turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- CAE Simulation - Femap Forum
- Mesh problem on matched surfaces

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-12-2015 11:12 AM

I'm having problem creating tetrahedral mesh on my model. More precisely meshing two parts with matched surface i get following message:

Tet Mesh Solid

1 Solid(s) Selected...

Meshing Surfaces...

Unable to link mesh locations between Surfaces 4501 and 7165. Surfaces must be on same solid or must be coincident.

Merging...

233 Node(s) Merged.

Loading Elements...

Checking Elements...

Elements do not form a closed outer surface. There are free edges.

2 independent surfaces located. 0 voids.

MESHING SOLID 108 ______________________________________________________

-- SURFACE MESH 2 Triangles

-- SURFACE MESH QUALITY

MINIMUM ANGLE _____________________

25.0 > A > 15.0 1 Elements

0.5 > A > 0.0 1 Elements

Worst Angle = 0. Element 77281 (92752 92753 92755)

Shortest Edge = 0. Element 77281 (92752 92753 92755)

Longest Edge = 3. Element 77282 (92419 92753 92752)

>>> ERROR: ERR 5621

>>> ERROR: FACE 1 WITH VERTICES : 2 3 4

>>> ERROR: SMALL INRADIUS : 0.000000000000000E+000

Mesher Aborted...

*Surfaces must be on same solid or must be coincident* and they are coincidental, but mesh is only generated on one solid. I used Mesh Size on Solid with Assembly/Multi-Solid Sizing to achieve surface match.

What can cause this problem and is there some way to avoid it?

Just a little digression, what I'm actually trying to achieve is something similar to:

https://www.youtube.com/watch?v=s-udGFfR3QI

but with this method i get poor element quality, so i made triangular prisms to control elements in volume of solid.

Initial geometry.

Geometry after removing volume of prism.

Every help or advice is greatly appreciated. Thanks in advance.

6 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-12-2015 11:45 AM

Hello!,

The TET mesher runs OK if both surfaces are not only coincident, but have exactly the same geometry. I means that both surfaces should have the similar curves, length, size, etc..

Try to mesh the surfaces of the solids with 2-D PLOT-ONLY seed mesh, if your 2-D mesh is successful then the 3-D TET mesh will be OK.

Or post your FEMAP model here and we will take a look to it.

Best regards.,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-14-2015 10:01 AM

Thank you for your response Blas.

I always prepare surfaces so that they have same geometry.

I found that there are several issues that can cause the problem i described.

The easiest scenario is when you have completely identical surfaces, points and lines mach perfectly,mesher can't create mesh and reports that there are nodes that causes errors. Solution for this is just to create one or two slices across surfaces and it will help mesher to generate mesh.

Second scenario (that caused me a lot of headache) is caused while using Solid Remove. Edge on surface is divided in two places instead of one or it isn't divided at all. So now instead of just two break points on two coincident edge lines it ends up with more points. Distance between those points is around 3.5E-7.

Through whole model i use same order to get my geometry, and i get this problem only few times.

For this i used Move by Point and moved points that desen't mach and then return them all on same coordinate, but Move by Point doesen't always work on solids.

Do you know some of conditions in with Move by Point doesn't work on solid and is there some other method to deal with those points, because order of E-7 very small or there is some other tolerance and distance between those points is outside of tolerance for generating mesh.

Milan

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-14-2015 12:09 PM

Hello!,

A command I use a lot with success is **SOLID CLEANUP > ADVANCED** activating the option to remove small edges, this is a great command, and I use it when the standard **GEOMETRY > SOLID > SOLID CLEANUP** command do not remove small edges or sliver surfaces. Play with the small edge tolerance and you will see a great improvement, this is a little jewel hidden between commands available in FEMAP since many years, but really powerful.

In general I don't use MOVE BY POINT command a lot, depends of the problem type, better post your FEMAP model here to see the best approach to follow, OK?.

Also, is very important you run the newest version of **FEMAP V11.2.1**, you have a lot of enhancements in geometry manipulation, we are the ENVY of most CAD systems!!.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-17-2015 05:37 AM

Hello,

there is an another method to repair this problem. You can make combined surfaces and combined curves from problematic surfaces and curves. So you don't need to repair solids, and surfaces will match to mesh sizing.

Best regards

Peter

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-17-2015 12:34 PM

I completely overlooked Solid Cleanup. In past i only used Solid Cleanup to remove redundant geometry and sliver surfaces, but i will definitely check those advanced options.

I think that this is just what I needed, because my problems originates of very complex geometry. Just for reference, part of a model I'm working on (400x200x115m).

Thank you Blas, I appreciate your help.

Milan

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-17-2015 02:50 PM

Hello!,

**Peter**, I use a lot as well the MESHING TOOLBOX **Combined/Composite Curves & Combined/Boundary Surfaces** commands, but I see a problem here: if later I want to perform any geometry operation with solid (say GEOMETRY > SOLID > SLICE) then the solid body is difficult to edit, or at least the resulting geometry is not predictible. Then always I let the **Combined** commands under MESHING TOOLBOX for the very last step, when no more geometry editing is required.

**Milan**, I am happy you discover the SOLID CLEANUP >ADVANCED, I like it a lot because any change in the geometry is not radical, is like "natural" editing!.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc