[SeanQuallen]

Hello! I have a blade tip surface mesh that I'm trying to extrude into a 3d block (see the first attached picture). However, whenever I do so I get skew errors caused by lines overlapping each other on the extrusion front (see second picture).

I couldn't possibly list everything I've tried to correct this, but some parameters I should mention:

• I'm using a very small splay value (1e-4) for the 'open' edges and poles on each half of the blade, otherwise they fold over themselves.
• I get ~40 layers before skew if I use algebraic extrusion. I get skew immediately if I use hyperbolic. What I have been using is 10 layers of algebraic, and then switching to hyperbolic (I need 130 layers total). When I do this I get skew at ~70 hyperbolic layers in the form of the picture shown below.
• I've played with all of the hyperbolic smoothing parameters, including setting them all to zero and setting them all to very high values (max for Volume and Kinsey-Barth), but still get skew problems.

If anyone has any ideas I'd really appreciate it. Note that I'm a Pointwise/meshing novice such that I might be missing something very basic. Please don't hesitate to point out something incredibly simple out of fear of condescension.



Thanks!


Sean

[cnsidero]

Sean,

I see that you have a pole in your domain. My experience has been to avoid poles in domains that you want to use the hyperbolic extrusion from. They seem to make the algorithm unstable.

All is not lost though. It's relatively straightforward to replace the pole with an O-H topology. Briefly, the steps would be:

- split the domain along a circumferential grid line
- delete the pole, which will in turn delete the small domain resulting from the preceding split
- split the connector at the inner boundary of the remaining domain in two places. Split it such that the resulting first and third connectors have same number of points
- re-dimension the two free connectors left over from the deleted domain such that the sum of the number of points on both minus 1 equals the second connector from the preceding split
- assemble a structured domain from the four connectors
- smooth the two domains with the solver. Pick both domains, Grid>Solve, Edge Attributes, set the Boundary Conditions to Floating. Back to Solve tab and run 10-20 iterations.

The attached images demonstrate this idea on a simple domain.

[SeanQuallen]

Thanks Chris. I have moved away from using pole domains for my block extrusion as I need the result to be a single block. However I now have a new problem, but I'm creating a separate thread for it.