Tetrahedral meshing algorithm failed

[zhirayr]

Hi

What on earth does this mean. The faces are all meshed (tet), then once abaqus contructs the tetrahedral elements it gives an error "tetrahedral meshing algorithm failed". Can someone please help. I have a very twisty object that needs meshing and nothing is working

Zhirayr

 

[corus]

Try altering the global seeding or the local seeding to get it to mesh. Another problem is that you might have an error in the shape if you've imported it from a CAD drawing. Remove unwanted vertices and try correcting the geometry. Alternatively if you know where it might be failing try using the Virtual geometry to remove edges and small faces.

corus

 

[zhirayr]

Right that's most certainly correct. The part I'm importing is from Pro/Engineer 2002 (STP file) and is giving problems. I get a warning that the part has imprecise geometry (I have tried repairing but with no luck), and when I mesh a whole face is highlighted as the problem. I'm not sure what to do, I cannot simply remove this, but there may be something I can do in Pro/Eng to solve it (perhaps make the part less accurate!)

 

[corus]

In general I'd avoid importing parts, unless the geometry is particularly difficult, as it takes more time to correct the drawing than it does to create it yourself properly in CAE. Unfortunately managers attend courses on 'integrating the knowledge supply-chain' believing it will speed things up whereas a course on 'reality' would tell them differently.

I'd advise that you send the drawing back and ask them to draw it properly instead of leaving gaps everywhere. You could also partition the part into regions and then mesh each region separately. This will tell you where the problem lies. If you continually zoom into edges you'll probably find double lines or double points undicating that the part was drawn imprecisely. Try the Virtual gemoetry option in the mesh module to renove unwanted edges. This will make the mesh smooth over edges and make the geometry jagged with the deges of the elements. It's not a good result but if they couldn't be bothered to draw it properly in the first place what can they expect.

corus

 

[zhirayr]

Thank you very much for you help. I did in fact mesh the regions separately and figured out the problem.

Yours

Zhirayr

 

[brep]

Just a point here, "Imprecise" is not something to be abhorred... If you just want to tet mesh a part, then an imprecise part is most likely not going to need any "repair" at all. In fact, depending on the source CAD system, there is nothing you can do to make it "precise" since that orginal CAD data was modeled using very loose (in ACIS's definition) tolerance. Pro/E by default uses "relative tolerance" which can come back and bite you if you model something long/thin. Rel Tol gives an absolute tolerance value = (bounding box diagonal * rel_tol). I've seen this problem more times than I can remember. A couple of tips: use absolute tolerance (and make it small!) in your Pro/E start part, that way when you start a model you'll already know exaclt what tolerance you'll be regenerating to. Sometimes it is difficult to regenerate a part when you change the tolerance scheme midway through your design

Now, back to CAE. An imprecise part may cause problem with certain boolean operations, typically when you are doing extensive partitioning for structured meshing. Tet meshing is **specifically designed** to handle tolerant (imprecise) parts.

Finally, CAE provides (in the Tools-Query menu) a whole bunch of geometry diagnostics tools. You should use these to interrogate the model to find: short edges, sliver faces, free edges, shell faces etc etc etc. If you are using 6.5-1 then you'll be able to do a whole lot more now to repair bad geometry: repair small edges to collapse tiny edges, also try the merge edges to join a whole bunch of edges into one. This last comman works really well even if you drag select the whole model... Nice if you've imported a CATIA model with the typical problem of having multiple edges along curved faces. Another great query tool is Mesh Gaps/Intersections. Once you have a boundary mesh you should run this check to see if there are any overlapping triangles. Rather than try and make the tet mesher do something with this bad boundary, you can go back and add seeds, use geometry repair, use virtual topology...