CFD analysis with AcuSolve
 

Hi everyone,

for the office we are planning to bring AcuSolve to the CFD department since we already have Hypermesh to create cool meshes :)

Do u have some comments about AcuSolve? Do u know if it can make 2D analysis?

We are at the moment not trying to achieve huge calculations with it. Incompressible flows is what we are planning. Maybe two phases (air, water) but that's all.

Thanks in advance, people.

;)
mems21

Hi

We are using Acusolve a lot, it is great on 2D simulations and also have several great fetures,

Do not hesitate to contact me for any help.

Regards
Elena

As far as I know, Acusolve can solve 2d using one cell width.
So 2d analysis with one cell width is possible.

I guess acusolve does not have any multphase to solve air water. Atleast I dint read anything from manuals.

Elena,

What kind of simulation work do you do with acusolve ?

Hi Rachel,

thanks for your Info.

Considering the limitations of AcuSolve and assuming that we are not going to calculate anything out of its scope of calculations, in your opinion, is it Acusolve a software to consider as main software? Or would you have it as a software to support another one like Fluent, STAR...?

Thanks ;)
mems21

Acusolve is certainly a powerful solver. If it does what you need and accurately then there is really no need for another code.

In general Acusolve dances to a slightly different drummer than the other codes (or at least it used to - it may have been hidden by the pre/post processor now). It is basically an equation solver that, if you happen to choose the right boundary conditions, will give you the answer to a fluids problem. That being said, if you set it up right it is fast, robust and accurate.

I like the problem setup being in an ASCII file, you can see what the code is working with. I currently use CCM+, which has many good features as well, but on a complicated problem it is essentially impossible to really know what is in the model, whether it has been propagated from client to the server processes,what has been changed,....

Hi Mems21

As Robert mentioned, it is fast/robust and text file driven.
If the physik is ok for your application, then a leading program.

Since I am a LaTeX/Linux user, I like the 3D images inserted in PDF docs by acureport tool.
http://www.acusim.com/doc/AcuReport_...nce_Manual.pdf

Cheers,
R.

Hi Rachel,

thanks a looooot for the Info.

Looking forward to start with AcuSolve :)
mems21

Hi,

Anybody actively using AcuSolve? If you are facing any issues, let us discuss.

Cheers,
/R

Acusolve Tutorials
 

Hi everyone,
Anyone can help me to learn Acusolve as early as possible with pdf or videos:)

If you a customer then the best resource would be Altair Client Center.
http://www.altairhyperworks.com/ResL...l&category=All


There are lots of PDFs and video recordings to get you started in the client center :)

For freely accessible tips and tricks :
http://www.altairuniversity.com/acusolve-cfd/

I am using AcuSolve to simulate thermal analysis for automobile lamps.

I started with a simplified model which is just a box with two vents (lamp housing) and a solid cube (acts like a bulb). And I simulated two cases:

i. Two vents Open
ii. Two vents Closed

other conditions are listed below:
Boussinesq Model for Air
Box Wall Temperature= 323 K
gravity turn on
solve for temperature, flow and temperature-flow

for case ii, everything went well, air was heated to blow up;
but for case i, I tried different BC types (outflow, inflow) for the Opening vents but the air flow always went into wrong direction (should be against the direction of gravity).

I would like to hear from you if you've any ideas.

Thanks,

Could you please upload your .inp 8input) file and if possible also the .acs (AcuConsole database) file?

Have you tried contacting your local Altair support ?

I sent my files to altair technical support and they said they would contact me once they got results, but no news so far.

Anyway I uploaded all my files onto Google Drive.
You can access via- usr: cfdonline.share@gmail.com
pwd: cfdonlineshare

Sorry, it took me a while.

Temperature seems to be fine.

However there is a velocity component in Z-direction in entire domain. I could not get time to have detailed look. DO you know the reason for this velocity in -Z?

I will try to look again later in the day.

I got the same results and the velocity in Z direction was due to the gravity.

However, in my setup, the gravity was in -Z which meant that the flow should go up in +Z.
Now the simulation showed an opposite appearance.

Finally had some time to catch up with this model...
I have uploaded a variation of the same on your drive.

It is now "boxed". No inlet or outlet, completely closed system. The one you started with two outlets and no inlet was unlikely to be stable simulation.

https://docs.google.com/file/d/0B9k4...it?usp=sharing

Hope it helps.

with top outlet
 

another update:
After "opening" the box i.e. creating one outflow with backflow condition, its working. Velocities field is as per expectation.

Database is downloadable from :
https://docs.google.com/file/d/0B9k4...it?usp=sharing

The closed box and the box with one side open seem to be OK. But I wonder how can I make the box with two opening working.
I also simulated the same in SC-Tetra and using two opening with simply static pressure = 0, and it gave a reasonable result.
Now I want to do the same thing in AcuSolve but got trapped on this B.C. setup

Just copied the BC settings from upper opening to lower and its working.

https://docs.google.com/file/d/0B9k4...it?usp=sharing

Is this something similar to what you expect?

Yes, this is exactly what I want.

I thought I'd tried two opening using SBC-'outflow with backflows' but it gave an opposite flow against the physics. Perhaps I did something wrong; I will go through your model carefully to see if there are something I missed.

Thanks so much for your kindly help!

This model has hydrostatic pressure setting enabled at both outlets.
Also a steady state solution was used a initial value for transit run.

This hydrostatic pressure is interesting. Actually I've tried to apply a p*g*h pressure on lower opening. I thought the it is too sensitive to impact the results since for air p*g*h is so small and also it is not practical if I have some openings that are not parallel to the reference. Now it makes sense.

I have used SC-Tetra before and it seems that SCT will automatically take into account for hydrostatic pressure.

Thanks a lot for your help:)

Some notes about Hydrostatic Pressure from the AcuSolve Command Reference Manual:

"If gravitational force is modeled using the GRAVITY command, then hydrostatic_pressure=on should be set for most pressure or stagnation pressure boundary conditions in order to properly account for the hydrostatic pressure. This is most commonly needed on outflow boundaries."

Just a quick question about this simulation. Were you able to see mass conservation between the inlet and outlet? From the velocity vector plots, it looks like the velocities are much higher at the top than at the bottom. As i have not run this simulation, i have not taken a look at the results. My conclusions below are based on the plots you have shown.
As the mass flux over a surface area is (density x area x velocity), it does make sense that velocities are higher at the top. However the magnitude of difference between the inlet and outlet does not seem to match the expected difference in density.

Mass conservation was pretty good. See the screenshot of mass flux at those surfaces.

Since both the top and bottom were "open" boundaries and not specifically inlet or outlet, there are some regions at the top where there is mass coming into the box.

Results
 

How u are seeing the results in Acusolve.Do we have go for Post Processing tool?

Within the Hyperworks suite you can use Acufieldview or Hyperview.

Hi Hellorishi,

I have started using AcuSolve for CFD analysis. I need to give a batch run(consisting of different cases). I found that .inp file should be used for giving batch run but AcuSolve is not generating .inp file in my case. What should I do to get that .inp file?

Thanks in advance!!!

Cheers,
Pradeep

Hi Pradeep,
Are you using AcuConsole or HyperMesh to generate the mesh and export .inp file? Are you getting any error message, while exporting the file?
Your local Altair Support might be able to conduct a webmeeting with you to find out the exact reason. Where are you located ?

Hi Hellorishi,

I used hypermesh to generate the 2D mesh and generated 3D in AcuConsole only.

I figured out how to generate the .inp(input file). It was near the generate mesh icon.

Altair support helped us in fixing it.

Thank you so much for your reply.

Cheers,
Pradeep:)

P-V Coupling in Acusolve
 

Hi Everyone,

Im pretty new to FEM based CFD and Acusolve. I did a few tutorials (Manifold and Elbow). I am curious about the lack of P-V coupling algorithms. Is it in built in Acusolve or is there no need for that in FE based CFD? Might be a lame question, but I need to know :)

Regards
Vignesh

AcuSolve has a coupled pressure-velocity solver. You can see that in the Log file as "flow" equations residuals ratios.
The coupling of temperature and flow, is optional. It depends whether flow and temperature needs to be coupled (natural convection) or not.

Also if you are trying any new tutorials make sure to use HyperWorks CFD or SimLab interface and not HyperMesh or AcuConsole. New features are being released in HyperWorks and SimLab.

Hi Rishi,

Thanks for your reply. Let me explore the solver controls.

I am indeed using HW-CFD

Hi Everyone,

Is there a way I can define an interior wall in acusolve, just like we do in Fluent?

Regards
Vignesh

HI VIgnesh,

If you are using HyperWorks CFD (any version) or SimLab 2020.1 onwards, then there is something called as AutoWall that takes care of the interior surface, automatically. There is generally no need to explicitly define such interior walls, unless you want to specify some extra BC like additional heat flux on that wall.
What are you trying to achieve with this interior wall? Is it for evaluation? Or is just a wall at the interface of solid-fluid?

Hi Rishi,

I am simulating flow through a pipe. I need to check, if the fluid
(water) hits a target kept at a distance from the pipe. In this case, I cannot define the outlet of the pipe as outlet right. If it is so, I cannot see if the fluid hits the target. Hence, I need to define this face as interior, so that I can measure velocity and pressure at this face (during postprocessing), and also can see if the fluid hits the target. My target will be the outlet in this case.
I need to do this in acuconsole/hypermesh.

Regards
Vignesh

In AcuConsole it is easy, just disable the Simple BC and keep the Surface Output active for that surface. Here is a screenshot.
BTW, I would be curious to know any particular reason you would be still using HM or AcuConsole and not the new interfaces?

Thanks for your reply. Its actually for a client and not for me :)