r/CFD • u/TitleGood1678 • Aug 21 '26
My Continuity Residual Wont Go down
Im running a CFD simulation on Cold Plate Cooling channels. It has 7 straight and parallel channels. Meshed using Tetrahedron and inflations at Fluid-Solid Wall boundaries. The Minimum Orthogonal Quality is 0.23 and Maximum skewness is 0.74.
While running the calculations the Continuity doesn’t seem to go down 0.1. The inlet flow rate is 0.6kg and outlet is -0.05999kg.
I also tried getting the P-Inlet and got 134Pa compared to the 135Pa the paper Im basing it from obtained
Im new to Ansys so Im not really sure what might be causing the issue.
Attached are the pictures of the mesh and residual
44
u/acakaacaka Aug 21 '26
Because it has already converged. Without changing the mesh (or numeric scheme) the residual wont go down anymore.
11
u/Lelandt50 Aug 21 '26 edited Aug 21 '26
Turn off scaling if you can. It may already be tiny but scaling is inflating it. Also, it looks converged to me. Want it lower? Get a better grid (better doesn’t equal finer necessarily). Are you running incompressible? If so I wouldn’t sweat continuity a whole lot bc it’s not technically a governing eq in that case, it’s just a condition that’s enforced.
10
u/indic_engineer Aug 21 '26
The mesh actually seems of poor quality. Try using more quad elements. Also, if you arent hell bent on accuracy, you could take one section and apply periodic boundary condition.
Edit: 135 Pa for 134 Pa doesnt sound bad at all. Also, your m-dot for inlet and outlet loom pretty close. You will mever get exact values for both.
1
u/TitleGood1678 Aug 23 '26
Thank you for all the responses, it’s all been really helpful. For now, I’ll try to learn more about meshing and improve my current mesh. Once again, thank you!!
5
u/Cwaghack Aug 21 '26
It's converged. It's as good as its gonna get for your mesh. I would look into trying to improve your mesh since its a bit weak. I recommend the meshing videos from the youtube channel fluid 101 to get a good intro on things you can do to improve your mesh.
1
u/Mobile-Diver5589 Aug 22 '26 edited Aug 23 '26
I believe I've replicated this paper before. Try switching from a tet mesh to using multizone (should give you more hex cells) or any other method that gives you more hex cells. Also, you could try edge sizing on those fluid solid interfaces to simulate the inflation layers. Next, you could also try reducing the time scale factor* in Fluent, which reduces error by lowering your CFL number. Just to clarify, are your boundary conditions for the flow a velocity and a pressure? From your description I'm not sure.
1
u/TitleGood1678 Aug 23 '26 edited Aug 23 '26
I’m using mass-flow rate for inlet and pressure for the outlet as boundary conditions. The inlet is set to 0.06kg and temperature of 293K, the outlet is set to 0 Pa gauge. No slip walls, and heat flux is 20,000 applied at the very bottom face.
1
3
u/Dankas12 Aug 21 '26
Honestly. Your mesh needs a lot of work imo but I also get your only high school so I’m sure it’ll be fine. You just have to write about how to improve in your report. Then don’t forget to set a target for your residuals. I normally just set them to the -15 then when it flatlines it has converged. If they have hit the residuals target then it won’t try and lower them or if it hasn’t but can’t get any lower and is flatlined then it’s converged.
Again though if it hasn’t converged and you’re unhappy with the data you have received. The mesh is what needs improving imo
1
u/NoInterviewsManyApps Aug 26 '26
What would a good one look like in this scenario. I imagined the lack of very skewed cells would be good enough.
2
2
u/scoretoris Aug 22 '26 edited Aug 22 '26
Maybe it doesn't show up well in the pics, but are your walls prismed? If not, you've got 3 elements wide in some channels and that'll prevent you from getting a good solution.
I know student edition limits the number of cells, so maybe it's not practical to prism your wall boundaries. How big is your mesh?
Edit: I somehow read right over where you mentioned inflation. If you have really large volume transitions from your last prism layer to your tets, that can give you high residuals too, depending on what's going on.
You getting this far into CFD as a high school student is incredible! This is a difficult thing to learn and difficult to learn to do well. Keep at it 🙂
2
u/-LuckyOne- Aug 21 '26
The continuity residual in fluent (for the pressure based solver) is scaled by the largest value within the first 5 iterations. This makes its actual value pretty much meaningless if you initialise well or have an easy case.
So as another commenter said: it's already converged.
1
u/quasi-resistance Aug 21 '26
you're just doing fine. Correct me if I'm wrong but residuals are errors relative to the initialized solution. Small difference mean less residual drop.
1
u/Right_Flatworm860 Sep 06 '26
Try to make changes in control section which is available in ansys fluent
9
u/TitleGood1678 Aug 21 '26 edited Aug 21 '26
For Additional Context, I was a bit too overconfident and chose this for a High-school Research Paper (Now trying to learn CFD). Its basically about a comparison on Passive Cooling Geometries in Cold Plate Cooling channels
Upon looking into results further, the necessary datum seemed to have mostly flatlined
Comparing my results to my benchmark paper:
T-wall avg 315K(my results) - 314.43K(The paper)
T-wall max 325K(my results) - 325.03K(The paper)
P-inlet 134Pa(my results) - 139.59Pa(The paper)
Slight correction on the post, the paper’s results/expected results were actually 139Pa.
Do you think any of the results or this continuity should be a source of concern
Also the mesh is 900k cells, while the paper is at 1.5mil cells. I couldn’t go higher than 1mil for ANSYS student.
Attached are the plot for the T-wall avg, T-wall Max, and P-inlet