Eng-Tips is the largest engineering community on the Internet
Intelligent Work Forums for Engineering Professionals
-
Congratulations waross on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Thermal analysis of bodies NOT in contact
- Thread starter biricio
- Start date
Am I correct in understanding that this box is open to the environment? That makes things a bit tricky if you believe that the bulk air temperature with in the box will change significantly... at that point you're getting into CFD world, or at least with some sort of flow network model (i.e. a can of worms). If you're willing to assume that the bulk air temperature is not significantly affected by the hot cylinder, it doesn't look too terrible...
Well, it looks like you'll have free convection on the exterior of the box - that one seems easy. As long as you're willing to accept that the bulk temperature of the air in the box will not be significantly changed by the hot cylinder, you can also apply free convection boundary conditions to the interior of the box.
That leaves you with radiation transmitting heat between the cylinder and the box - which can be applied with the Workbench GUI in v13. However, you have to make sure that you handle symmetry properly, or you'll generate very wrong results (see RSYMM in the command reference). See the Thermal Analysis guide for more details about using the general radiosity solver.
I haven't actually tested out the new GUI, but just in case it doesn't work for your problem, here is a handy article explaining how to insert radiation into Workbench with command snippets:
Good luck.
Well, it looks like you'll have free convection on the exterior of the box - that one seems easy. As long as you're willing to accept that the bulk temperature of the air in the box will not be significantly changed by the hot cylinder, you can also apply free convection boundary conditions to the interior of the box.
That leaves you with radiation transmitting heat between the cylinder and the box - which can be applied with the Workbench GUI in v13. However, you have to make sure that you handle symmetry properly, or you'll generate very wrong results (see RSYMM in the command reference). See the Thermal Analysis guide for more details about using the general radiosity solver.
I haven't actually tested out the new GUI, but just in case it doesn't work for your problem, here is a handy article explaining how to insert radiation into Workbench with command snippets:
Good luck.
- Thread starter
- #4
Hi, thanks for the answers (especially flash3780).
I have changed the geometry.
The system now is close.
I have a big box with two inside cylinders.
The smaller cylinder has a temperature of 120 °C.
I put a link (RADIATION) to the faces of the cylinder largest and the box.
What's wrong?
Attach file (Ansys WB 13).
Thanks
I have changed the geometry.
The system now is close.
I have a big box with two inside cylinders.
The smaller cylinder has a temperature of 120 °C.
I put a link (RADIATION) to the faces of the cylinder largest and the box.
What's wrong?
Attach file (Ansys WB 13).
Thanks
- Thread starter
- #5
- Thread starter
- #6
- Thread starter
- #7
- Thread starter
- #8
- Thread starter
- #10
First opinion : You must apply convection boundary condition to the outside of thebox. So you must know outside air temperature. and inside wall of the box you can use convection and radiation.
Second : Fill the box in DM with fluid volume for air. and extract the other volume from the Fluid volume of air. In mechanical add air material to the fluid volume. Dont forget to apply convection outer walls.
Second : Fill the box in DM with fluid volume for air. and extract the other volume from the Fluid volume of air. In mechanical add air material to the fluid volume. Dont forget to apply convection outer walls.
- Thread starter
- #12
It's complicated.
From the pdf file I thought it was much easier.
On page 2, under the second picture, is written:
In this case, the center small block (transparent) has a fixed
temperature and is radiating to the middle block (displayed). This block, in turn, radiates to another block (transparent) that encloses it, and the third block radiates to space.
In the article doesn't speak to fill the Box in DM with fluid volume for air.
From the pdf file I thought it was much easier.
On page 2, under the second picture, is written:
In this case, the center small block (transparent) has a fixed
temperature and is radiating to the middle block (displayed). This block, in turn, radiates to another block (transparent) that encloses it, and the third block radiates to space.
In the article doesn't speak to fill the Box in DM with fluid volume for air.
- Thread starter
- #13
- Thread starter
- #14
Ok, so here's the deal. You have an enclosed space. Ansys Workbench is unable to handle convection in enclosed space without using APDL command snippets. A word of warning, though, this is easier with ANSYS Classic.
I recently posted an example of how to do convection to ambient in Workbench here:
In my opinion, modelling pure conduction into the air will not accurately capture the behavior. You need to apply convective coefficients to calculate the heat transfer between the air surface and the air. Mind you, this analysis uses some advanced features.
The model will need to determine the air temperature inside the box. How? You'll need to insert a space node somewhere in the model and attach it to surface effect elements. Ansys will then calculate the air temperature when the model is run. Before you start, have the ANSYS Command Reference, Element Manual, and Thermal Analysis Guide in front of you. The process goes something like this:
1. Create named selections (in Classic they're called "Components") on the interior of the box and the exterior of the cylinder.
2. You'll then need to create a "space node" to convect the convection elements ([tt]N,NODE_NUMBER,X,Y,Z[/tt]). You do this by inserting an APDL Command Object in your boundary conditions
3. Define a new element type, real constant number, and material number
4. Set keyopts 5 to 1 and keyopt 6 to 1; I'd also recommend setting keyopt 7 to 1 and keyopt 8 to 2 in order to apply a parametric heat transfer coefficient. You'll also want to set real constant 13... probably equal to 1/3. The film coefficients may be input as a material property (see the MPTEMP and MPDATA commands). In Ansys terminology, HTC = (film coef)*|T1-T2|^n.
5. Set your element type and real constant number ([tt]TYPE[/tt] and [tt]REAL[/tt] commands)
5. Select the surface nodes ([tt]NSEL,S,NODE,my_NAMEDSELECTION[/tt]) and create a surface mesh, being sure to connect it to the space node ([tt]ESURF,NODE(X,Y,Z)[/tt]).
6. Select your newly created surface elements ([tt]ESEL,S,TYPE,my_TYPE[/tt]) and apply your film coefficients with the following command ([tt]SFE,ALL,1,CONV,1,-my_MATERIAL[/tt]).
The last thing to take care of is surface-to-surface radiation. As of ANSYS 13, it's available within the GUI, although I haven't tried it. The other way is to use command objects. The following document explains how to apply radiation with command objects.
Be SURE to include symmetry (RSYMM) otherwise your results will be incorrect.
Now, there are a couple of tricky things involved. Firstly, the lack of a command line makes it tough to apply all of those boundary conditions. Ansys Workbench runs has to run the entire analysis, which makes testing out commands difficult. Secondly, you can't see the elements or the space node that you create with command line scripts in Workbench. Thirdly, it is not possible to see that your boundary conditions were applied correctly without outputting still images with more APDL scripting.
Again, this analysis would be much easier to do in Ansys/Mechanical APDL. The other option is a CFD analysis... but that's its own can of worms.
I recently posted an example of how to do convection to ambient in Workbench here:
In my opinion, modelling pure conduction into the air will not accurately capture the behavior. You need to apply convective coefficients to calculate the heat transfer between the air surface and the air. Mind you, this analysis uses some advanced features.
The model will need to determine the air temperature inside the box. How? You'll need to insert a space node somewhere in the model and attach it to surface effect elements. Ansys will then calculate the air temperature when the model is run. Before you start, have the ANSYS Command Reference, Element Manual, and Thermal Analysis Guide in front of you. The process goes something like this:
1. Create named selections (in Classic they're called "Components") on the interior of the box and the exterior of the cylinder.
2. You'll then need to create a "space node" to convect the convection elements ([tt]N,NODE_NUMBER,X,Y,Z[/tt]). You do this by inserting an APDL Command Object in your boundary conditions
3. Define a new element type, real constant number, and material number
4. Set keyopts 5 to 1 and keyopt 6 to 1; I'd also recommend setting keyopt 7 to 1 and keyopt 8 to 2 in order to apply a parametric heat transfer coefficient. You'll also want to set real constant 13... probably equal to 1/3. The film coefficients may be input as a material property (see the MPTEMP and MPDATA commands). In Ansys terminology, HTC = (film coef)*|T1-T2|^n.
5. Set your element type and real constant number ([tt]TYPE[/tt] and [tt]REAL[/tt] commands)
5. Select the surface nodes ([tt]NSEL,S,NODE,my_NAMEDSELECTION[/tt]) and create a surface mesh, being sure to connect it to the space node ([tt]ESURF,NODE(X,Y,Z)[/tt]).
6. Select your newly created surface elements ([tt]ESEL,S,TYPE,my_TYPE[/tt]) and apply your film coefficients with the following command ([tt]SFE,ALL,1,CONV,1,-my_MATERIAL[/tt]).
The last thing to take care of is surface-to-surface radiation. As of ANSYS 13, it's available within the GUI, although I haven't tried it. The other way is to use command objects. The following document explains how to apply radiation with command objects.
Be SURE to include symmetry (RSYMM) otherwise your results will be incorrect.
Now, there are a couple of tricky things involved. Firstly, the lack of a command line makes it tough to apply all of those boundary conditions. Ansys Workbench runs has to run the entire analysis, which makes testing out commands difficult. Secondly, you can't see the elements or the space node that you create with command line scripts in Workbench. Thirdly, it is not possible to see that your boundary conditions were applied correctly without outputting still images with more APDL scripting.
Again, this analysis would be much easier to do in Ansys/Mechanical APDL. The other option is a CFD analysis... but that's its own can of worms.
- Status
Similar threads
- Locked
- Question
- Locked
- Question
- Locked
- Question
- Locked
- Question