Hi Jason, Thanks for the suggestions. I managed to mesh the two cylinders by uniting them. But a blue line appears (evenin the mesh) from the face coonecting the two cylinders to the the bottom circular face of the 2nd cylinder. What does this line mean?

And then, back to my old problem- about my solid model imported from ProE...... Is this the order that I have to follow?

1. Import the solid model as a STEP file. 2. Create a cyliner around the solid ( actually, the solid is supposed to be inside the cylindrical tube) 3. Create the second cylinder connected to the first cylinder end- to- end. 4. Follow your suggestions of uniting the two cylindrrs 5. Subtract the volume of the solid from the volume of the first cylinder to get the flow field within and around the solid. 6. Mesh all the 3 volumes applying the sizing functions.

Please correct me if I'm worng anywhere.

Expecting your reply.

Thanks a million for all the help.

Cheers, Vidya

Instead of starting a new thread, simply respond to the post... it keeps the conversation grouped together, otherwise you end up having part of the conversation being at the bottom of the forum, part in the middle of the forum, and part at the top of the forum.

Can you get a picture of the blue line and send it to jason_at_bae@yahoo.com. Go to File->Print Graphics, change it from Printer to File (.tiff is fine). I'm not 100% sure on your geometry, so it could be a lot of things. It could have to do with the way the cylinders intersect. I could make a lot of guesses, but without seeing what it is, that's all they'd be. It may not affect you though. If you could mesh it without any problems, then you can probably ignore the line, or you can merge the two faces that the edge separats before meshing and that will get rid of it (Assuming its something simple that caused the line of course). This line could also just be the tangent line of the curved surface (just used to show you the extent of the surface... it's not actually part of the geometry).

As for the order, the only comment I have is about the 3 volumes. If you unite the two cylinders, then they become one volume. And if you subtract the imported geometry from the big volume, then you are left with only one volume (the cylindrical shape with a hole in it the shape of the imported geometry). If you connect the cylinders instead of uniting them, then you'll have two cylinders instead, but still not three. Other than that, I agree with your order.

Hope this helps, Jason

For my geometry imported from ProE as a STEP file, is it OK if I create the cylinder, subtract the volume of the solid from that of the cylinder (without the RETAIN VOL option) and mesh the subtractec volume directly without meshing the edges, or faces? I tried meshing the edges, then faces, and finally the volume according to the GAMBIT hierarchy, but the program crashed. So I meshed the subtracted volume directly. Is this correct? Will it cause problems after exporting to FLUENT?

For your info, my originl task is to mesh the flow field within and around the solid. So I imported the geometry, created the cylinder, then subtraction of the solid vol from the cylinder vol, then meshed the subtracted vol directly.

If this method is wrong, is there any other way I can mesh the flow field without causing the program to crash?

Thanks a lot, Vidya

Typically Gambit will crash because of memory errors. One thing that seems to help is to save, and to save often. This frees up the memory that was being used to maintain the "undo" command, and sometimes that's just enough to keep Gambit from crashing.

Other times, it's a program level crash, and who knows why this happens... usually it's geometry... sometimes I've had it crash over and over and over on the same step for the same geometry... then I restart the computer and it works fine... or even better is I had a problem all day Friday... came in Monday morning and asked one of the other guys to look over my shoulder to see if he knew what the problem was, but it didn't happen again (didn't restart the machine over the weekend because I was running another job on some remote machines... the only thing that changed from that Friday to that Monday was the date).

Anyway, the only reason you typically mesh from edge to face to volume is to control your mesh. If you're defining sizing functions to control your mesh, then you don't need to do this, or if you're simply defining a uniform mesh size across your entire domain you don't need to mesh according to the heirarchy. Since it's crashing when you mesh according to the heirarchy, and not when you go straight to the volume mesh, it leads me to believe that it's just due to the memory problem, and you may be able to get around this with saving the file before meshing the volume.

Now, you have to be much more careful if you go straight to the volume mesh... you have to be careful that you have a good mesh. After you mesh (save it just in case it crashes ) you need to look at the skewness of the face meshes and of the volume meshes. You should look in areas of complicated geometry to make sure you're happy with the mesh (making sure there's no weird bumps that can show up out of no where on imported geometry, and also making sure that you think the mesh is refined enough to capture the flow physics). The analyze mesh tool is a huge help in this (it's the button on the very bottom right of the screen... looks like a little yellow mesh with a magnifying glass over it). Also, use the analyze mesh tool to look at some planar cuts through the geometry and make sure that the mesh distribution looks good, and that the mesh transitions smoothly from areas of refined mesh to areas of coarse mesh. You should do this even if you follow the heirarchy. It's good practice to analyze your mesh before you ever send it to the flow solver.

Hope this helps, and good luck, Jason

I looked at the mesh quality earlier too and it showed the two sliding bars at the bottom at ~ center position. So does this mean that the mesh is fine? How do you check for the weird bumps or some other such abnormalities?

Also, when I took the mesh to FLUENT, and looked at the velocity vectors in the XZ plane (after slicing the cylinder using the point and normal vector, as you explained), I get a sudden jump in the flow from 0.175 m/s (the inlet velocity) to 8.35 billion m/s near the wall of the geometry........ this is totally baffling me. And this is happening only on one side of the geometry. The geometry is symmetrical. And then after this section, the flow returns to normal laminar flow again. My question is, does such anomalies happen due to improper meshing? Some weird things that popped up in the flow solver? If so, how can I rectify the mesh only in that region? And is it possible to force the velocity at the wall in that region to be zero (in the boundary conditions)?

My other thought is that it may be due to the units conversion......... the dimensions of my geometry as well as the cylinder created in GAMBIT are in mm. But FLUENT calculates everything in SI units. How do you make FLUENT to calculate everything in consistent units?

Thanks in advance for all the help and advice.

Vidya

Fluent will always calculate in SI units (m-N-s). You can change your mesh scale (Grid->Scale) and you can change what units Fluent displays (Define->Units), but you can't ever change what units Fluent actually calculates in. This shouldn't be an issue though. If you do run into problems where your geometry is small, and the round-off error becomes significant, then you can use the double precision solver instead (fluent 3ddp or fluent 2ddp).

I would say your mesh or your boundary conditions are the reason your velocity is blowing up. There's no physically possible way to get the flow to go from .175m/s to 8.35(10^9)m/s (just for reference, the speed of light is just under 300(10^6)m/s). If your outlet pressure is 0Pa absolute (gauge+reference), then who knows what you're going to get. Or if you have a highly skewed element in an area of strong flow curvature, then you're incorporating a lot of error (especially if the cell size it too large).

Those bars you were looking at when you examined your mesh were probably to control the planar cut you are looking at through the mesh. You should play around with these sliders to see the mesh along different cuts through your geometry. You have to make sure the right elements types are enabled (2D or 3D, and hex, tet, pyramid, or prism... or turn them all on... I would set the type to 3D, and then select all of the element types next to it... once you're more familiar with Gambit, then you can start playing around with what you're looking at). Also, make sure your quality measurement is equi-angle skew. Once you have these settings, then play around with the sliders to see the mesh cut through different locations in your geometry. Look at the mesh to make sure you think it's sufficiently refined in areas, and that it doesn't grow too quickly from refined areas to coarser areas. Once you are comfortable with your mesh sizes and growths, then change from "Planar" to "Range" at the top of the Examine mesh window. Then the new sliders at the bottom of the examine mesh control the range of cell skewness you are looking at. You can play around with these sliders to see the areas that have the highly skewed cells. Or you can click the "show worst cell" button and it will zoom in on the cell with the highest equi-angle skewness. In the text window it will also print what the skewness is of this cell (lower is better, but try to stay below 0.85, but going up to 0.92 or 0.95 can be alright depending on mesh size and location... the CFD purists will argue with me on that point, but if you have one cell in an area of low flow curvature, and it's small, then the error you create is small, and usually insignificant compared to other assumptions like constant profiles at inlets).

Once you're comfortable with the mesh, and get a reasonable solution, then you should remesh your geometry with a more refined mesh and re-run the case. Keep doing this until you get a consistent solution from one refinement to the next. This will tell you what kind of mesh resolution you need to properly capture your model (this is your mesh sensitivity analysis). You might find that your initial guesses at mesh size are way too coarse to properly capture your geometry.

Hope this helps, and good luck, Jason

Hi Jason,

Is there any way how I can introduce a pulsatile waveform into my meshed flow domain volume(i.e., the volume obtained after subtracting the volume of the solid from that of the cylinder)? Also since my solid geometry is that of a valve frame (intended to be inserted into the leg vein), I also have to wrap leaflets around the flanges. Then introduce the pulsatile waveform (from WINDAQ). How can I inyroduce this waveform into FLUENT and then do the flow calculations?

Thanks a ton for all the help.

Cheers, Vidya

Jason- another question for you....... is it possible to force the velocity at the wall (of the solid geomety as well as that of the cylinder) to zero in the boundary conditions? I know FLUENT does this by default? But is it possible to set the vel at the outer surface of the solid also to be zero? I do not want any flow at the wall of the solid or in the gap (this is extremely tiny) between the solid wall and the cylinder?

Sorry for my incessant questioning. Regards, Vidya

I'm not sure what you're asking here... any BC you define as a wall will have the no-slip condition (assuming a viscid calculation of course). If there's a small gap that you don't want flow through, then you should've removed that gap when you were working with the geometry in Gambit. Otherwise you would need a BC wherever there's an opening of the gap, and you can go and redefine all of these as "walls". This will stop flow from getting through. But once again, that's something to be done in Gambit.

There may be other ways of doing this with UDFs, but I have no experience with actually writing a UDF, so I wouldn't be able to help you.

Jason

A pulsatile inlet is going to be a UDF problem for sure. Look through the UDF manual and at the UDF examples on www.fluentuser.com

Hope this helps, Jason

Jason -

I fgound nothing on the website that you mentioned........except stuff for buying (laptops, etc). How do I find info on UDFs for pulsatile flow here?

Thanks, Vidya

Sorry, that was www.fluentusers.com (forgot the last "s"). You need a username and password. If you're a corporate account, then you can contact your service advisor for this. If you're an academic account, then your administrator should have this info. Either way, the documentation also comes with Fluent, and you can ask the people who installed it about where the documentation was installed.

Jason

Jason -

Is it possible to create a leaflet around my solid geometry that opens and closes according to the pulsatile conditions specified? I want to to simulate this condition:

A flexible leaflet is wrapped around the flanges of the geometry (valve frame) and this leaflet opens and closes according to the pulsatile flow conditions.

Can I create the leaflet (I have the dimensions) in GAMBIT? Or will GAMBIT treat this as a wall or some solid? Do I have to use Dynamic mesh to simulate the movement of the leaflet? The geometry is the same that was created in ProE and I sent it to you a couple days ago.

Thanks, Vidya

That sounds like a dynamic mesh model, but I don't know how you would go about doing it. You can try starting a new thread (stating your whole problem) and someone might be able to help.

Good luck, Jason