free surface representation of stilling basin

[jbecker5]

I am trying to use Simulation CFD to model  flow exiting a culvert and discharging into a basin where then it then flows over a weir back into a channel.  I am new to the program but think it will help validate our design in terms of velcoity reduction.

Does anyone have an example of a similar application or a work flow to follow?  That would be really helpful!

Currently, I have been bringing in a mock basin but when I try to add surfaces to close the volume off the program crashes.  Is there a better way to do this?  There is not much detailed information about solving for free surfaces.  I think I may not be setting up the model correctly as I try to build sides of the basin without defining a clear volume.

Thanks,

Jason

[waited]

Hi Jason,

I have run some weir examples in the past with SimCFD. It is important to create volumes that are initially filled and some volumes that will become filled as the transient unfolds. For the weir examples, I had volumes that were initially filled upstream of the weir. Then I would assign a volumetric flow rate to these upstream volumes to create the desired flow rate. Over the course of the simulation, the fluid level would rise in these upstream volumes and eventually pour over the weir.

It is important to have a fairly fine mesh on which the free surface will be defined. In some cases, this may dictate the placement of extra volumes which can be used as mesh refinement zones. This will improve the smoothness of the free surface.

In your message, you mentioned getting a crash. Was this during the "Solve" phase of your analysis?

Dave

[jbecker5]

Thank you for your response.  Yes once I click automesh and try to click "Solve" it crashes.  I also got an error when I tried to add bounding surfaces in the geometry tools.  So I need to create a volume that represents the culvert coming that initialy has water in it with a flow rate?  I guess I need to try to build the 3D volume that would be the water space not the containing walls of the basin.  The goal is to see if we can discharge the culvert into a basin (probably trapezoidal in XS shape).

Is it also possible to model a sloped concrete channel with baffle blocks to simulate the velcoity decreasing at the culvert outfall?

Maybe a sketch of the volumes you used would be helpful in getting me started since I have only been using the software for two days now.

[waited]

Hi Jason,

For your application, you should be creating volumes and a 3-D mesh.  Take a look at my attachments for some ideas of how these models might look.  I would suggest starting real simple ( for example, just create a single 3-D volume part and then use a volumetric flow rate boundary condition to fill it.  Then expand to more complex models.

Dave

[jbecker5]

I have attached a screenshot of the model, which I actually got to run.  I am not sure if the 3D geometry is right nor I am sure how to correctly view the results like you had shown in your earlier image.  I would ideally like to see velocity and water surface versus time.  I used a flow rate boundary with the leftmost volume full of water at time = 0. 

Are there certain control parameters I need to set for the free surface to show up?

Thanks again.

[waited]

Hi Jason,

I usually use the iso surfaces rendering for the free surface problems.  Choose Iso surfaces, then click on add (+).  Set Quantity to VOF, and Color by Velocity Magnitude.  The VOF will render the free surface.  Velocity Magnitude will color this surface using the magnitude of the velocity at the surface.

Dave.

[jbecker5]

I see - I changed the results to show the iso surface like you recommended but nothing showed up.  I still think maybe the simulation is not set up correctly or the control parameters are not right because I thought I would see the continous flow into the basin and the basin filling up but the results appear blank and the convergence plot does not show the velocity lines as it did for the run before.

Any suggestions?  If there is an easy way to attach the Simulation CFD file I could do that so you can see what I am working with.

Thanks,

Jason

[waited]

Hi Jason,

If you would attached a cfz file to your next reply, I could see what is missing.  Here is some information on the cfz file,

http://forums.autodesk.com/t5/Simulation-CFD/Need-to-send-us-your-simulation-model-to-review/td-p/47...

Dave

[jbecker5]

I tried to attach my cfz file but got an error saying the contents of the attachment doesn't match its file type.

Assuming I can successfully send the file to you, I would appreciate if you could take a look.  I know I need to refine the 3D geometry but I want to first get a handle of running the simulation and viewing the results.

[waited]

Hi Jason,

Try zipping up the cfz file first and see if that attaches successfully.

Thanks, Dave

[jbecker5]

Not sure the size limitsof attachments but see cfz file below.

[waited]

Hi Jason,

I got your file and it loaded sucessfully in SimCFD.  Let me review it and I'll get back to you.

Dave

[waited]

Hi Jason,

Here is a list of the changes I made,

1) Volumetric Flow boundary condition, uncheck "Fully Developed Flow".  Fully Developed Flow did not work in your version of the code.  This bug has been fixed in versions that will be released later.

2) The inflow rate of 2ft^3/hour is very slow, so I changed it to 2 ft^3/s, the filling time is over 3 minutes at this rate.

3)  Rather than 8 inner iterations, I used 3, should be enough.

4)  On the Free Surface Window, I set the Accelerations = ( 0, 0, 0 ).  These accelerations are for accelerations other than earth gravity ( like seismic loads or tank sloshing ).

5)  On the Free Surface WIndow, I set the earth gravity to ( 0, -1, 0 ).  This will allow the water to flow over the weir.

The attached file shows the results at 2 ft^3/second.

Dave

[jbecker5]

Thank you so much for your input - I really appreciate you taking the time to offer your help.  I wish Autodesk had more user information on modeling free surfaces. 

I made the changes to my model (since I did not know what program to open the results file you sent in) and ran the simulation.  I played around with the flow rate and a finer mesh size to see if I can get the basin to fill more quickly.

I am still a little unclear on viewing the results: is the free surface respresetnation different than an iso surface?  In the images you sent me, you had nice water surfaces colored by velocity.  Also I tried to using the Animate button to show the depth of the water and velocity distribution over time as the basin fills up but it would not let me.  I have attached an image of what the screen showed when the simulation was done.

In terms of modfying this basin model to represent our planned design, is there a way to specify an unsteady state flow into the model?  Basically I want to simulate a hydrograph existing a culvert and discharging into a basin and then passing over a weir back into the existing channel.  Any specific recommendations to properly represent this?  If the area I am trying to model is much bigger (40 x 20 feet), will the program crash if I try to make a finer mesh?  Also I would like have the simulation run for a long time (hours) to simulate the beginning and end of the peak flow - is this possible to do?

[waited]

Hi Jason,

Here are the answers to your questions,

"I played around with the flow rate and a finer mesh size to see if I can get the basin to fill more quickly."

The filling rate will be dictated by the volumetric flow rate into the fluid cavity.  A finer mesh will yield smoother free surfaces.

"I am still a little unclear on viewing the results: is the free surface respresetnation different than an iso surface?

In the images you sent me, you had nice water surfaces colored by velocity."

For viewing, I use the Iso Surface rendering.  Once you have clicked on the "Iso Surfaces" button in the results section, click on the + add button.  Set "Quantity" to VOF and "Color By" to Velocity Magnitude.

"Also I tried to using the Animate button to show the depth of the water and velocity distribution over time as the basin fills up but it would not let me."

The animation feature uses the saved reults data.  On the Solve->Control area, use the Save Intervals drop down to set how often to save results.  In my case, I set Results every 100 Steps.  When your simulation has finished, right click the screen and select Animate.  Select All the stored Steps and then click Animate.  It take a while to load all this into an Animation.  When it is ready, use the play, forward, back controls to play the animation.  Note too that you can use the Results->Dynamic Image buttons to save the animation to a file.  The zip file that I attached last time, was an animation file that can be played using the SimCFD Viewer.

"I have attached an image of what the screen showed when the simulation was done."

These results look fine.

"In terms of modfying this basin model to represent our planned design, is there a way to specify an unsteady state flow into the model?"

Yes - just make the inlet volumetric flow rate a time varying function.  Those options exists in the boundary condition area.  You can specify a flow vs time piece-wise linear curve.

"Basically I want to simulate a hydrograph existing a culvert and discharging into a basin and then passing over a weir back into the existing channel.

Any specific recommendations to properly represent this?"

Just model each piece as a 3-D part and that should work fine.

" If the area I am trying to model is much bigger (40 x 20 feet), will the program crash if I try to make a finer mesh?"

You are only limited by your machines memory.  For example, I can run 30 million elements on a 24 GB machine.  If you create a mesh that is too big your machine will try to utilize your hard drive as virtual memory and your processing speed will slow significantly.  You should try to keep your element count down to around 1 million elements per GB of RAM.

"Also I would like have the simulation run for a long time (hours) to simulate the beginning and end of the peak flow - is this possible to do?"

This is possible, but it will require quite a bit of computational time.  Models with 10 million elements, running thousands of time steps will require days of computing time.

Dave

[jbecker5]

Dave,

Two more questions as I try to update my previous model based on our current basin design.

1.  How do I go about creating a boundary condition where water flowing in a channel just leaves the model.  Before I had set up volumes representing differnet sized tanks that fill up but I want to model water flowing into the basin from a pipe, leaving the basin through a weir and openings in the weir wall, and then flowing down a short length of channel.  Do I need to create a special BC indicating atmospheric pressure?

2.   Is there anything special to know about using unsteady state flow as the input?  I know I need to enter the flow data as a BC but I wanted to check to see if there are suggestions for modeling a hydrograh (with a peak of around 1450 cfs)?

I am in the process of updating my 3D volumes based on our new geometry and hope to have the model running later this week.  Ideally I want to run the model for a full storm (24 hours) but I do not know what my computer and the number of potential mesh elements how feasible this will be to do given a free surface time step of 0.01 second.

Again appreciate your help through this whole process.

Jason

[waited]

Hi Jason,

1.  How do I go about creating a boundary condition where water flowing in a channel just leaves the model.

The free surface model assumes that fluid can flux into a model via a prescribed inlet velocity, mass flow rate, or volumetric flow rate ( flow arrow points into the model ).  Fluid can flux out of a model using the same BCs  ( boundary conditions ) when the flow orientation points out of the model.  In addition to these velocity type BCs, pressure is used as well.  When the gage pressure is greater than zero, it is assumed that this surface is a source of fluid and this pressure will force the fluid into the fluid domain.  A zero pressure indicates a fluid exit.  For most problems, I use a volumetric flow rate on the inlet face and put a pressure = 0 boundary condition on the problem outlet.  The software will automatically add in the gravitation head terms at your pressure outlet.  So, pressure = 0 really means zero pressure at the free surface and the density * gravity * height head terms are added to the fluid below the free surface.

2.   Is there anything special to know about using unsteady state flow as the input?

Not really.  You just need to use a BC where time = transient, time curve = piece-wise linear.  Use the Time Curve input window to add (value, time) pairs.  Data might look something like this,

1 m3/sec,   time = 0.

1 m^3/sec  time = 600.

10 m^3/sec time = 1200.

etc.

Notice that there is a plot button, so you can review your data.  Also, note that there is an Import option if you have data from an excel spreadsheet.

Good Luck with your analysis.  Simulating 24 hours will require quite a bit of computer time.

Dave

[jbecker5]

Dave,

I am testing my latest 3D geometry and a question arose about the boundary condition.  Currently we have a culvert face that I applied a volumetric flow rate boundary to.  For lower flows though, the culvert XS area is not fully utilized.  I am not sure if the program assumes the complete XS area and determines the velocity based on the flow rate?  Is there a way to set the boundary condition such that for low flows only part of the culvert is being used and then as the flow increases more of the surface designated as the BC is required?

Would adding another pipe section help with this?  I am afraid it will add alot of elements and require excessive computation time but based on another hydraulic modeling program, we should see velocities of around 5 fps initially and CFD shows 0.8 fps. 

Jason

[waited]

Hi Jason,

The best way to model several different flow rates would be to to stack a series of volumes at your inlet so that you can select a flow area that yields the appropriate inlet velocity.  For low flow you might select only the inlet face of the lowest volume.  The software divides the inlet volumetric flow by the area that the boundary condition has been applied to, yielding the inlet velocity.  The problem with using a large inlet area is that the flow will enter at a low velocity over a large area and then gravity will accelerate it to a high speed stream with a lower height.  That results in too much velocity.  Applying the same volumetric flow over a smaller area should yield a velocity that is more commenserate with expectation.

Dave

[hs.simanto]

HI!! waited!!!

Can you please upload some of your weir problems support file? that would be very helpful to understand! thank you 🙂