40m QIL Cryo_Lab CTN SUS_Lab TCS_Lab OMC_Lab CRIME_Lab FEA ENG_Labs OptContFac Mariner WBEEShop
  COMSOL elog  Not logged in ELOG logo
Entry  Mon Dec 4 16:27:13 2017, aaron, Mechanics, PonderSqueeze,  
    Reply  Mon Dec 4 17:42:53 2017, gautam, Mechanics, PonderSqueeze, FEA on optimus 
       Reply  Mon Dec 4 19:49:32 2017, gautam, Mechanics, PonderSqueeze, FEA on optimus 
          Reply  Tue Dec 5 10:50:54 2017, aaron, Mechanics, PonderSqueeze, FEA on optimus 
             Reply  Tue Dec 5 19:50:47 2017, aaron, Mechanics, PonderSqueeze, FEA on optimus 
                Reply  Tue Dec 12 11:50:12 2017, aaron, Mechanics, PonderSqueeze, FEA on optimus SERaLIGO.jpg
Message ID: 118     Entry time: Mon Dec 4 16:27:13 2017     Reply to this: 119
Author: aaron 
Type: Mechanics 
Category: PonderSqueeze 
Subject:  

Meshing Surface Layers

Defining New Selections

I don't know why I wasn't seeing this problem with previous models (perhaps because I wasn't importing any CAD or STEP files), but my latest attempts at meshing and selecting specific domains of my model were being thwarted by inconsistent domain definitions. I was previously always manually selecting domains, which is confusing because all domains just get assigned a number when they are created. Worse, sometimes the numbers assigned to domains change when the model rebuilds, especially if there has been a significant change in the model geometry. This results in later steps selecting the wrong set of domains (or boundaries, etc).

To fix this problem, I created new selections (sets of domains, boundaries, or etc that receive their own label and can be selected as a group later in the model). The new selections include:

-Domain selections that separate surface and bulk layer for all domains in the fibers (fiber stock, neck, thick section, taper, and main section, in order from the horn to the center of the fiber)
-Boundary selections for all domain selections described above

This is probably also a necessary step for getting reliable results when interfacing with MATLAB, and might explain some weird problems I was running in to a while ago and just made haphazard fixes for.

Mesh Steps

I use the following mesh steps to get what seems like a pretty reliable meshing:

  1. Mesh the upper tapers (bulk and surface separately) with a free tetrahedral mesh
    1. I mostly use the defaults for an extremely coarse mesh, but the only parameter that seems to make a large difference is the minimum mesh size. I set this to the skin_depth for the surface layer, and (fiber_main_radius-skin_depth) for the bulk. fiber_main_radius-skin_depth should be the radius of the bulk domain, and the skin_depth characterizes the smallest length scale in the surface layers. I have some limited ability to tweak the minimum mesh sizes when the surface layer is comparable in size to the fiber_main_radius (so the surface layer is comparable to the entire fiber radius), but it seems to be best to keep the mesh this fine when the surface layer becomes small.
  2. Mesh the main fiber (bulk and surface separately) with a swept mesh
    1. I create a distribution with a fixed number of elements, at ceil(fiber_main_length/fiber_stock_radius/2). This is somewhat arbitrary--the stock has the largest radial length scale, so I figured I'd divide up the main fiber into units that tall. A better thing would be to know how high a mode we are interested in studying, and break up the fiber into enough pieces to observe that mode. Seems fine for now, might want this distribution to be a bit coarser though.
  3. Mesh the lower tapers (bulk and surface separately) with a free tetrahedral mesh
    1. Use the same size settings as on the upper tapers
  4. Mesh the thick sections (bulk and surface separately) with a swept mesh
    1. The distribution uses a fixed number of ceil(fiber_thick_length/fiber_stock_radius/2) elements. Again perhaps this can be coarser; it also doesn't attempt to make a finer mesh at the thermoelastic cancellation region.
  5. Mesh the necks (bulk and surface separately) with a free tetrahedral mesh.
    1. I use an extremely coarse mesh with the minimum mesh element size set to fiber_thick_radius-skin_depth for the bulk; for the surface it is an extra coarse mesh instead, because the extremely coarse mesh gave low quality mesh elements. I'm not sure why this is, I can't see much difference and the problem only seems to happen to one of the 8 neck sections (why not in all sections?). The problem only arises when the skin depth is less than 20um, for the other parameters at the nominal aLIGO values.
  6. Mesh the stocks (bulk and surface separately) with a swept mesh
    1. Distribution is again ceil(fiber_stock_length/fiber_stock_radius/2), resulting in 2 vertical divisions of the stock.
  7. Mesh the horns with a free tetrahedral mesh
    1. Size is an extremely coarse mesh, where the minimum element size is set to the skin_depth (because the horn sees the boundary of the stock surface, so its smallest adjacent element can have a scale down to the skin_depth), and maximum growth rate is increased to 9 (any higher results in low quality mesh elements; I set it high because most of the horn does not need to be meshed as finely as the part directly in contact with the fiber stock).

Note on the skin depth: I defined the thickness of the surface layer by the parameter skin_depth. Since we are interested in how the energy in the surface layer changes with the radius of the fiber, and expect that the surface depth doesn't change much with fiber radius (a very thick fiber will have a few micron surface layer; so will a fiber half that diameter). I managed to get the mesh working with a 15um surface layer, but was having trouble getting a 10um layer. I wasn't completely sure how small a surface layer would be necessary, but for a test mass 1/100 the size of the aLIGO masses, the main part of the fiber would have a radius of 20um, so if we want to study the surface layer for masses down to that size I figure the skin depth should be at most around 10-15um. It would be better to be motivated by the actual scale of the physics going on at the surface--how deep to micro cracks and other lossy imperfections go?

Study

I'm running the frequency study on a small number (2) of frequencies in each decade from 60Hz to 10kHz (so there should be 5-8 total frequencies in the study). I started it at 4:25pm on my local machine, and it hasn't gotten very far in 30 minutes, so I may abort the study and try to make the mesh coarser--especially the distribution settings, which are easy to change.

ELOG V3.1.3-