Time dependent intake flow simulation 1

[aebstract]

I'm trying to do something exactly like what is in this video:

http://www.youtube.com/watch?v=X3ecq8MNfk0

I've got pretty much everything for my model set up as best I could based on what went on in that video. What I'm stuck at is trying to get results to where it displays the same way, where I can watch what happens as each valve opens (pressure changes) and it cycles through. I'm getting strange results where the air seems to be doing odd things and not being pulled in towards any outlet any more than the others at any given time. I don't really know what information you need to go forward. I'm creating a flow trajectory and telling it to "play" to get the animation but nothing is changing at all and it all just runs constantly in the same pattern.

 

[aebstract]

One full week and not a single response, not even a "take a look here" or anything. Nice community.

 

[kellnerp]

OK, I'll bite even though I don't have Flow.

For starters just do a simple model.

Static flow
One port open, the others closed.
Repeat for each port.
Setup your post processing on that and make sure your model has sufficiently fine gridding to capture flow around tight or small features.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

http://www.linkedin.com/in/engineeringtransport

Phenom IIx6 1100T = 8GB = FX1400 = XP64SP2 = SW2009SP3
"Node news is good news."

 

[Isarmann]

I'm sorry no one stepped in to answer this for you. From what I've seen, so very few people are doing time-dependent analysis there just really is no one to go to for help.

I can help you with where you've been going wrong on this, though.

What you're seeing when you've tried to animate by clicking "play" is one frozen moment in time, put in motion to show what was happening, yes, but only at that one point in time. You want to see a time-dependent result, and if you set up the simulation correctly, you already have the data from many points in time.

Okay, so you know how you have "load/unload results" to get at the dataset... and when you open it, it's the main .fld file you choose, but you can see there are very many numbered .fld files in that data folder as well. The "main" .fld file you choose is the master file for the whole set--- the numbered ones are the specific data for each point in time.

So, when you want to animate (and I would not try this with flow trajectories at first--- use isosurfaces set to temperature or something to "show" the gas; if you do it with flow trajectories, it has to make that minor calculation ("calculating flow trajectories, please wait") that you see when you activate one-- it has to do that for every frame. In my own work, I have one frame for every .01 milliseconds, and I look at about 10 milliseconds of realtime, animating at 100 frames per second--- it's a lot of calculation. Using isosurfaces, it doesn't have to specifically calculate those example trajectories; it just goes off of the fluid results data it already has.

Okay, so near "load/unload results" is that other button with a disk icon called "flow simulation results"--- using the Load Time Moment option there, you can choose any of the .fld files, and thus change which of the moments in your run you're looking at to start with. Still just one moment, but you can spot-check the whole run this way.

Now, to actually animate, create your isosurfaces, your cut plots, what have you, then open the animation creation section either by "animation-insert" or by clicking a plot or isosurface and clicking "animate". Within the animation window, you MUST use the wizard, tiny button next to plus/minus just over the animation window's feature tree. On the first page of the dialogue, click "delete previous tracks" and choose how long you want the animation to take to play. Next choice, skip it, has to do with rotating the model. Then you will have a choice between loaded results (meaning, the ones you already have loaded, that one moment in time), or "scenario". Scenario is the code-word for a time-dependent situation. So choose it. On the next page, choose the "proportional distribution" radio button, and "physical time" next to it. The sliders down below allow you to choose how much of your dataset, in realtime, you want to look at. I model 20 milliseconds from the start of an event, so by default the upper one is set to zero and the lower to 20 ms. So if I want to look at only from 1 ms elapsed until 4 ms elapsed and not more, I adjust each slider accordingly.

When you click "finish", you will see the animation window fill in with small diamonds stretched over the amount of time you specified for the animation--- each diamond is a results node point. You must then insert a control point by hovering over the animation window right by the start line, and level with your entry in the feature tree for "isosurface 1", or whatever. Insert control point and drag until it matches the full length of the animation. It is much easier to do this if you resize, using the plus/minus buttons by the wizard button, to show all the time node points on one page. Once you have the line representing your view (the isosurface or cut plot "control point" you inserted) running all the way under the diamonds as far as the whole animation length, click play and watch it work. The second tab in the animation window is where you can choose the framerate (up to 100 fps) and the filename, should you choose to "record" the animation to disk. If you do so choose, it will play faster and more smoothly--- the animator will do what it can, but it cannot load results at the rate of 100 frames per second, even if you want it to--- those settings will come into play once it has been recorded.