Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Transient Thermal Multilayer Thin layers
I am trying to run a model to simulate the Transient Thermal Temperature profile through a multilayer polymer film though a Heat Sealing process.
The model consists of a Lidding Film (PE) Sealed to a multilayer film, comprising (PE,Tie,PE,Tie, Polymer, Tie, PET).
The thicknesses of the film layers are small compared to the lateral dimensions, and are 15 - 200um, compared to a section of film surface sealed (4 mm wide).
The Seal Bar applies high temperature (140 DegC) to the top surface (lidding) and transfers through to the base web to melt the PE to give a seal.
With an initial temperature of 20 DegC, and Ambient of 20 DegC, some nodes fall as low as 6 DegC.
I understand it may be time step issue, or solver convergence, with a big temperature difference for the high heat transfer rate sealing process.
I would like to understand what parameters can be changed, or mesh refined to get a better solution to this issue.
I have tried both CCX and Internal solver, but Internal oscillates.
I am guessing it is the high aspect ratio solid elements,
Thanks for your help.
The file is too big to load, so any help on uploading the geometry and BC's alone, appreciated.
Nick
The model consists of a Lidding Film (PE) Sealed to a multilayer film, comprising (PE,Tie,PE,Tie, Polymer, Tie, PET).
The thicknesses of the film layers are small compared to the lateral dimensions, and are 15 - 200um, compared to a section of film surface sealed (4 mm wide).
The Seal Bar applies high temperature (140 DegC) to the top surface (lidding) and transfers through to the base web to melt the PE to give a seal.
With an initial temperature of 20 DegC, and Ambient of 20 DegC, some nodes fall as low as 6 DegC.
I understand it may be time step issue, or solver convergence, with a big temperature difference for the high heat transfer rate sealing process.
I would like to understand what parameters can be changed, or mesh refined to get a better solution to this issue.
I have tried both CCX and Internal solver, but Internal oscillates.
I am guessing it is the high aspect ratio solid elements,
Thanks for your help.
The file is too big to load, so any help on uploading the geometry and BC's alone, appreciated.
Nick
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
One way to make your liml file lighter is to clear the result before sending. Right click on top of the solution in the tree menu and select clear.
Regarding your model issues I would start with a 2D section of the zone of interest (heated) just to check parameters.
See if you can attach the file.
Edit: I send how I would start facing the problem starting with 2D and confirming temp profiles and time needed to heat properly without burning anything.
I don't expect the high aspect ratio of the elements or the model would be a problem, at least not if the heat is mostly flowing either normal or parallel to the layers.
I agree with disla about starting with a simpler model. Then you can get these issues resolved faster.
I will try a 2D cross-section first.
I am getting quite good correlation between my 1-D FD model and the FEA model, so I have no problem with accuracy etc., but I would like to see the transient.
I'll let you know how the 2-D model looks before trying the larger 3-D model.
Refining the mesh helped a little, and I don't think the minor instability will affect the overall result.
I do have another issue, though.
I want results for selected nodes, and I have named them, and can get results in a table.
However, the Node numbers in the table do not match the Node numbers selected in the Named Selections !
When I click on the Profile Group, numbers are shown for the selected nodes, but the tabular results show different numbers.
Also, the three nodal results (for the width ?), are shown, whereas I really only want the equivalent nodal, centre (plain strain equivalent) temperature.
Is it possible to strip those additional results out ?
Also, I am writing an Excel macro to transpose the tabular results into columns. Are there any easier ways to export the data in a more manageable form ?
I have attached the stripped down model without results.
These are located at different points in the model.
Perhaps the Names Selection needs to be updated for model refinement ?
Ccx and Mecway expands shell elements to solids creating new nodes.
Regarding the node selection or removal, you could activate the coordinates check button and postprocess filtering by coordinates and then sorting by Y coordinate.
¿Which "similar instability" do you refer to?. At first sight the process seems pretty smooth.
Maybe if you ramp the temperature from 0 to 140 to avoid a discontinuity in t=0s.
Heat transfer coefficient also goes suddenly from 5000 to 50.
Edited: Take a look at this forum regarding the proper mesh size/time step relationship on heat transfer by conduction problems.
L=sqrt(k*t/(rho*Cp))
https://www.comsol.com/forum/thread/16808/weird-problem-in-comsol-tmeperature-measurment?last=2016-10-21T13:43:33Z
*NODE FILE,OUTPUT=2DYour model has element sizes of 500um width. According to the formula your mesh wouldn't be able to capture the cooling process correctly. Maybe it is the origin of the instability you mention.
L<sqrt(k*t/(rho*Cp))
PET
Mesh Size < 74,54 um
PELD
Mesh Size < 76,86 um
HP
Mesh Size < 93,10 um
TIE
Mesh Size < 93,68 um
When changing to just 2D node output, the results matched the named nodes.
Hi disla, I understand the mesh aspect ratio is high, and I don't really need that large a model for the, essentially 1D phenomena I am trying to model.
I will reduce the geometry.
Essentially, it is a high aspect ratio problem, as the thickness is small compared to the lateral dimensions. The film in is 500um thick, but 100 - 200mm L x W.
There is some heat transfer to the edge, but most of the heat transfer is 1D.
I am still trying to get the appropriate HTC coefficients for the process, but the relative results I am getting will give an indication of what is happening.
Thanks for your help.
Now I get why you talk about "similar instability" .
Looking at the base node where the heat transfer rate is higher I can see the oscillations. Looking at the period between them, it is clearly related with the time step which in my opinion is unable to capture the phenomena. It is Ok far away where heat flux is lower but not there. One appropriate ratio L/dt would be 200 which imposes a quite small mesh size and dt of 1um/0.005s.
You can also prepare a non uniform mesh grid with more elements in the area of interest.
See Attached results.
I had used the data remote from the instability for the analysis I was doing.
I can see the improvement in the models and step sizes you used.
Thanks for your help.