thermal expansion

General discussion about Elmer
Post Reply
Roland
Posts: 226
Joined: 12 Apr 2018, 11:29
Antispam: Yes

thermal expansion

Post by Roland »

Hi,
I try to make an example of thermal expansion in a square thin bi-material plate made of aluminium(body 1) covered with an insulating coating (body 2). The corresponding case.sif is here attached with a jpg showing the meshed plate. The heat equation (say HT) is coupled with the linear elasticity physic (say LE) in order to determine the displacement resulting from the thermal expansion, in transient state from 0 to 20s. A heat source is set in the aluminium body, corresponding to a global injected power of about 260 W. For the boundary conditions we set convective losses on the 2 upper and lower external faces for HT and a zero vertical (along z) displacement for LE on the 8 vertical thin side faces of the bi-material plate. Dimensions: Aluminium:105mm*105mm*0.3mm/ insulating_coating:105mm*105mm*0.5mm
The GCR algorithm is used for LE and the solver seems to converge well.
After 20s solving, according to the same example made with Comsol, the vertical displacement (displacement_z) should be around 10 mm (the plate bends due to the bi-material phenomena). Unfortunately Elmer shows a resulting vertical displacement (displacement_z) of only something like 40 microns which seems uncorrect.
It would be very nice if somebody could take a look at the case and give some help elements for fixing this problem.
Thanks in advance.
Roland
Attachments
plate.JPG
plate.JPG (58.88 KiB) Viewed 1281 times
case.sif
(3.76 KiB) Downloaded 75 times
raback
Site Admin
Posts: 4812
Joined: 22 Aug 2009, 11:57
Antispam: Yes
Location: Espoo, Finland
Contact:

Re: thermal expansion

Post by raback »

Hi Roland,

Did you try with quadratic elements? Linear elements in elasticity suffer from "locking" which means that displacements are underestimated. I think internally Comsol often uses quadratic elements although the mesh looks linear.

In Elmer you could either use quadratic nodal element (hexahedrons with 20 or 27 nodes) or define p-element with the line in Solver section (for many, not all solvers):

Code: Select all

Element = p:2
Hope this helps.

-Peter
Roland
Posts: 226
Joined: 12 Apr 2018, 11:29
Antispam: Yes

Re: thermal expansion

Post by Roland »

Hi Peter,
Thanks for your answer. I will try that and keep you informed.
Just another thing: will you have a few moments to take a look at the EM_levitation model (I sent you the case.sif 2 or 3 weeks ago) which works almost perfectly now, except for some liquid "peaks" which appear on the surface of the levitated charge after several time steps?
It would be very kind of you if you could give me some help elements for getting a perfect liquid shape...!
Thanks in advance
Roland
Roland
Posts: 226
Joined: 12 Apr 2018, 11:29
Antispam: Yes

Re: thermal expansion

Post by Roland »

Hi Peter again,
I just tried to add the line "Element = p:2" in the elastic solver, but then the solver does no more converge and displays following error message:
"ERROR:: IterSolve: Numerical Error: Too many iterations were needed."
I will try to re-import the geometry from Comsol with quadratic elements this time (it's an option when exporting a geometry).
Any idea from your side would be also wellcome...
We keep us informed.
Thanks
Roland
mika
Posts: 230
Joined: 15 Sep 2009, 07:44

Re: thermal expansion

Post by mika »

The sif files repeats the constraint

Displacement 3 = 0

twice in the same BC section. You should at least add constraints which prevent both rigid body translations in the X-Y plane and rotations around the Z-axis to have a unique solution. The lack of uniqueness may cause convergence problems.

In addition, the sif file defines

Active Solvers(2) = 2 1

As iterations within a time step are prevented (Steady State Max Iterations = 1), should you solve the temperature first to avoid a lag?

-- Mika
Roland
Posts: 226
Joined: 12 Apr 2018, 11:29
Antispam: Yes

Re: thermal expansion

Post by Roland »

Hi Mika,
Thanks for your answer.
Concerning the BC conditions, ok I will supress the twice repeated Displacement 3 = 0 and let it only once. It corresponds intentionnaly to just forbid the 8 vertical side faces of the plate to move vertically, which means that the plate is just set (on his 8 vertical side faces) on something which could be a supporting table, you see? I didn't enter other BC's since I want the plate to be free to expand in the x-y plane but also to bend due to the bi-material plate(the 2 materials have 2 different thermal expansion coefficients which causes the bending). The here attached jpg result shows the bending in the same example with Comsol, showing a vertical Z displacement of about 10 mm, while Elmer gives only something like 40 microns!
Concerning the solvers, could you explain what exactly means " Steady State Max Iterations"? I still don't master very well all the solvers settings... For instance how is it possible to first calculate (in time dependant over 20s for instance) the heat transfer physic in a first step and then, by giving the calculated temperature to the linear elasticity solver, to run this linear elasticity solver in a second step? Is this possible with Elmer?
Thanks in advance for your help!
Roland
Attachments
plate.JPG
plate.JPG (40.42 KiB) Viewed 1256 times
Roland
Posts: 226
Joined: 12 Apr 2018, 11:29
Antispam: Yes

Re: thermal expansion

Post by Roland »

Hi,
As suggested by you, Peter (many thanks!), I added in the linear elasticity solver the line "Element = p:2" and now, after also correcting a remaining error in the physics (my fault!), the result is perfect and exactly the same as in Comsol!
Please Peter, keep me also informed when you have a little time to take a look in the EM_levitation case.
Many thanks again!
Roland
kevinarden
Posts: 2237
Joined: 25 Jan 2019, 01:28
Antispam: Yes

Re: thermal expansion

Post by kevinarden »

For instance how is it possible to first calculate (in time dependant over 20s for instance) the heat transfer physic in a first step and then, by giving the calculated temperature to the linear elasticity solver, to run this linear elasticity solver in a second step? Is this possible with Elmer
In the simulation section you can create a restart file, and only run the heat solver equation for the first 20 steps

output file = heatsolve
binary output = true

You can then do a second run with only the LE solver for 1 step, it will restart form the end of the first one and create another step that has the last heat condition plus linear displacement, restart position could be any step, but 0 means restart from the last step

restart file = heatsolve
restart position = 0
Roland
Posts: 226
Joined: 12 Apr 2018, 11:29
Antispam: Yes

Re: thermal expansion

Post by Roland »

Thanks Kevin for these explanations.
I am not sure to understand everything in detail but I see the spirit of the method.
I will try this and keep you informed, and probably ask futher help...
Thanks again
Roland
kevinarden
Posts: 2237
Joined: 25 Jan 2019, 01:28
Antispam: Yes

Re: thermal expansion

Post by kevinarden »

Here are the first run heat solve sif, and the restart linear elastic sif
heat.sif
(3.03 KiB) Downloaded 88 times
le.sif
(3.12 KiB) Downloaded 78 times
Post Reply