Community
CFD Forum
Welcome to Autodesk’s CFD Forums. Share your knowledge, ask questions, and explore popular CFD topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Grey "i", mesh dian, vel rep problems, transient results

16 REPLIES 16
Reply
Message 1 of 17
jrm_1971
515 Views, 16 Replies

Grey "i", mesh dian, vel rep problems, transient results

1. What do the grey "i" icons next to the following mean after meshing? What are the diagnostic arrows telling me?

 

Surface Refinement: False

Gap Refinement: False

Length Scale: 1.4

 

When I hover over Length Scale, it is giving the option for Diagnostics. When I do diagnostics it is showing arrows for potential problems found, the arrows are not normal to the surface. The arrows are shown at the inlet/outlet.

 

My analysis is a 0.406" ID closed conduit with volumetric flow rate and temperature BCs at the inlet and pressure at the outlet.

 

I have refined the mesh for the conduit and fluid (gas).

 

2. Also, when I do velocity traces (center away from the wall) on the surface normal to the inlet, the traces only go so far (long spiral conduit 35 ft lg.). Does this mean the fluid is not going all the way through the conduit? Good engineering sense tells me gas should fill a small diameter conduit quickly. Is there a way to probe individual points on the inlet/outlet for velocity? Is k-epsilon the best turbulent setting for small diameter closed conduit?

 

I have done 100 iterations both steady state and transient, compressible and incompressible. It is turbulent flow with Mach number below 0.5.

 

3. For transient results, shouldn't I be able to move through the VCR buttons forward and backward to see each iteration? It stays stuck at 100 (Last). I would like to see the results (velocity, temperature, heat flux) in correlation with time.

 

 

16 REPLIES 16
Message 2 of 17
Jon.Wilde
in reply to: jrm_1971

1a) As far as I know the 'i' is just for information.

b) The diagnostic arrows are different, I assume you were within the Edge thumbnail of the mesh diagnostics? Check the help as it describes it well, but they are showing you the edges that are the same or shorter than the size you have specified. We often increase this value to reduce the mesh count or avoid issues with tiny edges.

 

2) Has the model converged? Is the mesh sufficient to capture the flow?

ADV4 is helpful for flows in very thin pipe work 

Be very careful with the setup of sub-sonic/compressible analyses, you cannot use the standard BC's, check out the help again but post if you need more information.

Use a cut-plane to probe individual points, hold down the shift key and float the cursor over the plane.

 

3) No, only if you save out results at specified intervals (Solve -> Save intervals). These can quickly fill a hard drive or cause an analysis to become huge so we recommend saving 20-30 or so over the entire duration of an analysis.

Message 3 of 17
jrm_1971
in reply to: Jon.Wilde

1a) As far as I know the 'i' is just for information.

b) The diagnostic arrows are different, I assume you were within the Edge thumbnail of the mesh diagnostics?(I have no idea what Edge thumbnail is. I right clicked the "i" next to the category allowing for diagnostics and clicked the diagnostics button in that dialog box) Check the help as it describes it well, but they are showing you the edges that are the same or shorter than the size you have specified. We often increase this value to reduce the mesh count or avoid issues with tiny edges. (Please provide a link. I feel like being dropped in the forrest without a compass).

 

2) Has the model converged? Is the mesh sufficient to capture the flow? (The analysis converged and the mesh is 1/2 the default)

ADV4 is helpful for flows in very thin pipe work

Be very careful with the setup of sub-sonic/compressible analyses, you cannot use the standard BC's, check out the help again but post if you need more information. (Link please, forrest issue again).

Use a cut-plane to probe individual points, hold down the shift key and float the cursor over the plane.

 

3) No, only if you save out results at specified intervals (Solve -> Save intervals). These can quickly fill a hard drive or cause an analysis to become huge so we recommend saving 20-30 or so over the entire duration of an analysis.

Message 4 of 17
Jon.Wilde
in reply to: jrm_1971

b) The diagnostic arrows are different, I assume you were within the Edge thumbnail of the mesh diagnostics?(I have no idea what Edge thumbnail is. I right clicked the "i" next to the category allowing for diagnostics and clicked the diagnostics button in that dialog box) Check the help as it describes it well, but they are showing you the edges that are the same or shorter than the size you have specified. We often increase this value to reduce the mesh count or avoid issues with tiny edges. (Please provide a link. I feel like being dropped in the forrest without a compass).

 

Are you aware than you can press the small blue '?' icon at any point to be taken to the help?

Or search the help for 'edge diagnostics' and you should find this, the help is a great place to start.

 

The edge and surface diagnostics can be accessed from the meshing window 'diagnostics'. Sounds like you have found this already, there are 2 thumbnails here. Edge and Surface. The help describes what these do better than I did above.

 

2) Has the model converged? Is the mesh sufficient to capture the flow? (The analysis converged and the mesh is 1/2 the default) Are you able to share the support file (cfz)?

ADV4 is helpful for flows in very thin pipe work

Be very careful with the setup of sub-sonic/compressible analyses, you cannot use the standard BC's, check out the help again but post if you need more information. (Link please, forrest issue again).

 

From the help 'internal compressible flow'. It is best here to work on one model at a time, can I ask if you have had training or access to formal training through a reseller/partner?

Message 5 of 17
jrm_1971
in reply to: jrm_1971

I think I see where the misunderstanding is. You good friends on the other side of the pond are calling what we call "tab" "thumb nail" got it. After reviewing the help and tooling around in the program, I am not seeing how to refine the problematic edges and sufaces.

 

Also, what is ADV4? That is not in the "help".

 

From the description from the help for internal compressible flow, I don't believe the hand calculated Mach number of about 0.5 is close enough to the 0.8 recommended in the help. I would appreciate elaborating what is meant by "Be very careful with the setup of sub-sonic/compressible analyses, you cannot use the standard BC's". However, tweeking the problematic edges and surfaces may result in mesh that allows for proper analysis. Please advise.

 

No formal training at this time due to $$$. It's you and me.

Message 6 of 17
jrm_1971
in reply to: jrm_1971

Also, when I hit "Solve" for the transient case, it did not give me the option to save intervals

Message 7 of 17
Jon.Wilde
in reply to: jrm_1971

Before you hit 'solve' but within the first thumbnail (control) of the solve window you should see the option to 'save intervals' as below. This analysis is set to save out results every 50 timesteps (in this case it would be every 50 seconds)

 

Save Intervals.jpg

Message 8 of 17
jrm_1971
in reply to: Jon.Wilde

1. After reviewing the help and tooling around in the program, I am not seeing how to refine the problematic edges and sufaces.

 

2. Also, what is ADV4? That is not in the "help".

 

3. From the description from the help for internal compressible flow, I don't believe the hand calculated Mach number of about 0.5 is close enough to the 0.8 recommended in the help. I would appreciate elaborating what is meant by "Be very careful with the setup of sub-sonic/compressible analyses, you cannot use the standard BC's". However, tweeking the problematic edges and surfaces may result in mesh that allows for proper analysis. Please advise.

Message 9 of 17
jrm_1971
in reply to: Jon.Wilde

OK somehow being able to save the results wasn't available before but now it is.

 

1. After reviewing the help and tooling around in the program, I am not seeing how to refine the problematic edges and sufaces.

 

2. Also, what is ADV4? That is not in the "help".

 

3. From the description from the help for internal compressible flow, I don't believe the hand calculated Mach number of about 0.5 is close enough to the 0.8 recommended in the help. I would appreciate elaborating what is meant by "Be very careful with the setup of sub-sonic/compressible analyses, you cannot use the standard BC's". However, tweeking the problematic edges and surfaces may result in mesh that allows for proper analysis. Please advise.

 

NEW NEW NEW

 

4. Now I am getting the warning below. I am most interested in how to do "3". I am not able to find that option.

warning.jpg

 

5. Please see the image below. The diagnostics is occuring before and  after meshing. The conduit/fluid is split (at the 1/2 line) becuase the geometry upstream will not allow for cutting planes to view the behavior. Is there a way to refine the problematic edges/surfaces? Refining the mesh doesn't fix it.

cfd post.jpg

Message 10 of 17
Jon.Wilde
in reply to: jrm_1971

Good morning,

 

1) t looks as though the geometry here may have some issues, they might be where that split line is but I cannot tell. Where is surface 37?

Find it first. Then when in meshing, switch to 'Surface Selection', Select it, Refine it, then press Apply and Spread Changes. You may also need to fix it in CAD, it depends if the issue is bad geometry or simply not enough mesh to capture it properly.

 

2) ADV4 is Advection Scheme 4. Search for Advectino Scheme, this will come up in the help, sorry for the confusion.

 

3) Start with an incompressible model. What is your maximum velocity?

 

4) The Small Object and Edge Merge Tools are underneath the 'Geometry' tab. If they were necessary, the Geometry dialogue box would likely have popped up when you launched into CFD in the first place. If it ever does, run throuh the first 2 thumbnails, merging edges and then removing small ojbects if necessary. These are only meshing tequniques though, we aren't actually fixing bad CAD.

 

5) Your comment here is not too clear to me. The positioning of the cutting planes within CFD is not at all related to geometry, so you can position them wherever you like, no need for split lines. It looks to me like you need to fix an issue that you have in CAD, keep things simple.

Message 11 of 17
jrm_1971
in reply to: Jon.Wilde

Jon,

 

OK, I am not sure that I have a great solid model for analysis, but it appears to be better. I had an issue with the conduit spiraling around and intersecting itself. Fixed that. Also, the conduit and fluid are now one piece and not cut in halves as shown in the previous diagram. The reason this was done in the past is so the top halves could be hidden and the flow could be visualize all the way through (a disadvantage of using planes is only one section of the spiral can be visualized at a time. Impossible to visualize for a 3D spiral with just planes). The mesh has been refined, edges, etc. corrected through the geometry dialog box.

 

1. I am still getting issues with the traces not propagating through the whole conduit. However, sectioning a plane through the discharge end of the conduit, and probing ("shift" with cursuor over plane), I am seeing the expected discharge velocity. Is there some reason the traces do not propagate through the whole conduit? The mesh is 25% (fine) of the automatic mesh.

 

I did to the Advection 4 which the help describes as best for small closed conduits.

 

Incompressible model selected. The max velocity is about 164 ft/s (at the center of the conduit and zero at the walls as expected ), approaching sub-sonic but not near enough for compressible analysis according to the help.

 

2. In the pre-processor, when solve is set to steady state, a number of intervals are selected to save with respect to iterations. How can I extract time in the post processor with respect to those intervals? For example, if temperature is set to the inlet surface with respect to volumetric flow rate (both are set as BCs at the inlet surface), how can I see how long it is taking for that temperature to propagate through the system? Similarly for transient?

 

3. Heat transfer: I want to see the heat transfer and the time it takes for that heat to transfer once the fluid enters the conduit at a set temperature. I have the temperature at the inlet surface of the fluid inside the conduit set as an initial condition. I have a film coefficient set to the volume of the fluid outside the conduit (as a BC). I have a temperature assigned to the surfaces of the "shell" for the fluid outside the conduit (as a BC). Also, I have tried with just the temperature set to the outside of the shell and starting temperature of the fluid inside the shell without the film/heat generation. Those would be a wild guess anyway. The conduit would be exothermic and the fluid in the shell endothermic and the heat transfer between those is what is trying to be determine. I have tried both steady state and transient. Heat transfer is set in "solve" I am not seeing anything close to the anticipated BTUs/hr of heat exchange from the conduit to the fluid outside the tube. In fact it is close to zero. Where and what kind(s) of heat sink should be set to a tube/shell heat exchanger?

Message 12 of 17
Jon.Wilde
in reply to: jrm_1971

1. This sounds like an issue with the traces now, if the results are good and you can verify this via a cut-plane. Have you tried using an ISO surface to show the uniformity of the flow through the cente of the tube? You can also make this show vectors, rather than just a surface.

 

2. The save intervals for a Steady State analysis are meaninless, as this is just a single point in tmie we are converging on. There would only be a time option to select if you ran a transient study.

You would need to use Initial Conditions on the volume (be sure to swich from surfaces) of the fluid to do this.

 

3.Same issue here I think, do not use the surface, assign the initial condition to the entire volume. If you have a fixed temp outside the shell, this would overconstrain the model and prevent it heating up, is this to model an ambient condition? You could use a film coefficient here (I typically use 5 W/m2/K) at the ambient temp.

 

Does that answer all your questions and help at all?

Message 13 of 17
jrm_1971
in reply to: Jon.Wilde

1. This sounds like an issue with the traces now, if the results are good and you can verify this via a cut-plane. Have you tried using an ISO surface to show the uniformity of the flow through the cente of the tube? You can also make this show vectors, rather than just a surface. I have. The ISO and plane probing looks good. It is just a mystery why the traces disipate through the conduit. Maybe Autodesk CFD does not know how to handle traces in a 3D spiraling conduit?

 

2. The save intervals for a Steady State analysis are meaninless, as this is just a single point in tmie we are converging on. There would only be a time option to select if you ran a transient study.

You would need to use Initial Conditions on the volume (be sure to swich from surfaces) of the fluid to do this. OK thanks

 

3.Same issue here I think, do not use the surface, assign the initial condition to the entire volume. If you have a fixed temp outside the shell, this would overconstrain the model and prevent it heating up, is this to model an ambient condition? You could use a film coefficient here (I typically use 5 W/m2/K) at the ambient temp. I have taken away the overconstrained BCs and initial conditions. Here are the BCs as they exist now: volumetric flow rate applied to the inlet surface, pressure applied to the discharge surface, film coefficient applied to the outside surface of the shell. Initial conditions: Temperature applied to the volume of fluid in tube (this fluid has flow for my study). Pressure of 14.7 applied to the top of the shell side fluid (this fluid is designed to be static). I am still getting heat flux near zero (both in steady state and transient). I would expect it to be in the thousands of BTUs/hr. The heat sink just isn't sinking for some reason. Please advise.

 

Does that answer all your questions and help at all?

Message 14 of 17
Jon.Wilde
in reply to: jrm_1971

I think we may have to leave (1) for now, I am just not sure what the issue is, without seeing the model it is tough to troubleshoot. It does sound as though the flow results are OK though.

 

I would like to focus on (3) as your setup is not quite correct by the sounds of it. I am not 100% clear on what the 14.7 pressure for, please could you expand on this?

Message 15 of 17
jrm_1971
in reply to: Jon.Wilde

I would like to focus on (3) as your setup is not quite correct by the sounds of it. I am not 100% clear on what the 14.7 pressure for, please could you expand on this? 14.7 is in psi. It is atmospheric pressure (or 1 bar as my friends in the UK use). As mentioned, the fluid on the shell side is static (it does not flow). A good example is a process storage tank with a static fluid in it being heated by a coil with a fluid flowing through the coil. I assigned the atmospheric pressure to the top of the static fluid because I have gravity turned on in Solve. As one might expect, the static fluid moves around in the tank as it is heated. Storage tanks, in some cases and in my case, have an atmospheric vent, hence no pressure other than atmospheric. I am under the assumption, to properly model this phenomena, I have assigned gravity and atmospheric pressure.

Message 16 of 17
Jon.Wilde
in reply to: jrm_1971

Ah, I understand. That is something that we cannot model right now, the effect of height of fluid within these models.

 

You can still take into accounf the effect the heat will have on the fluid density, but there is no need to assign a p=0 to the top surface, this just leaves it acting as an opening for flow to enter/exit. Remove the p=0 and it will act more like it would in reality, with fluid unable to escape - maybe apply a film coefficient, just to allow heat to escape?

Message 17 of 17
Jon.Wilde
in reply to: Jon.Wilde

I have your file now, thanks.

 

There are a couple of points to make:

 

  1. To properly capture heat transfer through a solid, you need to have at least 2 elements through the thickness, so it would probably be worth splitting the coil into 2 so you essentially have one coild inside another, this will guarantee a mid-node with no additional meshing work needed.
  2. The same applies to the outer solid of the unit.
  3. You need to have a temperature at the fluid inlet
  4. We probably need to refine the mesh generally - run with those suggestions first and then refine the mesh to 0.7 and see if the results change, if they do, by more than 5%, refine again and continue until the results remain stable.

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report