of your block. You have a channel in the rubber material for most of the length. Do you need the rubber split into a Top and Bottom then bond it together with contact? It would solve faster using Share Topology.

Increase Mesh Density Near High Distortion
The initial mesh is being distorted and causing numerical problems and it stopped 3.8 mm out of 10 mm desired.

       

Bias your mesh to make smaller and more square elements at the surface where where the maximum distortion is occurring. A biased mesh would better cope with the displacement being applied. This mesh made it to 4.2 mm out of 10 mm, a bit better but not enough.

 

Contact with Surface Instead of Displacement
I assume the faces of the model that have the displacement applied are actually being squeezed by a surface. If you replace the displacement on the faces with displacement of a surface and add contact with the faces, you may get a more realistic simulation of the deformation.  Is the edge of the surface actually a sharp corner, or does it have a small radius along the edge? Including a radius on the edge of the surface and enough elements on the rubber to follow the radius will help to have the model converge. In this example, the displacement got up to 8.7 mm out of 10 mm before an element distorted.

Regards,

Peter

  • Liked by
  • jonnyflowers
peteroznewman posted this 2 weeks ago

Mechanical Settings Best Practice

I noticed that you have duplicate contact definitions in your archive. If you right click on a folder in the Contact branch, and Check Overlapping Contact Regions, you will see a long list. This is caused by having a setting in Workbench, Tools, Options checked. With this checked, each time you Attach the CAD geometry, it automatically adds contact pairs on all the adjacent faces it finds. This is the installation default for ANSYS, but I think it is a dangerous setting.

  • Liked by
  • jonnyflowers
peteroznewman posted this 2 weeks ago

Frictionless Support is limited to initial face dimensions
Another change needed in your model is to delete the frictionless support and replace it with an oversized rigid surface and frictionless contact. Frictionless support is a "short cut" that takes the faces picked and creates the rigid surface and contact for you "behind the scenes". This is a good time-saver when there are small displacements, but when there is large displacements, there is no surface for the material to expand onto. The node on the edge gets hung up on the edge of the invisible surface and gets highly distorted.

There may be a reason to use some friction, since the radius on the top rigid surface starts to apply a force on the rubber that pushes it to the right and ends up distorting the element at the edge of the fixed constraint on the bottom. Another solution might be to have the fixed constraint on the right vertical face of the rubber block instead of on a part of the bottom face. That would directly oppose the force put on by the frictionless radius.

 

  • Liked by
  • jonnyflowers
jonnyflowers posted this 2 weeks ago

Thank you for the help Peter, I am running a simulation now that uses some of your advice.  Unfortunately I can't use a radius as I am interested in the contact with the sharp edge.  Would it be possible for you to attach an archive for the file you made so I can get a closer look at how you put it all together, I would really appreciate it.

Thanks

peteroznewman posted this 2 weeks ago

Hi Jonny,

If you have a sharp corner, the stress might be so high that you would cut the rubber, which you won't see in the simulation. You will need a very fine mesh below the corner to model the sudden change at the corner so even a small radius would help the solver to converge.

I used two more "tricks" to get the solution to solve to the full 10 mm of displacement. I don't know which one was necessary, or if both were, but those changes were to (1) add a hyperelastic material model (Yeoh 1st order) to your material, and (2) to change the SOLID186 element formulation using keyopt(2) and keyopt(6) to make the elements work better with incompressible materials.

 

Without those changes, the solution failed to converge at 8.8 mm when the elements "exploded" into a pattern called "hourglass" mode. You don't want this to happen. It went from this...

to this on the next iteration.

I have attached an ANSYS 18.2 archive that solves in 7 minutes on 8 cores. I simplified the model by taking out the channels, but you could put them back in fairly easily with a pull operation. This is a coarse mesh and you will want more detail around the silicon chip. The contact is not performing well with this coarse mesh.

You can show your appreciation by clicking "Like" on the posts that are helpful. Good luck with your project!

Regards,

Peter

Attached Files

  • Liked by
  • jonnyflowers
jonnyflowers posted this 2 weeks ago

Thank you, I am running a sim at the moment with a lot of your advice thrown in.

Why the use of connectors instead of supports though?

peteroznewman posted this 2 weeks ago

If you try to apply a fixed support to a rigid body, you will find you can't.  You have to use a fixed joint to hold a rigid body to ground.

  • Liked by
  • jonnyflowers
peteroznewman posted this 2 weeks ago

I took my model with the two "tricks" mentioned above: Hyperelastic material and Element Keyopts, and made two copies. I ran one copy with just the Hyperelastic material and the other copy with just the Element Keyopts.  Neither copy ran to convergence. Both "tricks" are needed to run to convergence.

The Element Keyopts require a command snippet under each rubber geometry (ctrl drag works to copy it to the solid below). I set Element Control to Manual then the Brick Integration Scheme to Reduced. This is the same as Keyopt(2) but sometimes the solver reset Keyopt(2) when I left Element Control to Program Controlled instead of Manual.

 

----------------------------------------------------------------------------------------

   

      

  • Liked by
  • jonnyflowers
jonnyflowers posted this 2 weeks ago

Thanks, I have added these tweaks and I am running the simulation now

Can I ask where you got the values you used for the Yeoh material properties?

Thanks

Jonny

peteroznewman posted this 2 weeks ago

If you go to the ANSYS Help and search for Yeoh, you will find an entry 4.6.11. Yeoh Hyperelasticity.

It documents that a first order N=1 model, 

I used the shear modulus and bulk modulus calculated for the PDMS Elastic material model you provided to calculate c10 and d1 from the formulas above.

Regards,

Peter

jonnyflowers posted this 2 weeks ago

So with the next step in my model, I have been applying a set of hydrostatic elements to the interior of the channels, I am unsure if this works when I use symmetry.  The script I am using is below and it is being solved with a transient analysis;

!   Commands inserted into this file will be executed just after material definitions in /PREP7.

!   Active UNIT system in Workbench when this object was created:  Metric (m, kg, N, s, V, A)

!   NOTE:  Any data that requires units (such as mass) is assumed to be in the consistent solver unit system.

! It is assumed that NO SYMMETRY effects are in this model.

 

fini

/prep7

*get,typemax,ETYP,,NUM,MAX    ! max defined element type

*get,realmax,RCON,,NUM,MAX    ! max defined real constant

*get,mat_max,MAT,,NUM,MAX     ! max defined material

*get,nodemax,NODE,,NUM,MAX    ! highest numbered node in model

 

! Create a new higher number for element type, real, and material

newnode=nodemax+1000          ! number for pressure node for HSFLD242

newnumber=typemax+1

*if,realmax,ge,newnumber,then

   newnumber=realmax+1

*endif

*if,mat_max,ge,newnumber,then

   newnumber=mat_max+1

*endif

 

et,newnumber,HSFLD242         ! 3-D Hydrostatic Fluid Element

keyopt,newnumber,1,0          ! UX, UY, UZ, plus HDSP at pressure node

keyopt,newnumber,5,1          ! Fluid mass calculated based on the volume of the fluid element

keyopt,newnumber,6,1          ! Incompressible

mp,dens,newnumber,6440        ! Density of Galinstan, kg/m^3

                              ! Ignoring thermal expansion in this example

type,newnumber                ! Ignoring TB,FLUID in this example

mat,newnumber                 ! Ignoring Reference pressure for compressible gas

r,newnumber,0.10156           ! Applying intitial atomospheric Pressure = 0.10156 N/mm^2

real,newnumber                ! 

 

cmsel,s,Channel1        ! Select nodes on interior

esln                          ! Select elements that touch these nodes

n,newnode,0,0,1.2e-002        ! Pressure node at 0,0,400 (automatically moved to centroid?)

ESURF,newnode                 ! ESURF HSFLD242 elements over solid element faces

                              !    Extra node "newnode" with ESURF with HSFLD242

allsel

fini

/solu                         ! return to solving

 

  • Liked by
  • peteroznewman
peteroznewman posted this 2 weeks ago

If you search the ANSYS Help for HSFLD242, you will find this paragraph that says you can use symmetry if you keep the pressure node on the symmetry plane.

The pressure node (Q) can be located anywhere in the fluid volume, except when the fluid volume has symmetry boundaries; in this case the pressure node must be located on the symmetry plane or on the intersection point or edge of multiple symmetry planes. The pressure node is automatically moved to the centroid of the fluid volume if there are no displacement degree-of-freedom constraints specified. To keep the pressure node on a symmetry line, you must specify symmetry boundary conditions at this node. (The displacement degrees of freedom at the pressure node do not have any displacement solution associated with them. They are only available for applying displacement degree of freedom constraints.) The pressure node is shared by all the hydrostatic fluid elements used to define the fluid volume. 

The comment about NO SYMMETRY in the script above is probably because it is not coded to obey the rule on the pressure node. I'm not an APDL expert so I can't help with the script, I just know how to use scripts other people write for me : )

I am curious what is the function of a rubber block with fluid channels and a silicon chip; if you are willing to share...

Close