CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Generating Mesh for STL Car in Windtunnel Simulation (https://www.cfd-online.com/Forums/ansys-meshing/67869-generating-mesh-stl-car-windtunnel-simulation.html)

tommymoose August 29, 2009 01:30

Generating Mesh for STL Car in Windtunnel Simulation
 
This will be a relatively lengthy thread, so here is some background. I'm working on a senior capstone project in the area of vehicle aerodynamics. The product I'll eventually be designing will be based largely on proving concepts and refining through CFD using Fluent. I downloaded an STL file of our test-car, a Porsche 997 GT3 RS, from a CAD data site. I'm using ICEM for pre-processing as my professor told me it is the best program we have for the job. I have quite a bit of screen-time using ANSA for surface meshing from a past internship, however working with ICEM is a completely new experience. The rest of what I'll post is questions I've had along with answers that Simon P. has been nice enough to answer. I'll continue to build on this thread as I have questions, hopefully get answers, and maybe some other students will be able to learn from it too!



Me: If I'm going to run the Octree mesher, do I need my entire model to be all red lines (connected surfaces) or can it approximate enough based on the surfaces?

Simon: No, you don't need all red lines. The mesher will still walk over gaps smaller than the mesh size even if you have yellow lines... However, having two yellow lines close together may cause the mesher to refine down and then give leakage, so I recommend deleting one of the two edges... Or just delete any curves that do not capture a feature that interests you (don't forget about points). Some items may end up with the same volume on both sides, this will cause them to disappear unless you mark them as internal walls in the params by parts popup... Marking them as internal walls will allow the mesher to keep them (like baffle surfaces) even if you car leaks...


Me: Is there a way to hide sections of the model so that its easier to view and move around? My STL file came in as one part, so I don't have the option of hiding parts yet and I'm trying to pick and choose to separate out parts.

Simon: You can blank surfaces, etc. but the easiest way is to simply put things into parts and then turn off parts you don't need to look at any more... You can group parts into assemblies to make it easier to turn off groups of parts, etc.


Me: Can you recommend a plan of attack for getting this geometry prepared to a state that I can run the Octree mesher? All I need are the exterior surfaces, and its going to be closed-grill, so no engine bay prep.

Simon:If you don't need the internal stuff (seats, etc.) just delete what ever you can. If something will cause any trouble or is difficult to delete it, then don't worry about it. The octree mesher refines and fits to all the geometry before it does the flood fill to determine what you want to keep, so... Set large sizes on interal items so it won't waste time refining for them. Removing items saves both the hassle of refining and the time to fit to the geometry... Then, if it looks more or less closed and you are near the end of the day, may as well set it off meshing when you go home... In the morning it may be done... If parts are missing, try the "internal wall" setting. If you get a leakage message, you can usually see where it is happening. It may be something you will want to fix or perhaps you just need to delete a curve or make the mesh size bigger.

My usual plan of attack is just to break the geometry up into parts (wheels, hub, windows, mirrors, bumpers, etc.) Along the way you are investigating the model, deleting bits you don't need, etc. If you see holes, close them. I acutally tend to convert the geometry to mesh and use the mesh editing tools to close holes because they are just a bit faster than the faceted repair tools, then I delete the geometry and convert the mesh back to facets (geometry). THis is all under the edit menu. I get the geometry more or less closed... (If you are starting with the nice mesh you got out of ANSA, you have already done this work and can probably just go right to meshing). Then I build a box around it, intersect the tires with the road, create a material point, double check my Part and Global parameters, and mesh it... Then I often delete the octree volume mesh and check the surface mesh for multiple edges, single edges, etc. It is easier to edit without the volume mesh, plus the Octree mesh isn't my favorite. Then I close and repair anything that I find. Then smooth like crazy with the laplace option. Then I do a tetra fill with deLaunay (I like the TGlib beta option). Then I run prism. Then I smooth with prisms frozen... Run final diagnostics and checks... Out to solver.

tommymoose August 29, 2009 01:36

Me: I spent a few hours simplifying and grouping the geometry. Since it all came from an STL file, it came in as one part and I couldn't separate out different surfaces. I had to run the "build diagnostic topology". Once I did this it added curves and broke up the surfaces enough to sort. I have more time than I do troubleshooting skills, so I went ahead and deleted pretty much all of the interior geometry. The wheels were a mess, so I deleted them and will remake a simplified version of them in solidworks and re-import as an iges (as I understand octree can handle STL and IGES in the same project).

I was deleting surfaces all along, and I'm not sure if I'm supposed to go through and delete all of the curves and points too. I was thinking I could delete all of them, and then re-make the important ones via "extract curves from surface"... would you recommend this?

Simon: Doing the wheels in IGES and importing them is a good idea, and yes, it is no problem to combine geometry formats in ICEM CFD.

Also, now that you have deleted all the interior surfaces, you can go to the geometry tab and delete curves, select all. Then delete points, select all. Then recreate these with the build topology tool. Build topo tool will create one curve between surfaces. Extract curves from surface will create a curve around the perimeter of each surface which usually means 2 curves between adjacent surfaces... Therefore, Build diagnostic topology is better.



Me: I'd like to simplify the geometry a bit... for example I deleted the emblem on the hood and now there is a hole so I want to fill it. However, there are no curves on the hood surface because they all belong to the original import part still, and I can't convert to a mesh to clean up the geometry (because I'm already in STL). Should I recreate curves on the surface like I mentioned above, then fill? What would you do?

Simon: For operations like closing the hole in the hood, you have lots of options. You could build topology and try to close the hole after it extracts curves. You could also go to the geometry tab and look for the faceted repair tools. There is one that lets you select the facet edges and fill to close the hole. If I had only a few issue, and I had already sorted out a bunch of sizes, etc. that is what I would do. If I had a ton of faceted repair work to do and didn't mind giving up on any geometry settings, I would use the Edit menu to convert facets to mesh... then I would use the edit mesh options (with surface projection off for closing that hole) to repair a bunch of issues. Then, you deleted the faceted geometry and go back to the Edit pull down to convert the mesh back to facets. During this process, it will ask if you want to build in sharp features, this is like build topo, so say yes. Then it will ask to merge close nodes, I usually say no.


Me: In PowerFLOW, I believe the volume mesh generation and simulation are all completed after the job is submitted to the cluster. In contrast, in ICEM, I generate the volume mesh first and then submit the simulation. Does this lead to memory issues when generating the volume mesh on a big file like this if I'm working on my home computer? I have access to a cluster and realize I may need to use it for the simulation, but is it common to use it for the mesh generation? For reference, I have a 2.4gHz Quad-Core processor w/ 4GB of RAM... a decent machine but I'm not sure what its capable of doing in ICEM.

Simon: If your machine is 32 bit, then it can really only use about 2Gigs of memory for any operation... With ICEM CFD, that would limit you to about 12 million cells (uncut) by the time you toss out all the junk, etc. that is about 6 to 10 million... If you need much more, you can chop the model up and mesh it in sections...

If your machine is 64 bit, then you have access to more of the 4 gigs and your model size goes up linearly.

You may also benefit by using ICEM CFD hexa to mesh the tunnel and then just having tetra in a smaller region around the vehicle. You could then merge the two zones...

tommymoose August 29, 2009 01:42

Just a quick question on the geometry preparation before I get into the meshing questions. After converting facets to mesh, cleaning up the mesh, then converting mesh back to facets, do you delete the mesh so that all you have left going into the mesh computation is surfaces, curves and points? During the conversion process, it leaves a shell mesh on my screen which I'm not sure I want.

<Simon>Right, I convert the facets to mesh, fix the mesh, then delete the geometry. Then convert the mesh to facets and delete the mesh… then apply mesh parameters to the geometry, etc. and generate a mesh on the geometry. The exception is if your surface mesh from the facets looks better than you would get if you generated it in ICEM CFD… In that case, just use it as a surface mesh and generate the volume mesh “from existing mesh” with a bottom up method like DeLaunay Tetra.


I have 4GB of RAM on my 64-bit Vista OS, so I should be able to make use of all of it (whatever Vista isn't hogging that is :p ). I ran an initial mesh which came out to about 12.5MM elements. During the process of making it, I developed some questions. Because I have no idea really what my max element size or height, or width, or deviation, etc. should be, I set the maximum to 0 so that the program could decide what is best (per tutorial). I would have expected the mesh elements to get larger the farther from the surfaces, but it seems to be the same throughout. I didn't specify anything for any surfaces, mainly because I don't know whats important. Do you have any rules of thumb for choosing global and surface mesh parameters on a car? I know that in PowerFLOW, separate parts would be made of peices of surfaces that we would want higher resolution (I.E. windshield-cpillar-glass transition). Should I make areas like this (front lip) its own part so that I can assign a more fine surface mesh, or does that not really matter?

<Simon>I usually set the Max size to something large (and a power of 2) like 512 or 1024. Setting it to 0 should have worked if you had set sizes somewhere else, but if you don’t set any sizes, it probably poped up something asking if you wanted to set an auto size? This would divide the distance between Min XYZ and Max XYZ by 1000 and use that for the Max size. And yes, breaking the model up into parts is a good first step. Then you can easily adjust the mesh size to refine that front lip part, etc.


You said that you like to delete the octree volume mesh (essentially using it as a surface mesher?), and then do a Delauny off of that surface mesh. To save time, would you make the bounding box very tight around the vehicle so the computer doesn't have to spend time meshing the full volume of a "tunnel"? Then once you delete the volume mesh, you could create the tunnel you'll be using to solve with and then use Delauny or Advancing Front to fill in the volume?


<Simon>That depends… If the car were not touching the tunnel, then yes, I would do that. But if it were touching, then you would have the hassle of connecting all the surface elements where the wheels meet the road. Often I would just set a really big max size in the tunnel so it doesn’t waste time doing a fine mesh. I suggest a method for dealing with tunnels using the merge option.


Meshing a very large tunnel has its drawbacks in the time it takes to mesh and also solver. PowerFLOW would mesh progressively larger zones the farther from the vehicle, so that the outer regions would only compute every 64 times or something like that. Is there something like this in ICEM/Fluent?


<Simon>If you have access to TGrid, I could recommend taking the surface mesh of the vehicle from ICEM CFD and sending it to TGRID to use their “Hexa Core” option. This is a common process with our racing customers… And actually, I heard recently that UAV was doing it that way also. This will create the hanging nodes that you want and actually can give Cartesian hexas right to the wall in many cases.


As you can tell from the image, I got some leaking. I'll check for holes/gaps and close it up better before next try. I can't seem to find the internal wall option though. I would like to make the front lip jut down as a single layer surface, or a thin one at the most, but I imagine that without a setting like single-sided-wall or internal wall the mesh will ignore it and mesh right through it?


<Simon>Right, without the internal wall option, that front lip will just disappear (the mesher will think the surface was a mistake and do you a favor by removing it.) The solution is to look again for that internal wall option ;^). Go to the Mesh tab, 2nd Icon is “Params by Parts”. This menu allows you to set Mesh parameters by parts (as the name implies). Move over to the right and you will see checkbox options for “int wall” and “split wall”. I think you want “int wall”.


tommymoose August 29, 2009 01:46

Me: I'm having some trouble with the mesh, so I'll explain what I did. I converted the facets to mesh, cleaned it up and made it air-tight as far as I can tell. Then I converted back to facets and deleted all of the mesh shells, lines and points. At this point all I have left is the facets, and the iges geometry I imported (wing and wheels). When converting back to facets I built in the sharp features which left green curves all over the part. I followed your guidance and kept the tunnel full-size, put max element size to 512, and specified smaller sizes on the individual parts. I pretty much put 0.25 on all of the critical areas and 1 on the rest. When I meshed, the only thing it ended up meshing were the wheels, wing, and front-lip (which was set to interior wall), along with some random facets scattered around.

On a second try, I did the same thing, except this time I ran topology first so that it deleted the green/non-associated curves and replaced them with yellow and red curves. I experimented with different tolerance settings, but curves keep showing up where I wouldn't expect. I went ahead and meshed with the same parameters.

On a third try, I increased the global mesh size to 10, hoping it might mesh over any holes I could have left. I got similar results.


Simon: I can guess that you have the same volume material on both the inside and outside (you have an opening some where) and octree tetra is just ignoring the surface mesh on those parts because they are within the same volume.

1) You could force it to show you the hole by putting an ORFN material point in the CAR. When the flood fill runs and finds the inside, it will give a message about "Fluid.0 can reach ORFN.1" It will show a jagged line connecting the elements along the path between these two material points... THe line wil go right thru your hole. You will be able to close the hole or just keep the surface mesh...

2) Or you can trick it into keeping the surface mesh by going into the mesh tab => Params by parts, and turning on the "int wall" option for everything.

tommymoose August 29, 2009 01:49

Me: That first method worked to show me the hole! I meshed it overnight and when I woke up the jagged line went right through the seam between the tail light and quarter panel. If there are more than one hole will it show me that or does it only do one at a time? It's hard to detect this prior to volume meshing... Is there a way to show open holes before hand? Certain build topology settings?

Simon: The first method will show you only one jagged line (the first path of leakage)... but all the single edge holes will be outlined in yellow (single edges diagnostic). You can also turn on this diagnostic at any time by right clicking on "shells" in the model tree and choosing "diagnostic", then check the "single edges" box. (Note; don't leave this on all the time since it also limits selection to single edges...) I guess it can miss holes with double edges (like if you were running a model full of 3D parts and a whole 3D part (like the door) was missing, but it doesn't sound like you have that situation.


Me: Am I better off closing the hole or keeping the surface mesh? I'd guess for what I'm doing (deleting volume then delauny) I could just fix the surface mesh manually after I delete the volume... Yeah?

Simon: The decision about closing the hole (geometry level) or fixing the surface mesh is very subjective. If I have just one little issue or just a few issues with the mesh and regeneration would take over night, I would probably just fix the mesh (not remesh the whole thing). I might also fix the geometry if I thought there was a chance of remeshing later (refinement study or somthing). But if you see a bunch of problems that would be easier to fix at the geometry level, or missing important geometry detail, or mesh editing would take too long relative to remeshing, then I would work on the geometry level...


Me: I feel like there has to be some consequences of option number two. It seems too easy to just set everything as an interior wall? It may generate a nice surface mesh but the holes will still be intact... Is that a problem with delauny-ing from it?

Simon: Number two isn't awful... You end up with fluid inside and outside. This is a lot closer to real life and you will see that there is not much motion of the fluid in the vehicle unless you have an interesting gap that rams air inside... I guess you would be wasting computational time solving that space... Delaunay also doesn't mind it... (Delauany hates holes in the envelope, but holes inside are just baffles.)

But if I did #2, it would just be an intermediate step, like keeping only the surface mesh after floodfill. ICEM CFD mesh editing has lots of ways for me to diagnose and fix up my mesh... Sort out single edges, investigate multiple edges (make sure they are appropriate), sort out non-manifold verts, etc. and then run delaunay...

PSYMN August 29, 2009 11:27

Thanks.
 
Thanks for posting this email conversation for others...

Simon

tommymoose August 29, 2009 15:31

1 Attachment(s)
Thanks for all the help!

I plan on using the car for multiple runs, so I closed up those holes at the geometry level and remeshed last night. It all looks pretty good so far! I'd like to delete the volume mesh and work with the surface mesh to make sure its fully sealed like you said. After that I'll create a Delauny mesh from it. I was planning on turning shells off, volume on, then deleting visible. I'm having trouble deleting the volume mesh though... only because when I go to turn on the volume mesh the application just thinks. I gave it an hour with no results. Is there a way to delete the volume mesh (without deleting the surface mesh) without actually turning it on to view?

Here is an image of the shells in wireframe... anything that looks solid is really just meshed at 0.25. The rest at 1, with the tunnel set to 0 (max global size = 512).

PSYMN August 29, 2009 16:01

I almost never turn on the volume mesh in ICEM CFD...

Instead, go to Edit mesh => Delete

It will say "select elements" and a tool bar will pop up...

The last icon in the tool bar is "all volume elements".

Click it.

Simon

PSYMN August 29, 2009 16:02

Fun with Prism...
 
Next will be fun with Prism... ;)

tommymoose September 3, 2009 00:05

That sure worked... Thanks!

When inspecting the mesh, I check off single edges in the diagnostic menu, but it's still hard to see... The yellow doesn't jump out because all the parts and curves are different colors. What's the best way to go about this and clean the surface mesh up? If I'm going to do a Delauny mesh off of this surface mesh, it should be a closed shell right?

If I want to have the part of the tunnel my tires intersect be a sliding surface, do I need to do anything different at this stage? Tunnel labeling? Also, should I put a symmetry plane in now? I could utilize the symmetry on some runs but will also have asymmetrical runs. Thanks!

PSYMN September 3, 2009 11:45

...
 
Using Shell => Diagnostics or using Edit Mesh => Check Mesh, you can get to a situation where you only see single edge shells. I usually do it thru Check mesh, create a subset and then add a couple layers to the subset so I can understand the problem.

Delaunay can handle openings within the envelope. It will treat those as internal baffle walls and add volume mesh on both sides. It cannot accept holes in the envelope. It will fail and should create an error subset to show you why.

I would create a curve of intersection between the tires and the road (Geometry tab => Create curves.) You may even want to take it a step further (and use the geometry tools in ICEM CFD or perhaps modify the original IGES wheel before importing) to remove any cusp features where the tire meets the road… This will save meshing hassle later on.

Even if you plan to run asymmetrically, you can take advantage of symmetry while meshing. This makes everything faster because you are only meshing half the model. In the end, you can easily copy-mirror the mesh if you needed a full model for the solver.

tommymoose September 7, 2009 21:33

I'm cleaning up the surface mesh I have now before Delauny meshing... I imagine having a clean surface mesh will lead to a cleaner volume mesh?

What is an acceptable level of quality in the histogram? I've heard people say nothing less than 0.3, but for complex geometry this would be difficult.

When cleaning up the worst elements, I'm going "mesh -> shells -> color by quality" then taking care of the worst ones I can see. I can't find a way to have it display elements of quality < X though... Its hard to spot the tiny/thin bad elements manually, so is this possible?

Thanks alot!... I'm moving through this slowly but surely...

PSYMN September 8, 2009 11:17

Sure, there is definitly a better way.
 
Yes, of course, a better surface mesh leads to a better volume mesh.



I go to the smooth or mesh quality and run my check… This creates a histogram in the bottom right corner. You can adjust the range of the histogram if it is too hard to see the lowest columns. Left click on columns to display the mesh from each column on the screen (track lightly as this may be memory/display intensive). Right click on the histogram to create a subset of the elements in the highlighted columns… Then go over to the model tree. Under the mesh branch, you will find a subset branch. Turn off the shells and other ways mesh is displayed and just display the subset. These are the elements of that histogram bar (or however many bars were highlighted when you created the subset). Right click on the subset and “add to subset”, this will add attached surface elements. You can have other options if you chose to "modify" the subset. "Add to subset" a few times until you get enough elements to understand the situation. Most can be fixed by either adjusting node projection, merging away sliver nodes, splitting edges, or swapping edges. Move nodes may also help.



After fixing up an area, right click on subset again and choose "remove from subset", then remove the area you repaired. This just helps to clean up what you are looking at so you can focus on the remaining clumps.


Removing a subset does not delete the mesh, it is just a display trick.


I usually also use Check mesh and create subsets to find single and multiple edges, non manifold verts, etc.


After you have made all your fixes, run the smooth again and create another histogram...


This may be a somewhat iterative process, but don't let it make you crazy. There is always a worst element and you may need to say, "that is just the best element that will fit in there due to my geometry constraints". Your solver can handle it (most of the time). If 0.3 is the goal for Fluent, you can probably handle a few between 0.01 and 0.3.



Also, when you get to Prisms, expect they will have lower quality, but down to 0.01 is usually fine for Fluent.

tommymoose September 8, 2009 13:12

Thanks for the detailed explanation Simon!

tommymoose September 9, 2009 18:32

There are ducts in my front-lip that I want to be open on the initial simulation, however I created and surface meshed a surface so that I can make them closed on later runs. How can I get the mesher to ignore this surface when I run the Delauny volume mesh?

I unchecked the part so it was hidden and changed it back from int-wall to a regular surface in the part mesh setup. I was hoping it would just mesh through it, but in the summary in the text-area it said a certain number of volume elements belonged to it or something. I tried to turn on the volume mesh to see how it turned out, but it was taking forever (then my computer auto-restarted... stupid windows updates). Just wondering if there is an easy way to have the mesher ignore certain parts :) Thank you!

PSYMN September 10, 2009 14:22

I can't think of a good title
 
Once you get to Delaunay, you are just meshing from the surface mesh. If you want it to ignore a certain surface mesh area while meshing, the only thing I can think of is to simply delete the surface mesh in that part…

On the other hand, you could keep that surface mesh for Delaunay, it would force nodes to line up across the opening which is not a bad thing. Then set up the bocos to tell the solver that the surface is just for post processing (not a wall) or make it a wall to simulate blocking the hole without needing a remesh. You could also delete the surface tris before running in the solver if you would prefer.

Also, never turn on all the volume mesh for a model this big… Unless you are in cut plane mode…

tommymoose September 14, 2009 22:45

I've created prisms now. I decided to go with the standard settings and 4-layers worth. After that, I froze them and smoothed the rest of the mesh with 25 iterations up to 0.5. I still had about 3500 elements between 0.0 and 0.05 when that was done so I unfroze the prisms and re-smoothed 5 iterations worth up to 0.2. This got it down to ~900 elements between 0.0 and 0.05. Overall though there are thousands below 0.3, but it makes up about 0.5% of my elements.

Does the specific number of low quality elements matter, or just the percentage of them to overall? Will the simulations fail, or can I just expect some diminished accuracy when I have a lower quality volume mesh?

Assuming I can get through that, I'm now trying to setup the boundary conditions for the output to Fluent. There is the symmetry wall which I'll be using. I notice now however that I just have a part "Tunnel" but it is not broken up into the floor, inlet and outlet. Can I do this retroactively or must it be done before the volume mesh?

The tutorials don't have much specifics on setting up the boundary conditions. How would I go about setting up the sliding floor? Also, I think that standard practice is to use a pressure differential between the inlet and outlet, but how do I determine what differential gives me the fluid speed I want? Thank you very much for answering these uber-noob questions :o

PSYMN September 16, 2009 17:30

Answers
 
1)You may be able to get better quality, so perhaps you shouldn’t give up, but rather look to see where and why you are getting these poor elements. But yes, they are not the end of the world. Rather than focus on quantity or percentage, I look at how bad they are and where they are. If they are in an area of critical interest or where a lot is going on, they could reduce your accuracy or cause divergence.
2)Yes, you can get the mesh to change to match geometry… The first step is to adjust the geometry parts. Put the inlet surface into the INLET part, etc. Setup your geometry the way you should have in the first place. Then go to Edit Mesh tab => Repair Mesh => Associate Mesh. Use the select items in a Part option to select the TUNNEL part, or use the Select all surface mesh elements… This will use a normal ray from the center of each selected element to the nearest surface and take the part from that surface. Then you can proceed to apply bocos.
3)For the moving floor, set it up as a viscous wall, but then apply a velocity to it in Fluent. I usually use a velocity inlet and a pressure outlet which makes it relatively easy to match the inlet velocity to the moving wall floor. Others in the CFD-Online community may have other suggestions for how to best setup Fluent bocos for external aero. Ask that question separately in the Solver users section.

tommymoose October 10, 2009 16:47

1 Attachment(s)
I've read on here that for improved accuracy, you want to keep the volume mesh very fine in the wake-zone behind the car. For the zones around critical parts of the car (lip, a-pillars, wing, etc) I can just set the mesh parameters to be finer (0.25 compared to 1 for the rest), however when there is no part that the area corresponds to, I'm not sure what to do.

One thing I'm trying is to "adjust mesh density" along the symmetry wall right behind the car. I'm hoping the fine volume mesh that is created from that surface will carry around that whole area. Its hard to verify what the volume mesh looks like though, as the computer is unable to display it.

Any ideas? I'm attaching a picture of what I have right now. I'm going to run my Delauny mesh off of this (octree mesh with volume deleted). Can you comment on how the density behind the car looks? Should it be finer? Thanks!

PSYMN October 10, 2009 21:04

Create Mesh Density...
 
You could work with the surface width parameter, etc.

But what you really want to do is "Mesh tab => Create mesh density". Once there, look into the help or search the tutorials for instructions, but basically, this lets you create a density region and then set the "max size" within that 3D volume region. you can create boxes or lines (cylinders) or points (spheres). You can use points to help you place it (easier to select geometry) or you can place it around an existing geometry and move it into place (right click on density in the model tree to modify). Some people put several nested density boxes to help the mesh transition in the wake or combine it with a "width" setting of 3 on the surface of the vehicle.

You may also want to look at my hints and tips pdf...

ftp://ftp.ansys.com/outgoing/simon/ICEM_Tips2008.pdf

tommymoose October 15, 2009 21:03

1 Attachment(s)
Thank you for those tips and that link Simon. I was able to use the cars rear-end geometry to click around and create enough of a volume... then translate back behind the car for the density region. I'm attaching a picture.


I have a few random questions I've accumulated about meshing in ICEM. I'm significantly slower when surface mesh editting in this program than I was in ANSA, and I have to believe some (if not all) of it is due to not being aware of the rules and shortcuts. Here are a few questions hopefully you can help me out with :)

If I'm working on the surface mesh, the merge node tool seems to work inconsistently. This has to be one of the tools you use most, right? (I know in ANSA it was huge for me) Sometimes it'll paste one node to another and collapse an element (which is what I'm going for), but other times that wont work and I'll need to delete elements then create new ones, which takes much much longer. Any idea why this is?

What do the colors of the dots that show up when a node is clicked on indicate? Sometimes they're green and sometimes pink...

When creating elements, merging nodes, or any task that involves doing something repetitive, going back to the menu to hit "apply" every time is inneficcient. In ANSA I would click node 1, click node 2, then middle click, DONE, and move on the next node which would usually be around where the cursor was. I could fix up ~50 elements in about 10 minutes. Between the previously mentioned inconsistent merge problem, and this one, it would probably take me about an hour. Is there a shortcut to "apply" that I'm missing?

Regarding mesh quality - You smooth and correct after the octree mesh to get the best quality surface mesh you can get. Then comes Delauny. Then prism. Do you do manual volume mesh editting between in the middle of or after those last two steps? Just global smoothing w/ laplace?

Thank you so much for filling in the blanks I have!

tommymoose October 15, 2009 21:09

1 Attachment(s)
By the way.... my insurance premium thanks you for helping me go about development of the front-aero package via simulation. My driving record suffered a little bit this past week in the process of debugging the rear active wing :p

Hendster October 16, 2009 03:39

Quote:

Originally Posted by tommymoose (Post 232117)
I've read on here that for improved accuracy, you want to keep the volume mesh very fine in the wake-zone behind the car. For the zones around critical parts of the car (lip, a-pillars, wing, etc) I can just set the mesh parameters to be finer (0.25 compared to 1 for the rest), however when there is no part that the area corresponds to, I'm not sure what to do.

One thing I'm trying is to "adjust mesh density" along the symmetry wall right behind the car. I'm hoping the fine volume mesh that is created from that surface will carry around that whole area. Its hard to verify what the volume mesh looks like though, as the computer is unable to display it.

Any ideas? I'm attaching a picture of what I have right now. I'm going to run my Delauny mesh off of this (octree mesh with volume deleted). Can you comment on how the density behind the car looks? Should it be finer? Thanks!



hi, tom. i'm very interested on what u learn but i'm in the beginner level. i will do the job as like as u do to finish my project. i want to know how u can design the porsche, i mean what software u use to design it. thanks for ur answer, i'm waiting...

tommymoose October 16, 2009 13:21

Quote:

Originally Posted by Hendster (Post 232848)
hi, tom. i'm very interested on what u learn but i'm in the beginner level. i will do the job as like as u do to finish my project. i want to know how u can design the porsche, i mean what software u use to design it. thanks for ur answer, i'm waiting...

I downloaded the 3D model from a website. I forget which model I chose exactly, but we compared the model to the real thing and tried to choose the most accurate. I substituted in our airfoil blade, remodeled the wheels in solidworks and replaced the ones in the model (too complex), and did a ton of manual cleanup. Hopefully with the rest of the posts in this thread you can complete your own project :)

This might have been the model I downloaded - http://www.the3dstudio.com/product_d..._product=28866

rwryne October 16, 2009 13:23

Quote:

Originally Posted by tommymoose (Post 232817)
By the way.... my insurance premium thanks you for helping me go about development of the front-aero package via simulation. My driving record suffered a little bit this past week in the process of debugging the rear active wing :p


Did you try to explain you were speeding...for science?!?

PSYMN October 16, 2009 15:30

Answers...
 
Quote:

Originally Posted by tommymoose (Post 232816)


If I'm working on the surface mesh, the merge node tool seems to work inconsistently. This has to be one of the tools you use most, right? (I know in ANSA it was huge for me) Sometimes it'll paste one node to another and collapse an element (which is what I'm going for), but other times that wont work and I'll need to delete elements then create new ones, which takes much much longer. Any idea why this is?

What do the colors of the dots that show up when a node is clicked on indicate? Sometimes they're green and sometimes pink...


Since this thread had been mucked up a bit, I will use the quotes and answer this in pieces...

First, unlike hypermesh and other codes, the ICEM CFD mesh editing looks after the surface mesh and volume mesh together. When you are merging nodes, it may look simple on the surface, but it may be causing an inverted element or something like that in the volume... If that is the case, it wont allow it. You can move the node a little and try again, but I usually just delete my volume mesh and clean up the surface mesh on its own (delete elements and select all the volume elements using the last button on the selection tool bar). This makes mesh editing much quicker and easier. Then I generate the tetra/prism mesh from the surface mesh using Delaunay (and now Delaunay TGlib in 12.1).

The second question is about the node colors... These are colored by projection. Red nodes are point projected and will not move (unless you change their projection first). Green nodes are curve projected, they can be slid along curves. White nodes (or black on a white background) are surface projected, so when you move them, they slide on the surfaces. Blue nodes (CYAN actually) are volume nodes, they move in the plane of the screen. Most of our competitors just move all nodes in the plane of the screen. ICEM CFD maintains the projection to the geometry (including during auto operations) and therefore has greater accuracy.

Also, if you split an edge to create a new node, it will inherit the lower of the two. r-g will give g, r-w will give white. g-g will give green, g-w will give w, w-b will give blue, etc.

PSYMN October 16, 2009 15:39

Auto Pick Mode...
 
1 Attachment(s)
Quote:

Originally Posted by tommymoose (Post 232816)

When creating elements, merging nodes, or any task that involves doing something repetitive, going back to the menu to hit "apply" every time is inneficcient. In ANSA I would click node 1, click node 2, then middle click, DONE, and move on the next node which would usually be around where the cursor was. I could fix up ~50 elements in about 10 minutes. Between the previously mentioned inconsistent merge problem, and this one, it would probably take me about an hour. Is there a shortcut to "apply" that I'm missing?

Thank you so much for assuming we wernt this bad ;)

Yes, there is an option (which I use exclusively), under Settings => Selection, called "auto pick mode".

In most menu's there is a logical order of operations (select this, then that) with auto pick mode, it will just prompt you in the screen without expecting you to go back over to the DEZ...

Also, when a command is completed, it will start over again (assuming you don't just want to split one edge or move one vertex). To end a command completly, just middle mouse button again.

Another thing that may help is the hot keys... These are tab sensitive (Edit mesh hotkeys if you are on the edit mesh tab, Geometry hotkeys if you are ont he geometry tab, etc.). Do a search in the help for "hotkeys" and you can print out the maps. I am attaching one here, but had to lower the quality to make it fit.

PSYMN October 16, 2009 15:46

Process...
 
Quote:

Originally Posted by tommymoose (Post 232816)
Regarding mesh quality - You smooth and correct after the octree mesh to get the best quality surface mesh you can get. Then comes Delauny. Then prism. Do you do manual volume mesh editting between in the middle of or after those last two steps? Just global smoothing w/ laplace?

Thank you so much for filling in the blanks I have!

Nope, If I know I am going to toss out my Octree Mesh anyway, I usually do it before any mesh editing... Mesh editing is easier without the volume mesh gumming up the works... Then I improve the surface mesh as much as possible, this includes all my mesh checks, automatic smoothing and manual editing...

Oh yea, If you are not making extensive use of subsets then you are probably editing the hard way ;)

Most of the mesh problems are because of issues between the volume mesh and the surface mesh, once that is taken care of, we rarely need to volume edit (though it may come up from time to time and the tools are there).

Then I run my delaunay for the volume mesh, followed by some automatic smoothing and some final checks to make sure everything is ready for my prisms.

Then I run prism, followed by smoothing. For prism smoothing, freeze the prisms for the first few iterations or your top layer will get all messed up to accommodate the tetras. If the prisms are frozen, the tetras will adjust inward and then only smooth the prisms a little bit at the end if absolutely necessary.

Simon

PSYMN October 16, 2009 16:01

Fun with .lwo
 
Quote:

Originally Posted by tommymoose (Post 232941)
I downloaded the 3D model from a website. I forget which model I chose exactly, but we compared the model to the real thing and tried to choose the most accurate. I substituted in our airfoil blade, remodeled the wheels in solidworks and replaced the ones in the model (too complex), and did a ton of manual cleanup. Hopefully with the rest of the posts in this thread you can complete your own project :)

This might have been the model I downloaded - http://www.the3dstudio.com/product_d..._product=28866


I have had a lot of success downloading models in .lwo format and then using a program called "3D Exploration" version 1.5. I updated to a newer version once, but preferred the old version so I went back...

3D Exploration lets me output the .lwo as an STL file or .dxf file which I can easily import into ICEM CFD...

Then I convert geometry(facets) to mesh, clean everything up, convert mesh back to facets (geometry) and go from there.

Simon

PSYMN October 16, 2009 16:05

Backfire...
 
Quote:

Originally Posted by rwryne (Post 232942)
Did you try to explain you were speeding...for science?!?

Except that the outcome of the "science" would be a faster Porsche speeding by the police... Or at least one with better grip for keeping up that speed thru the corners...;)

Hilarious pic by the way...:D

tommymoose October 19, 2009 23:32

Quote:

Originally Posted by PSYMN (Post 232962)
I have had a lot of success downloading models in .lwo format and then using a program called "3D Exploration" version 1.5. I updated to a newer version once, but preferred the old version so I went back...

3D Exploration lets me output the .lwo as an STL file or .dxf file which I can easily import into ICEM CFD...

Then I convert geometry(facets) to mesh, clean everything up, convert mesh back to facets (geometry) and go from there.

Simon

Those sites seem to be small/well-managed enough that you can email them the format you want and they'll make it available within a day which is nice. Aside from that easy way out, I've had luck using Rhino for geometry conversion, and they have a free trial... which you can keep trying ;) It looks like 3D explorer is free, or $30 at most, so I may check that out if I need to do some more translations.

Thanks again for the great explanations! Its those little things you mention that are very helpful. I'm not in an office environment where best-practices and little tricks are spread quick, and many of those things aren't fundamental enough to have anything come up in a search, so its really helpful :)

PSYMN October 19, 2009 23:57

Happy to help.
 
When I first started using ICEM CFD, I was doing consulting in an office with lots of experts and very low cubicle walls (4 inches above the desks). It was a great place to learn quickly.

So many other users seem isolated and on their own, which could be very frustrating.

This is why I try to help one or two people every day here on CFD-Online.

tommymoose October 21, 2009 01:12

5 Attachment(s)
I'm getting divergence in Fluent using the K-epsilon model. I'm even just doing the first-order upwind option and having problems. I lowered the turbulent viscosity to 0.8 and both the turbulent kinetic energy and dissipation to 0.7 (per advice from my professor) and it still diverged after ~140 iterations.

I have a surface mesh of 173,000 elements (post deleting octree volume) that are all at least of 0.2 quality. I had 38 from 0.2 -> 0.25 and 132 between 0.25 -> 0.3. I ran a Delauny mesh, then added 6-layers of prisms with the default settings. Then I froze prisms and smoothed the tetras like you recommended.

One reason I think I may be having problems is that surface that I'm using as a symmetry plane in Fluent isn't perfect. I forgot to add a curve between a couple of surfaces (ex. windshield and SYM), so the edge wasn't sharp and the elements did a little bit of a "fillet" is a few spots. I tried to correct the problem before running the Delauny by using the move -> align nodes function, but its not perfect... in the Y-direction min is -.128 and max is 0.048 (inches). Would this lack of 100% planar surface cause the divergence issue? Any other issues you see in my surface mesh that might be leading to it?

If so I guess I'll have to just go back and do it all again.... I tell ya, there's no substitute for experience :D

tommymoose October 28, 2009 19:33

2 Attachment(s)
As an update, I met with my professor and he gave me some advice on how to troubleshoot my divergence issue -

I was unaware that you could stop the simulation at any point and view the results of the last iteration. My professor advised that I stop the simulation once it started diverging and look around the results to see where pressures/velocities are out of whack. I visualized using contours and auto-range turned ON (make sure you turn your "int-body" part off otherwise you'll freeze up). Sure enough, right where the the front wheel meets the floor, the velocity is 10k+ m/s :rolleyes:

I'll be going back now to see how I can tidy this area up. The prism's might have turned into pyramids in this area or some other quality deterioration occurred. I'll post back when I fix the problem.

PSYMN November 2, 2009 20:21

Your non-planar Symmetry plane...
 
Hopefully you can figure out your high velocity issue under your wheels. Many times Ford and others just put a fillet between the wheel and the ground to simplify this area. The real rubber doesn't meet the road at a sharp fillet either.

As for the symmetry plane issue. You can add curves (of intersection) after the fact and associate the appropriate nodes with them to build back your sharp corner...

The Symmetry boco does expect the symmetry plane to be a plane (even if this failure isn't causing a crash). You can achieve this quickly by setting the Exact Y value to zero. This is under the Edit Tab => Move nodes => Exact => Position => Modify Y = 0 and select all the symmetry plane nodes.

This trick is especially helpful with 2D models where Fluent does not accept any deviation.

tommymoose November 2, 2009 20:43

1 Attachment(s)
I skirted the problem by not putting prisms on the wheels. In the future I'll try what you suggested. Thanks for the tips on getting the nodes to zero... funny that the most fundamental/basic move feature would be the best one for the job.

I ended up running the simulation as-is and it was converging nicely. Once epsilon dropped below 10^-4 at about 400 iterations, it stopped and said it was complete. The residual values were still falling though, so I think I need to keep simulating. I've been really busy and haven't had time to figure how to seed a new run (or continue from my current data), but I know that's the next step.

For later simulations, I want to add in a front splitter. I would think that for comparison runs, ideally you want as much of the mesh unchanged as possible. This way, any differences in results could be attributed to the part changed and not mesh differences elsewhere. Am I correct in saying that? This is making me think that my methodology should have been to tweak the geometry from the beginning rather than cleaning up the mesh so much... oh well I knew this would be a learning process. As of now I plan on going back to the file with geometry in it, adding the splitter, and meshing from scratch. Is there an easier method than this that I'm not aware of?

Thanks!

Now I just need to figure out what to do with my output Cd of -954.... hopefully just a reference value issue

PSYMN November 3, 2009 18:39

Work from surface mesh...
 
Maybe you don’t need to go back to your original geometry to add the splitter…

Is it complex geometry or a simple drop from the chin of the car?

Either way, you can probably start with your current mesh file (pre-prism), delete the volume cells and go from there.

If it is a complex piece of geometry, then perhaps you will need to mesh it separately and stitch it into the rest of the model. The amount of pain required will vary significantly depending on your specifics, but it will probably be easier than starting over and will give more comparable results since most of the mesh will not change. If you can intersect the new geometry with the old one to get a nice curve of intersection, you can use that to make the model crisper…

If your splitter is simple, perhaps it is just an extrusion of the elements already in your model… Use the extrude command to extrude the line elements into shell elements. If it is a zero thickness splitter, make sure to mark its part as “internal wall” so that things go more smoothly.

If you post a pic, I can provide a more tailored solution.

tommymoose November 21, 2009 16:02

2 Attachment(s)
Its been a busy few weeks! I was able to run two simulations to make a comparison very easily. On the first run I set the "blockoffs" as a no-slip wall, and the second run I set them a porous media with no resistance. 10% better DF with them closed! Now it comes time to add in a splitter design or two to see if the open/closed effect is accentuated. I'm attaching an image of what I plan, along with an image that shows the detail of the front air-dam mesh currently. The splitter will protrude a few inches from the front and extend back under the car until it meets up with the underbody. It doesn't need to be sealed (this may make it easy to only have to connect to the line of facets that make up the front lip). Any advice?

After I find the best splitter profile, I'll do a study on the length that it protrudes from the front end. I'd imagine an extrusion is the best way to modify the splitter length once its in, but is there a limit to how much you can extrude? (this must modify element quality as it skews?) What do you think is the best way to do this?

Thanks Simon!

snailstb November 22, 2009 02:27

dear tommymoose:
thank you for sharing your experience in this thread, i learn a lot from it, it is a kind of you. :)

jsm November 22, 2009 23:47

Hi Simon & Tom

I also learned some new ideas and suggestions..........

Thanks a lot


All times are GMT -4. The time now is 20:46.