Hi all. I'm part of a senior design project that involves ASTM E1300 replication using open sourced FEM analysis. The project is detailed in the following blog https://marvinmodeling.wordpress.com/. None of the team members has extensive experience with Elmer and we've been struggling with the analysis.
At the moment were attempting to recreate deflection data of a statically loaded single pane monolithic glass panel. The panel is 60"x50"x0.085" sodalime glass with 5"x5" element size subjected to a 40 psf wind load. The ASTM E1300 deflection value were attempting to recreate is 1.09". Using Elmer tutorials as a guide, I've attempted the nonlinear elasticity and elastic plate equation sets. The closest I've come to replicating the deflection value is 0.0256".
I've spent more time than I'd like to admit trying to get an accurate solution. With so little Elmer experience I'm betting there's probably a really simple issue I'm missing. I figured I'd throw up a white flag and see if anybody had any thoughts, opinions, suggestions, etc. Any input would be greatly appreciated. Thanks!
Elmer Challenge

 Posts: 15
 Joined: 17 Feb 2019, 04:15
 Antispam: Yes
Elmer Challenge
 Attachments

 Sodalime glass properties.pdf
 (230.38 KiB) Downloaded 188 times

 case.sif
 (2.23 KiB) Downloaded 171 times

 60x50x0.085.unv
 (90 KiB) Downloaded 173 times
Re: Elmer Challenge
Hi,
Modeling a thin panel like this as a threedimensional body is known to be a hard problem for standard finite elements unless finite elements of high polynomial degree are used. Therefore I wouldn't expect a satisfactory accuracy by using 3D nodal finite elements.
To avoid poor accuracy a better strategy would be to apply special plate or shell finite elements (the plate solver module SMITC should be sufficient for accurate modeling of planar bodies) where dimensional reduction to two dimensions is applied. If you want eventually to couple the panel with some thick body that has to be modeled as a 3D body, the coupling of the bodies of different dimensions may however cause some troubles. If this scenario is expected, one might consider the 3D modelling of the panel with highdegree finite elements. The smalldisplacement elasticity solver (StressSolve) should support this option over a background mesh consisting of the lowestorder nodal finite elements. The additional command of the form (given in the solver section)
Element = "p:k"
with the integer k specifying the polynomial degree of the approximation could then be used. The nonlinear elasticity solver may have not been updated to support the highorder approximation.
Besides I couldn't generate a geometry model consistent with the posted sif file from the unv file (I tried the command ElmerGrid 8 2 60x50x0.085.unv autoclean and didn't get the number of boundary element groups referred in the sif file). I'm not sure whether there is an issue with the source file or ElmerGrid). Nevertheless, as already said, there may be other concerns as well. A better accuracy that what you mention should easily be possible with the plate solver.
 Mika
Modeling a thin panel like this as a threedimensional body is known to be a hard problem for standard finite elements unless finite elements of high polynomial degree are used. Therefore I wouldn't expect a satisfactory accuracy by using 3D nodal finite elements.
To avoid poor accuracy a better strategy would be to apply special plate or shell finite elements (the plate solver module SMITC should be sufficient for accurate modeling of planar bodies) where dimensional reduction to two dimensions is applied. If you want eventually to couple the panel with some thick body that has to be modeled as a 3D body, the coupling of the bodies of different dimensions may however cause some troubles. If this scenario is expected, one might consider the 3D modelling of the panel with highdegree finite elements. The smalldisplacement elasticity solver (StressSolve) should support this option over a background mesh consisting of the lowestorder nodal finite elements. The additional command of the form (given in the solver section)
Element = "p:k"
with the integer k specifying the polynomial degree of the approximation could then be used. The nonlinear elasticity solver may have not been updated to support the highorder approximation.
Besides I couldn't generate a geometry model consistent with the posted sif file from the unv file (I tried the command ElmerGrid 8 2 60x50x0.085.unv autoclean and didn't get the number of boundary element groups referred in the sif file). I'm not sure whether there is an issue with the source file or ElmerGrid). Nevertheless, as already said, there may be other concerns as well. A better accuracy that what you mention should easily be possible with the plate solver.
 Mika

 Posts: 1208
 Joined: 25 Jan 2019, 01:28
 Antispam: Yes
Re: Elmer Challenge
Also the 3D body is not rotating at the edges. I ran the problem and inspected the displacement at the edges. Therefore the model is behaving as a fixed edge condition which will have much less displacement than a pinned edge.
In addition, there is no restraint in the x or y direction, which static elastic bodies do not like. It makes convergence more difficult and you can end up with large displacements in unrestrained directions.
I generally try to hold the model at one node or surface in the other two directions in a way that doesn't cause stresses. For example if you grab 1 corner node in the X and another corner node in the Y, the body can't translate or rotate in space, since all of the other edges are restrained in Z.
In addition, there is no restraint in the x or y direction, which static elastic bodies do not like. It makes convergence more difficult and you can end up with large displacements in unrestrained directions.
I generally try to hold the model at one node or surface in the other two directions in a way that doesn't cause stresses. For example if you grab 1 corner node in the X and another corner node in the Y, the body can't translate or rotate in space, since all of the other edges are restrained in Z.

 Posts: 1208
 Joined: 25 Jan 2019, 01:28
 Antispam: Yes
Re: Elmer Challenge
I tried this with some other FEM codes the closest I could get with a 3D solid model was 0.4". I used shell elements and the answer came out 1.2"

 Posts: 1208
 Joined: 25 Jan 2019, 01:28
 Antispam: Yes
Re: Elmer Challenge
This is the solution I obtained with Elmer using the SMITC solver not the deformed shape i expected. The deflection is 1.65". Since the deflection exceeds the thickness of the panel the case is geometrically nonlinear. Is SMITC geometrically nonlinear? If I try the nonlinear elastic solver shell elements have no thickness, if I try the SMITC solver it is not nonlinear elastic?

 Posts: 1208
 Joined: 25 Jan 2019, 01:28
 Antispam: Yes
Re: Elmer Challenge
Shell solver has a good deformed shape but, 0.43" defelction
[/attachment]
[/attachment]
 Attachments

 shellsolvercase.sif
 (1.9 KiB) Downloaded 175 times

 Posts: 15
 Joined: 17 Feb 2019, 04:15
 Antispam: Yes
Re: Elmer Challenge
Greatly appreciate the replies. Lots of great information to consider. We ran into similar issues with the SMITC solver and have since focused on the nonlinear elasticity equation set. Also making attempts at manipulating the mesh size and volume in order to recreate the E1300 deflection values. Closest match to E1300 values now is with a 0.219" thick plate with an element thickness of 3. Results in a displacement of 0.39". The E1300 deflection value for this thickness is 0.54". Still a ways to go.
 Attachments

 cube_3 elements deep.grd
 (791 Bytes) Downloaded 168 times

 case.sif
 (1.82 KiB) Downloaded 168 times

 Posts: 1208
 Joined: 25 Jan 2019, 01:28
 Antispam: Yes
Re: Elmer Challenge
Still getting zero edge rotation in the Elmer solution, and E1300 values appear to be for pinned supports where the edge of the plate rotates. Edges having no rotation will significantly reduce the displacement.

 Posts: 1208
 Joined: 25 Jan 2019, 01:28
 Antispam: Yes
Re: Elmer Challenge
To get some rotation on the edges I extended the edges down 6 inches, the thin side walls would allow the edges of the plate to rotate some. Not a very good mesh, but the deflection is 1.3 inches.
Re: Elmer Challenge
I would still suggest handling problems of this type via dimensional reduction.
As the case appears to be nonlinear, the plate solver (SMITC) is not feasible due to its linearity. So, if the case is modelled using the nonlinear shell solver with simply supported edges (no displacement in the direction of surface normal), the attached files give the maximum deflections 0.534 in and 1.18 in for the plates of sizes 60" X 50" X 0.219" and 60" X 50" X 0.085". These values seem to be relatively close to what you expect.
Here one quarter of the plate is modelled by assuming symmetry conditions. Although symmetry conditions may not generally be feasible for nonlinear analysis, I suppose the material would here break anyhow before the onset of possible symmetry breaking. In addition, the load is increased gradually to avoid convergence troubles in the nonlinear iteration.
 Mika
As the case appears to be nonlinear, the plate solver (SMITC) is not feasible due to its linearity. So, if the case is modelled using the nonlinear shell solver with simply supported edges (no displacement in the direction of surface normal), the attached files give the maximum deflections 0.534 in and 1.18 in for the plates of sizes 60" X 50" X 0.219" and 60" X 50" X 0.085". These values seem to be relatively close to what you expect.
Here one quarter of the plate is modelled by assuming symmetry conditions. Although symmetry conditions may not generally be feasible for nonlinear analysis, I suppose the material would here break anyhow before the onset of possible symmetry breaking. In addition, the load is increased gradually to avoid convergence troubles in the nonlinear iteration.
 Mika
 Attachments

 plate.grd
 (711 Bytes) Downloaded 168 times

 simply_supported.sif
 (1.79 KiB) Downloaded 174 times