[tommymoose]

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]

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

[Hendster]

Originally Posted by tommymoose

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]

Originally Posted by Hendster

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]

Originally Posted by tommymoose

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

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

[PSYMN]

Originally Posted by tommymoose

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]

Originally Posted by tommymoose

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]

Originally Posted by tommymoose

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]

Originally Posted by tommymoose

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]

Originally Posted by rwryne

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...

[tommymoose]

Originally Posted by PSYMN

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]

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]

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

[tommymoose]

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

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]

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]

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]

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]

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]

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

[jsm]

Hi Simon & Tom

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

Thanks a lot