thermal expansion

General discussion about Elmer
kevinarden
Posts: 2237
Joined: 25 Jan 2019, 01:28
Antispam: Yes

Re: thermal expansion

Post by kevinarden »

Mesh size up to a point will change the answer, it is one of the attributes of accurate LE results, the other being higher order elements.
Roland
Posts: 226
Joined: 12 Apr 2018, 11:29
Antispam: Yes

Re: thermal expansion

Post by Roland »

Hi Kevin,
Yes but the mesh of the plate has the same size and (with Peter's help) I used p2 elements in my 2 models and nevertheless they don't give the same result!
What do you think about that?
kevinarden
Posts: 2237
Joined: 25 Jan 2019, 01:28
Antispam: Yes

Re: thermal expansion

Post by kevinarden »

According to Rich post Body 2 and 3 in EM model is the plate and coating and only have 81 elements. in the HE-LE model they have 100 elements.
kevinarden
Posts: 2237
Joined: 25 Jan 2019, 01:28
Antispam: Yes

Re: thermal expansion

Post by kevinarden »

Here is the HE_LE case that works. Case 1 is no air elastic body only and the deflection is 0.146. Second case is added air around the elastic body, but ignored it in the sif, same deflection 0.146. Third case is allowed the air to participate in the heat equation, but it slightly changed the temperature due to slightly different boundary condition. Deflection still close at 0.135.

I think there may be a bug in Roland's model that we have not found yet,
test_he_le.zip
(74.32 KiB) Downloaded 46 times
Rich_B
Posts: 421
Joined: 24 Aug 2009, 20:18

Re: thermal expansion

Post by Rich_B »

Hello,

I did not try to check the boundary conditions for consistency between the two models. If you want to reduce the complexity, you could use ElmerGUI to modify the mesh.* files for each model, and join most of the boundaries together, reducing the huge number of BC selections.

Just a thought.

Rich.
kevinarden
Posts: 2237
Joined: 25 Jan 2019, 01:28
Antispam: Yes

Re: thermal expansion

Post by kevinarden »

I recreated Roland's plate model from scratch and then made a version with air, simpler model. I did not get the same answer with plate only, plate with air ignoring air, and plate with air including air in heat equation. Three different answers.
coating.zip
(60.13 KiB) Downloaded 43 times
Rich_B
Posts: 421
Joined: 24 Aug 2009, 20:18

Re: thermal expansion

Post by Rich_B »

Hello,

I downloaded 'coating.zip', and ended up adding this third solver to both sif files.
Solver 3
Equation = SaveLine
Filename = profile_HT_LE.txt
Procedure = "SaveData" "SaveLine"
Polyline Divisions = Size(1); 100
Polyline Coordinates = Size(2,3)
-.105 0.0 -.0154
.105 0.0 -.0154
End
Then plot the x coordinate versus the z displacement, for all 20 time steps, for each case.
profile_ht_le.png
profile_ht_le.png (162.32 KiB) Viewed 528 times
In the next plot, the first time step shows negative z displacement.
profile_em_ht_le.png
profile_em_ht_le.png (94.16 KiB) Viewed 528 times
Rich.

Edit: The case EM_HT_LE from coating.zip, is missing Initial Condition 1 in Body 1, which is why the z displacement went negative on the first time step. Body 1 was set to zero degrees temperature initially by default. Adding the missing initial condition to Body 1 corrects the negative z displacement, and now both cases match.
Last edited by Rich_B on 16 Jul 2022, 22:53, edited 1 time in total.
Roland
Posts: 226
Joined: 12 Apr 2018, 11:29
Antispam: Yes

Re: thermal expansion

Post by Roland »

Hi Kevin and Rich,
Many thanks for your efforts!
But unfortunately, up to now, if I have correctly understood what you did in your tests (including your Saveline equation results, Rich), my models of the case plate alone and plate+surrounding_air (with air not activated) don't give the same deflection result (even if your test_he_le.zip model gives the same result...). Just for reference these same 2 cases in Comsol give the same 10 mm deflection result which seems the correct physical value. Concerning the plate mesh element numbers, Rich, I tested the same element number in both EM_HT_LE and HT_LE models, meaning 81 (9*9) elements for both, and the result are still very different (the correct one, meaning 10 mm for HT_LE model, and only something like 40 microns (!!!) for the EM_HT_LE model).
As you say it, Kevin, there is probably a bug in my models.... So I would be very (very...!) thankful to you if you could again take a look at my 2 models and try to find something which is wrong. I continue also on my side, since, as you can understand, I cannot let this problem unsolved...!
We keep us informed.
Thanks in advance!
kevinarden
Posts: 2237
Joined: 25 Jan 2019, 01:28
Antispam: Yes

Re: thermal expansion

Post by kevinarden »

I completely rechecked the model again, and tried changing some solver settings, no luck in finding a solution.
kevinarden
Posts: 2237
Joined: 25 Jan 2019, 01:28
Antispam: Yes

Re: thermal expansion

Post by kevinarden »

The only thing I could think of was mesh quality. In my test model that worked, the air mesh was hex and matched the plate. In Roland's model the air mesh was linear tets and the ones around the plate were fairly large. So I did the following:
1 converted the spiral.mphtxt to a gmsh using ElmerGRid
2 Used gmsh to refine the mesh by splitting elements
3 Used ElmerGrid to convert new gmsh file using -increase to make the tets quadratic instead of linear
4 Had to change the LE solver to direct (banded), the iterative gcr was not converging

Roland's model now solves correctly and matches the plate only case.

I made the gmsh, sif, and elmer mesh available on github
https://github.com/mrkearden/EM_HT_LE
Post Reply