Register to reply

ANSYS workbench 11 mesh help!

by bgbainbridge
Tags: ansys, mesh, workbench
Share this thread:
Mech_Engineer
#19
May25-10, 03:12 PM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,241
Quote Quote by minger View Post
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.

Quote Quote by minger View Post
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).

Quote Quote by minger View Post
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
#20
May25-10, 09:08 PM
Sci Advisor
P: 1,498
Quote Quote by Mech_Engineer View Post
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
#21
May26-10, 12:58 PM
P: 11
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
#22
May26-10, 01:11 PM
Sci Advisor
P: 1,498
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
#23
May26-10, 01:23 PM
P: 11
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
#24
May26-10, 05:11 PM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,241
Quote Quote by bgbainbridge View Post
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.

Quote Quote by minger View Post
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

Quote Quote by minger View Post
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 accross the elements. Still, he can probably afford to refine it some...

Quote Quote by minger View Post
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.

Quote Quote by minger View Post
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 propogating through the sample thickness more readily (especially after 5 seconds).
minger
#25
May26-10, 07:55 PM
Sci Advisor
P: 1,498
Quote Quote by Mech_Engineer View Post
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
#26
May27-10, 09:38 AM
P: 11
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


Register to reply

Related Discussions
Ansys Workbench Commands (Cable type elements) Mechanical Engineering 8
ANSYS workbench - finer elements gives errous results Engineering Systems & Design 4
Get a copy of ANSYS? Mechanical Engineering 1
Introducing Molecular Workbench Chemistry 0
Introducing Molecular Workbench General Physics 1