August 1, 2019 at 7:48 pmpeteroznewmanSubscriber
I'm learning CFD and have a model of a vacuum nozzle. The goal is to get a uniform ability to pickup debris over an 18 inch wide swath. I have a half model since the hose pulls air from the center of the nozzle. This design has two plates with holes in the mouth of the nozzle to break up the flow and avoid a very high velocity at the center of the mouth that occurs without the two plates.
I have a surface at the center of the large holes to plot the velocity.
There is a second plane though the center of the small holes.
Here is a view of the mesh. I have 12 inflation layers on all the surfaces on the inside of the nozzle, and the floor that the nozzle throat is suspended 5 mm above.
The inlet are the sides of the enclosure a good distance from the nozzle. The outlet is a pressure outlet at -1000 Pa.
My question is on convergence. Here is the convergence plot.
The residual value for continuity is 3e-2 which is my main concern. The residual values for x,y,z velocity are 3e-4 which may be acceptable.
What should I do to confirm that the above model is properly converged?
It might be that the skewness element quality is insufficient.
On similar model, I was able to get the residual value for continuity below 1e-7. That only had 3 layer of inflation.
On this model, I kept working on element quality until the skewness was < 0.86.
August 2, 2019 at 2:12 am
August 2, 2019 at 10:18 ampeteroznewmanSubscriber
The uniformity of pressure on the floor is one quality metric for the design. Here I can see more than a 2:1 pressure difference from the symmetry plane to the end of the nozzle. I expect I can even that out by adjusting the hole sizes from the the center to the end. That would be an interesting Design Optimization problem. Not sure how I would create the uniformity metric that would automatically calculate the estimate of 2:1 I just made visually.
Another quality metric is the velocity under the edge of the nozzle. Here it is about 4 m/s
August 2, 2019 at 11:02 amRobAnsys Employee
Looks good: I'll take next week off and leave you in charge in here!
The lumpy residuals mean the model is slightly transient: the jets will be oscillating slightly which will affect the numerical convergence but not the overall result. Use monitor points to help judge when the model stops changing. I'd also look at the new Fluent Meshing Watertight Geometry workflow: that'll help with quality (usually) as poly cells are both easier and more accurate.
What boundary conditions did you use?
August 2, 2019 at 11:40 ampeteroznewmanSubscriber
Thanks Rob, I'm starting to go through the Fluent courses on the ANSYS Learning Hub, so give me a few months to get past the novice level. I will check out the new Fluent Meshing workflow soon. Ah, yes, oscillations in the flow, that makes sense.
Inlet is 0 Pressure, Outlet is the brown semicircle at -1000 Pa of Pressure.
What I found amazing on the previous model with the good mesh quality is that when I first ran the calculation, it settled on a solution where the flow was going in the opposite direction and was blowing into the nozzle from the outlet. I fixed that by Patching the inside domain with a +Z velocity.
August 2, 2019 at 2:28 pmRobAnsys Employee
Yes, if you check the lectures using pressure in & out can give some interesting results as the mass flow is part of the solution. Try with a negative velocity (outlet) and I suspect it'll be much easier to get going.
August 2, 2019 at 5:04 pmpeteroznewmanSubscriber
On further review, the initialization is what affects the convergence, not so much the mesh element quality. The following are both on Pressure Inlet and Outlet BCs. On the same good mesh, if I use Hybrid Initialization I get this convergence.
But if I use Standard Initialization, I get this convergence.
I will try negative velocity on the Outlet on another trial.
August 5, 2019 at 10:28 amRobAnsys Employee
Yes: as the mass flow is part of the solution with pressure boundaries the initial conditions are very important. There is a note in the Fluent lectures: recommended inlet/outlet boundary conditions.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.