ANSYS workbench 11 mesh help!

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

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.