Troubleshooting Temperature Results in ANSYS Workbench 11 Mesh Simulation

[bgbainbridge]

I have a plate 35mm X 35mm and is about 2mm thick. In the middle of the plate there is a round insert that is a different material that is .1mm thick and 10mm in dia. I am applying a uniform heat flux to the top flat surface for 5sec and then let it cool for another 5sec. When I look at the temperature results on the top surface where the heat was applied there are "hot" spots that show up where it should be uniform temperature, and the edge around the insert is jagged and should be smooth. I am using the default mesh generator, how do I fix this? I am new to ANSYS and FEA so please use layman's terms as much as possible!
Thanks in advance,
Brad B

 

[minger]

I'm a little confused on your exact geometry, particularly the "insert". Can you elaborate a little more or show a figure?

 

[bgbainbridge]

Thanks for the reply,
The first picture is a wire frame, the inserted piece is just in the corner. This geometry was made by making a solid plate then cutting out a slot then the other material was inserted into the slot. Then the next picture is what the results look like.

 

[minger]

Are you reading in your boundary conditions from a separate run? That looks like a problem I've seen when I'm reading in BCs from one mesh, but trying to solve on a different one.

I also notice that the time is 5. Is this a transient, or what are the other load steps?

 

[bgbainbridge]

Yes it is a transient thermal problem, time is from 0-12 sec. The heat flux convection and radiation is applied for the first 5sec and just convection and radiation for the last 7sec.

 

[Mech_Engineer]

What does your mesh look like? How many elements are in it? My guess is you need to refine your mesh, and take a look at your boundary conditions in the cooling phase.

Also you want to make sure the option to "keep midside nodes" is checked, to make sure the elements in the mesh are using quadratic interpolation.

 

[bgbainbridge]

Thanks for the reply, I have tried refining the mesh by telling it an element size, but it does not see to help. I think the most I have tried is ~100,000 nodes and elements.

Where is the option "keep midside nodes" at?

Thanks!

 

[minger]

This doesn't look like a mesh problem. This almost looks like a analysis type, or degree of freedom problem. Even with a really poor mesh, the degrees of freedom will look smooth (e.g. stress analyses with poor mesh refinement still have smooth looking displacements, just not stress values).

I mean, I guess it would help to show the mesh, but also perhaps show a screenshot of your tree/loads/etc.

Also, look through the output file. Workbench can tend do things you might not realize.

 

[bgbainbridge]

I made two other models, one had the insert but the thickness was much larger than it is supposed to be, but the temperature seemed to come out pretty smooth. Another model I made instead of the panel being one large piece with a slot cut out of it I made it into 3 pieces. A large piece with a corner taken out the radius of the insert, then two individual pieces, one to go on top of the insert and one on the bottom. This seemed to work better but then it came up with a contact error and there was a little bit of blotchieness but much better than before.

I think this is what you were asking for

 

[bgbainbridge]

those look hard to see, so here is another try at the screen shots:

 

[Mech_Engineer]

Can you show us pictures of where your boundary conditions are applied? In a cross-section, do you have more than one element through the thickness of your sample (or are they shell elements)?

 

[Mech_Engineer]

those look hard to see, so here is another try at the screen shots:

Note that in the mesh options there is a drop-down named "Solid Element Midside Nodes" with "Program Controlled" selected. To make sure they are used, you simply select "Kept" in the menu.

 

[minger]

With what Mech_Eng said, the application of boundary conditions, particularly in a thermal problem, can be a PITA. I assume that you're applying different boundary conditions on the same nodes/elements?

This may be something better suited for Classic. Thermal analyses, particularly complex ones, are almost always better to solve in Classic due to there being less restrictions and just an overall ease and control.

For example, in Classic, rather than using contact elements (which are almost always the cause of issues) you can very simply tie two regions together using some heat convection coefficient that you either analytically or empirically determine.

One more thing that may help: It may be a little pain, but can host the output file somewhere that we can see it. Pasting it into the post would probably make the thread like 10 pages long, so if you can host it, it'd be preferable.

 

[bgbainbridge]

I think this is the file you wanted, I copied and pasted it from the solution information
http://docs.google.com/View?id=dfwngjv_1fh3rppfv"

The mesh that I have made have had both single layers and multiple layers but it does not seem to make a difference. I don't think I have any boundary conditions on the model. I once put that the edges were perfectly insulated but it did not seem to make a difference in the temperature solution.

Here are the pictures you asked for (I think)...sorry it is so blurry, I only have MS Paint to work with for screen shots

close up on how the disk material is inserted

I hope all of this makes sense, thank you all for your time looking into this for me

Brad B

 

[minger]

OK, now I have a bit better understanding of how the topology looks.

First, yes, you have significant meshing issues. Your part is essentially rectangular, there is no need for poorly generated tets. Break up your part such that you can have a nice hex mesh. This is especially important when you have thin pieces, because you need to maintain cells across the thickness. (Can you post a very close up of the interface region, same view angle, but much closer?).

This will greatly improve the quality of your mesh, and decrease the number of elements.

Now onto the boundary conditions. You are applying boundary conditions, that what your radiation/convection are. When you click them on the tree, the surface/volume will show red in the GUI. Can you highlight each and post the screenshot?

Again, the problem is almost always boundary conditions. You can especially run into problems when running thermal analyses and applying multiple boundary directly onto the solid elements themselves.

When I would do these, I would make a surface selection and overlay thermal-effect surface elements (SURF152 IIRC) over top of them. However, I would still run into problems where boundary conditions meet at corners/edges.

I am also very unsure why there are contact regions. Is the fit loose? If so, how can you be sure what kind of thermal contact coefficient to use?

Show your boundary conditions and then we can talk about that contact region, and redefining your mesh topology.

 

[bgbainbridge]

heat flux

radiation

convection

The model was made using Autodesk Inventor (assembly) and saved as a STEP file (for some reason ANSYS here won't take the Inventor model as is) the pieces don't have any gaps between them

Contact region1

contact region2

contact region3

 

[Mech_Engineer]

I think your boundary conditions and contact conditions are fine (I commonly use lots of contact conditions in my thermal models). I think getting a better hex (brick) mesh will fix your probelm, tets (especially linearly interpolated ones) are prone to error due to their formulation. When paired with the fact you essentially only have one tet through the thickness of your sample, I'm not surprised you're getting errors and non-linearity in the solution.

 

[minger]

OK, first, if your actual model is gapless, then there should be no contact elements for a thermal analysis. I mean, for a structural analysis, then yes, there will be contact phenomenon, but a tight fit part will essentially have no temp drop between the interface.

In order to get rid of the contact regions, you need to create a multibody part. Open up DesignModeler. Shift+click the three parts, right click, and then create new part. This should eliminate the contact regions.

Now, onto your topology. The goal is to create sections that can be easily hex meshed. This will involve breaking up, or slicing your part into pieces that ANSYS can "easily" known that it's a rectangular shape. You're main (large) piece is normally easily swept, but with the cutout, it will help to basically O-grid over the cutout. I have attached images of what the topology should probably look like (black lines are the individual pieces, red should be slice locations).

orgrid.png shows a top view. If you break up your part like then, then the mesher can wrap grid points around the insert while keeping everything in nice blocks. This will allow you to get a nice hex mesh.

topology.png shows an isometric view of the insert area. I would insert a couple of planes in the upper and lower pieces such that the lines remain parallel. That is the small slices in the upper and lower parts are kind of extensions of the thin insert. This slicing can be done in DesignModeler or in the CAD package. In DesignModeler, you typically use extensions from lines or surface to make cut planes, and then use the slice feature (note that bodies need to be imported as Frozen to slice).

As far as the boundary conditions, I am pretty sure that will cause an issue. You're placing multiple surface loads on the same set of elements. As I mentioned, you may have to do this in ANSYS Classic to get a good result.

Lastly, there are plugins for the major modelers to direct imports. Check the ANSYS customer portal for the plugin.

 

[Mech_Engineer]

OK, first, if your actual model is gapless, then there should be no contact elements for a thermal analysis. I mean, for a structural analysis, then yes, there will be contact phenomenon, but a tight fit part will essentially have no temp drop between the interface.

In order to get rid of the contact regions, you need to create a multibody part. Open up DesignModeler. Shift+click the three parts, right click, and then create new part. This should eliminate the contact regions.

You can make a multi-body part for a continuous mesh if you're worried about the contact conditions; I doubt he'll see a difference in the answer either way.

As far as the boundary conditions, I am pretty sure that will cause an issue. You're placing multiple surface loads on the same set of elements. As I mentioned, you may have to do this in ANSYS Classic to get a good result.

Looking closer at the boundary conditions, you have a problem in the heat flux condition you've specified to model the "laser." The flux condition is setting the total heat flow for that surface, irrespective of the radiation and convection conditions at the same surface. When you set the heat flux at the surface to be zero, no heat will pass through that boundary (perfectly insulated), and when the laser is on (12,500) there will only be heat flowing into the sample, not out through radiation and/or convection. In other words, your convection and radiation boundary conditions are doing nothing.

Fixing this for the cooling phase this is relatively simple, you just need to define 2 load steps that define heating and cooling phases of the sample. The heating laser can be defined for load step 1, but undefined for load step 2. This would allow the sample to cool naturally through convection and radiation.

Modeling the laser iteslf however presents a problem since using a defined heat flux at the surface prevents any other surface conditions from acting at that area (when heating or cooling). Instead I think you should use a defined heat flow at the surface (units of W rather than W/m^2) for load step 1, which (I think) would allow vector addition of the heat flow, radiation, and convective effects on the surface. Another option might be slicing a small volume at the surface to act as a volumetric heat source, or possibly using an analog radiation or convection boundary condition which puts in the correct amount of heat (not a very good option IMO).

Lastly, there are plugins for the major modelers to direct imports. Check the ANSYS customer portal for the plugin.

These are only available if he has them in his license.

 

[minger]

You can make a multi-body part for a continuous mesh if you're worried about the contact conditions; I doubt he'll see a difference in the answer either way.

Depends on the accuracy you need. Never use contact elements when they're not needed.

In other words, your convection and radiation boundary conditions are doing nothing.

Also, try turning radiation off and see what happens. I've personally had lots of issues with radiation before, so I know it can be quirky

 

[bgbainbridge]

Thank guys. Here is what I have, I split the geometry into more pieces like you suggested, I am not sure if I did exactly like you wanted me to but it seemed to work! thanks! I did adjust the convection, going from non at all to a extreme "h" value and you were correct, it changed nothing. I tried changing the hetat flux to heat flow but when I did that my temperatures changed drastically so I need to figure out what is going on there if I do have to use that instead.

Here is a close up of the geo:

And a picture of the mesh with the results!

Thanks for all your help,
Brad B

 

[minger]

You still have contact regions. I would highly suggest getting rid of those. You can do that be creating a multi-body part in DesignModeler.

Secondly, your mesh still looks too coarse.

Lastly, one of the most important questions when running any computational problem: What are you expecting, and how do your results relate to it?

What I mean is that your sides remain fixed at 43 degrees. Aside from the sides, your temperature goes from 63-64°. Is this reasonable? Perhaps you have an erroneous BC on your sides? Perhaps you have unit problems?

 

[bgbainbridge]

What it is, I have an actual composite plate with a inserted disk on the side, I am applying heat to it to see how the disk appears at different times. I am trying to model this in ANSYS and get the same results, I am having problems with this as well.
Experimentally I have the panel on a desk, apply heat to it from lamps from the top and record the temperature change of the surface with a camera. I am able to get ANSYS to reproduce the surface temperature curve by adjusting some of the material properties but along with splotchy results the inserted disk does not show up like it is supposed to. The temperature scale I have been adjusting to see if there is a hotter region above the disk (there is supposed to be one) and then compare it to the rest of the plate. I can get results for thin materials like the ones shown here but thicker materials with the disk close to the bottom, I can not see any affect of the disk on the surface like I am supposed to. I think this explains what you were asking

 

[Mech_Engineer]

What it is, I have an actual composite plate with a inserted disk on the side, I am applying heat to it to see how the disk appears at different times. I am trying to model this in ANSYS and get the same results, I am having problems with this as well.

You results at least seem to be smoother due to the better mesh, so one problem down. You can probably afford to refine the mesh some, maybe doing a mesh convergence study is in order.

You still have contact regions. I would highly suggest getting rid of those. You can do that be creating a multi-body part in DesignModeler.

How about this: when (and if) you create a multi-body part for meshing, compare the results to your current ones. I'd bet $0.50 they won't be appreciably different

Secondly, your mesh still looks too coarse.

In defense of the current mesh he should be utilizing midside nodes which probably means it's pretty good right now due to quadratic interpolation across the elements. Still, he can probably afford to refine it some...

Lastly, one of the most important questions when running any computational problem: What are you expecting, and how do your results relate to it?

Indeed, it sounds like he's got experimental results to compare it to, but he should probably look into a simple analytical model as well as a sanity check.

What I mean is that your sides remain fixed at 43 degrees. Aside from the sides, your temperature goes from 63-64°. Is this reasonable? Perhaps you have an erroneous BC on your sides? Perhaps you have unit problems?

It does seem like something isn't adding up... Shouldn't the temperature be somewhat uniform through the thickness of the sample? It looks like he's only solving temperatures in a thin layer at the surface of the model...

EDIT: of course this is a transient model, not steady state. Still, I would expect the temperature to be propagating through the sample thickness more readily (especially after 5 seconds).

 

[minger]

How about this: when (and if) you create a multi-body part for meshing, compare the results to your current ones. I'd bet $0.50 they won't be appreciably different

They might not be too different, but he will have gotten them 10x faster. (his initial mesh had 50k elements, 32k of them were contacts, plus the nonlinearity can increases solution time an order of magnitude. In fact, looking at the output, 85% of the solution time was only the contact elements)

It does seem like something isn't adding up... Shouldn't the temperature be somewhat uniform through the thickness of the sample? It looks like he's only solving temperatures in a thin layer at the surface of the model...

Agreed. It's almost like the interior elements are MESH elements instead of SOLID but I checked the output, and they're SOLID87/90.

 

[bgbainbridge]

Here is different a different simulation, the inserted material is different. On that previous picture, what has happened is that I changed the temperature legend so that I could see the hot spot in the corner that is supposed to be there, I had to adjust it so much the sides look blue because they fall between 63-43°

Thank you for all of your guys' help, I think I am starting to understand things, I can tell I have a long way to go yet