[aunmhd]

Dear ICEM Community,

I have a geometry comprising of a conical body in ICEM CFD. The geometry itself is pretty complex comprising of propeller blades mounted on a streamline body comprised of two cones. The overall quality metric (minimum) of the Pre-Mesh is 0.2 (I'm trying to improve this further a bit). The Determinant (3x3x3) of the Pre-Mesh however is giving me negative values only in one of the 6 Quarter O-Grids I have made around the conical tips in the front and back cones. Can somebody comment on why this is such and what I may do to fix this?

[bluebase]

Hi aunmhd,


it seems a few blocks might became inverted, because there isn't any element with a determinant close to zero.



there is a feature called "fix inverted blocks" you may try it a few times and see whether it fixed it.

[aunmhd]

Thanks bluebase,

The problem seemed to be originating from inverting blocks as you correctly pointed out. I was able to fix this issue by the 'Invert Selected Blocks' feature only selecting the blocks of the O-Grid. Using 'Fix Inverted Blocks' fixes the problem in the O-Grid but also inverts other blocks elsewhere in the domain which were otherwise properly 'aligned'. This continues in an endless loop where blocks are inverted rather randomly in the domain.

While we are on this could you please elaborate what is the significance of this quality metric determinant 3x3x3 and what minimum value is acceptable for solvers in general.

Thanks.

[AtoHM]

Determinant 3x3x3

[aunmhd]

Originally Posted by bluebase

Hi aunmhd,


it seems a few blocks might became inverted, because there isn't any element with a determinant close to zero.



there is a feature called "fix inverted blocks" you may try it a few times and see whether it fixed it.

Hey,

I require a boundary layer around my geometry (shown in red, blue and green).

If I create the Quarter O-Grids first and then try to create an O-Grid around the blocks, ICEM gives me an error.

I worked the other way around. Created an O-Grid around the blocks (boundary layer) and then created Quarter O-Grids. Although this did resolve the problem somewhat, however, it gives rise to elements with very poor hex element aspect ratios in the boundary layer.

Can you suggest how this issue may be fixed?

[bluebase]

Well, high aspect ratios in boundary layers is not inherently bad. It's important that the gradients are properly resolved. If the longest side is in flow direction in which gradients are small, then there is no problem. The large gradients normal to the surface are the ones you need to resolve, aren't they?


Regarding poor element, i can only give general recommendations: use the tools available!
Use quality histograms, and "scan plane" to study where those bad elements occur and why.
Try to figure out a way to make those bad elements into square boxes again.
This can be a lot of tedious work which hardly can be solved via a few written sentences...

[aunmhd]

Originally Posted by bluebase

Well, high aspect ratios in boundary layers is not inherently bad. It's important that the gradients are properly resolved. If the longest side is in flow direction in which gradients are small, then there is no problem. The large gradients normal to the surface are the ones you need to resolve, aren't they?


Regarding poor element, i can only give general recommendations: use the tools available!
Use quality histograms, and "scan plane" to study where those bad elements occur and why.
Try to figure out a way to make those bad elements into square boxes again.
This can be a lot of tedious work which hardly can be solved via a few written sentences...

Thank you for your reply.

The bad elements that I am unable to resolve are not a result of my blocking strategy. I have been careful with the angles. The problem arises when I add boundary layers to my model. I modelled the geometry in CATIA and upon import the algorithm applied to the surface transfer 'changes' the surfaces especially around the region where the propeller is attached to the spinner. The cell height based on y+ calculations is 1.4e-5 m. Once inflation layers are added, it gives rise to poor quality elements because of the surface quality. I tried modelling the spinner in ICEM but when I trim the surface with the curve at the propeller base, the problem persists. I export the geometry as .model file into CATIA.

Is there any way I can resolve this issue?

I have attached a photograph which shows part of the inflation layers and the 'smudged elements'.

[bluebase]

Is there any way I can resolve this issue?

I don't know exactly.

I think some imported surface might be triangulated internally. And 1e-5 is quite close to the default triangulation tolerance. Can you try to decrease (put a smaller value) the topology tolerance as well as the triangulation tolerance? At least two magnitudes smaller than your smallest characteristic length, so at least 1e-7.
You can find it somewhere in the settings, i think it is in the general options tab.

Then remesh.

Did that help?

[aunmhd]

Originally Posted by bluebase

I don't know exactly.

I think some imported surface might be triangulated internally. And 1e-5 is quite close to the default triangulation tolerance. Can you try to decrease (put a smaller value) the topology tolerance as well as the triangulation tolerance? At least two magnitudes smaller than your smallest characteristic length, so at least 1e-7.
You can find it somewhere in the settings, i think it is in the general options tab.

Then remesh.

Did that help?

The tolerance value can be edited while importing the geometry from CATIA. Like you suggested, I decreased the value to 1e-7. And . . . it works like a charm!

Thanks a million bluebase. Can't thank you enough. Cheers!