Simulation Mechanical Forums (Read-Only)
Welcome to Autodesk’s Simulation Mechanical Forums. Share your knowledge, ask questions, and explore popular Simulation Mechanical topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Multiphysics Simulation Stress analysis (deformation) and fluid flow

6 REPLIES 6
Reply
Message 1 of 7
znoroozi
1792 Views, 6 Replies

Multiphysics Simulation Stress analysis (deformation) and fluid flow

Hello All,

I am trying to simulate the fluid flow in a channel that is deformed under stress/strain. I was wondering how could I couple the two effects in Algor. My intuition is to first slove the model for stress analysis and then create a new part for the internal section of the channel and run a fluid flow simulation for the second part. The problem is that I am not sure how to take the channel difformation into account. Any ideas?
Also, I run the stress analysis simulation in autodesk inventor first and try to import the results using "Ad-ins" option, but the stress analysis results are lost and I don't see them in Algor. I trully appreciate any suggestions.
6 REPLIES 6
Message 2 of 7
John_Holtz
in reply to: znoroozi

In part because the Inventor simulation has a different solver which can make do with a coarser mesh, the transfer to Algor Simulation does not transfer the mesh, and therefore, we cannot transfer the results. We only transfer the CAD geometry and the loads/boundary conditions. So, your options are

1) use the deformed shape from your Inventor simulation to create the fluid part (if that is even possible)
or
2) run an Algor stress analysis with the solid parts AND fluid part. Export the deformed shape to a new Algor model and run the fluid analysis. ("File > Export > Make FEM"). In the stress analysis, you want the "fluid" part to have very weak mechanical properties. You are including it just so that you can get the deformed shape of the fluid. (That's probably easier than doing the stress analysis without the fluid part, and then trying to construct the fluid part from the deformed shape.) And in the fluid analysis, you are only including the fluid part; the solids can be deactivated or deleted.

John Holtz
Product Design Engineer, Algor Simulation
Autodesk, Inc.


John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 3 of 7
znoroozi
in reply to: znoroozi

Thank you so much for your reply. That is exactly the same solution that I arrived at after trying many different ways. I need to find a material for inside the channel that acts like a glue and follows the shape of the channel walls. Is there a way to define the contact between the two parts? I tried Contact->bond and contact->weld but none of the work. After running the simulation, the channel is deformed in a very strange and unexpected way and the displacement shows really big numbers (in the order of 10E8). The only force I define for the entire simulation is a G force of 3400 m/s2 in the x direction (horizontally, alongside of the channel).
Message 4 of 7
John_Holtz
in reply to: znoroozi

The large displacement certainly sounds as if the two parts are not bonded together, and if the part does not have boundary conditions, it "floated" away. Since you activated the bonded contact, it sounds like the problem is one of these:

1) there may be a gap between the fluid and channel that is larger than the tolerance for matching. (the default tolerance is 5% of the local mesh size)
2) you used a different size mesh or different type of mesh on the two parts, so the meshes do not match. (this makes sense since the mesh for fluid is probably different than that required for the stress analysis)

For item 1), either change the CAD model to remove the gap between the fluid and channel, or change the mesh matching tolerance in Algor Simulation ("Mesh > Model Mesh Settings > Options > Model" and change the "On-surface tolerance based on" and/or the "Tolerance value".

For item 2), you can use the Algor Simulation "smart bonding" which is essentially the same method that Inventor Simulation uses to bond dissimilar meshes between parts. Activate the smart bonding under "Analysis > Parameters > Contact" and set the "Enable smart bonded/welded contact" drop-down. Be sure to click the "Help" button on this dialog and expand the paragraph "Contact Options" to get a better understanding. (Although if the bonded part is very weak like your fluid, then the setting chosen for the smart bonding type should not make a difference.)

If the problem is something else that I have not touched on, please let us know.

John Holtz
Product Design Engineer, Algor Simulation
Autodesk, Inc.


John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 5 of 7
znoroozi
in reply to: znoroozi

Dear John,

Thank you so much for your thorough reply. I really appreciate it. Now, after I set up the model and try to export the deformed mesh using "Make FEM" option, the program halts and goes into the "program not responding" mode. I tried to attach the model to this message, but it was too large (~6 MB). Is there any other way that I could send you the file to take a look at?


With Regards,
Zara
Message 6 of 7
John_Holtz
in reply to: znoroozi

Hi Zara,

I just did a test. While it was working on exporting the model, the Algor Simulation interface did go into "not responding" mode. So I think what you saw is normal behavior. The command is slow, so I suggest you start it at the end of the day and let your computer run overnight.

Note that the exported file uses the exaggerated displacement shown in the graphics area! So if you want a true life deflected shape, you need to set the "Results Options > Displaced Model Options" dialog to "As an Absolute Value" and set the "Scale Factor" to 1.

John Holtz
Product Design Engineer, Algor Simulation
Autodesk, Inc.


John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 7 of 7
znoroozi
in reply to: znoroozi

Hi John,

I let the export (make .fem file) run for more than 54 hours, but at the end, it was not able to create the file; I ended the process. I have 34000 mesh nodes in that model. Is that number too high for the software to handle? The reason I generated a relatively dense mesh is that I want to simulate the fluid flow inside the channel and I need to have enough numbers of meshes in the z (smallest dimension) of the channel. After I convert the deformed mesh, it is impossible to change the mesh density or define a different type of mesh. Many of the options in the new .fem file are disabled. Do you have any suggestions?

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report