[kasto89]

hello all,

i have a problem in initialization of a block. I can not understand why pointwise builds some pyramids on the external side of the surfaces. I attach a picture.

thanks

[cnsidero]

Originally Posted by kasto89

hello all,

i have a problem in initialization of a block. I can not understand why pointwise builds some pyramids on the external side of the surfaces. I attach a picture.

thanks

Can you give us a little more information. Is it unstructured, structured or hybrid (prism+unstructured)? Did you examine the mesh in Pointwise? Is it OK there?

[kasto89]

the external surfaces of the cylinder are structured domains, the base circular area of the cylinder is an unstructured domain; the block is unstructured.

I built an other cylinder in the same way and i have not this issue.

I attach some pictures for a better explanation.
In the first picture you can see how i built the block, in the second one it is possible to observe the "external" pyramids on the surface.


thanks

[cnsidero]

Originally Posted by kasto89

the external surfaces of the cylinder are structured domains, the base circular area of the cylinder is an unstructured domain; the block is unstructured.

I built an other cylinder in the same way and i have not this issue.

I attach some pictures for a better explanation.
In the first picture you can see how i built the block, in the second one it is possible to observe the "external" pyramids on the surface.

thanks

Thanks. Much clearer. Somehow the block face normal got flipped. To confirm, select the block with pyramids pointing out and go into the block solver. You'll probably see the pyramids (dark grey outlines) on the wrong side of the wall. To fix it, get out of the solver, go to Edit > Add/Remove Faces ..., click Begin Flip Face Orientation, pick the (only) face, click End Flip Face Orientation, and OK. Re-export the mesh.

That should fix it.

I see you're using OpenFOAM so I'll offer another tip. If you haven't already, I highly recommend using renumberMesh, e.g.:

renumberMesh -overwrite

to reduce the matrix bandwidth. Pointwise meshes rarely, if ever, have even close to optimal point ordering and renumbering the mesh will help convergence. I've found cases where the solution won't converge without renumbering first.

[kasto89]

thank you very much, you resolved me a very annoying problem.

Can you help me to obtain the block extruding the base circular area? if i try to use as path one of the connector on lateral surface I can not match the other circular base, so the real stl.

thanks

[cnsidero]

Originally Posted by kasto89

thank you very much, you resolved me a very annoying problem.

Can you help me to obtain the block extruding the base circular area? if i try to use as path one of the connector on lateral surface I can not match the other circular base, so the real stl.

thanks

I believe you're trying extrude the triangles along the length of the curving pipe, correct? If the pipe is truly circular along the path, you will need to find/create the curve that's the pipe axis and use the pipe axis to Extrude by Path along. Be sure to enable to the Path Rotation option during the extrude so the face stays perpendicular to the path direction.

If this doesn't work, I would suggest making a structured mesh on the circular ends of the pipe, then along with the domains on the side of the pipe assemble a structured block.

[kasto89]

Yes, It is correct! I have already though to extrude the base using the "axys curve" as path, but i do not know how to draw it, is there a strategy?

I does not build a structured block because the other one downside contains a valve, so i have to make it unstructured and I do not want a strength change of shape of cells at the interface between the 2 blocks.
Sorry for my poor English and thank you very much.

[cnsidero]

Originally Posted by kasto89

Yes, It is correct! I have already though to extrude the base using the "axys curve" as path, but i do not know how to draw it, is there a strategy?

My first suggestion would be to see if you can extract it or rebuild it using the original CAD software that generated the geometry.

If this is not option, you can try to rebuild it in Pointwise. The success of doing so depends on the how the pipe's trajectory changes shape. If does something simple like a circular bend that this shouldn't be hard. If however it's a more general shape it'll be harder.

This difficult to explain in words so here it is in pictures (the number refers the image name suffix)

01: my pipe has a straight section, followed by a circular bend, followed by another straight section.
02: create a straight 2 pt curve across the diameter of the circular cross section
03: split the previous 2 pt curve in the middle
04: create a db point at split location (delete two curves). the point will be at the center of the cross section.
05: repeat 02 thru 04 for each cross section. Mine has 4.
06: draw appropriate curve type between each point. Mine is straight 2 pt curve, circular arc and another 2 pt curve.
07: final trajectory. create a connector(s) on trajectory that canbe used to drive path based extrusion

As I mentioned the trick will be knowing the trajectory path. If it's simple things like straight lines or circular bends, it should be no problem. Otherwise you'll have to guess and use a more general curve type (Bezier or Conic).

Good luck, Chris

[cnsidero]

Last two images.

[kasto89]

ok, thank you very much, i have already tried something like that.
now I have an other problem, I cannot initialized an unstructured block, "one or more entities could not be initialize";

ok solved, i had a bad surface

[bharatesh]

Hi guys,
even i have similar problem. I'm using Windows platform(32 bit), and the total cells are roughly 2 million, after creating the Block, when tried to 'initialize', the file is processed for some time and i get an error saying "One or more entities could not be initialized", i don't understand which entities could not be initialized!.


System info:
platform: Windows XP (32bit)
RAM: 1GB

Can somebody help me please..

[jchawner]

When an unstructured volume mesh cannot be initialized it's usually because the mesher cannot recover the surface cells. Therefore, check the quality of all the surface meshes on the block's faces.

Hope this helps.

[bharatesh]

Originally Posted by jchawner

When an unstructured volume mesh cannot be initialized it's usually because the mesher cannot recover the surface cells. Therefore, check the quality of all the surface meshes on the block's faces.

Hope this helps.

Thanks John Chawner,
I got the issue resolved, however i'm facing new one.. What I did is:-
1. Completed the meshing with 1.44 million cells (approx.),
2. Imported mesh file in .cas format to Ansys Fluent 14
3. Did Mesh Check, appears to be okay, and Orthogonal Quality is 0.12
4. When I try to Run the file in the solver, it says that the Max Skewness is more than 0.98. Since I did not get any warning message while doing mesh check, its now bothering me alot..
5. How can I reduce the Skewness??

I examined the mesh file in Pointwise, the 'Max. Included Angle' appears to be well below 173. Attaching the 'Centroid Skewness' screenshot.

[jchawner]

It seems that your best approach would be to determine which of Pointwise's skewness metrics best matches what Fluent calls "Max Skewness" and look at it in the Examine command and use the Extrema function to zoom in to it's maximum value. See what's going on there and take appropriate action.