I am having an issue with inserting a surface point mesh in the middle of a hole using Meshing Tool Box -> Feature Removal Option. I mean FEMAP gets rid of the holes (loops) from the surface but some how it is not inserting a surface point mesh. And I need the point so that I can insert 1D elements later.
Any suggestions on how I can manually or make the FEMAP insert the surface mesh point. The model has a lot of holes and I prefer FEMAP to introduce it automatically, but I will take the option to insert it manually even if the task is tedious.
I do not see any problem (I run FEMAP V11.2.2), here you are a surface with holes:
I mesh the surface in the MESHING TOOLBOX with horrible "automatic" mesh surface command (I always "work" the geometry to arrive to a correct & quality "mapped" QUAD mesh!!):
Next I issue command Feature Removal > Loops and FEMAP will create points at the center of the holes. To show them please make sure you have activated POINTS for visualization!! (use Ctrl+Q > Geometry > Points).
There's a chance the point will not create if it is not a constant radius arc/circle. But to be thorough...
If the symptom is that the point is not visible, then you may want to check that eg. the current active layer is a visible layer, or Automatic Add is on if using a Group.
You perhaps might need to try any operation which selects all points before/after your feature removal operation, just to see if the same number of points are present in the model. Or, you may want to mesh the surface anyway to see what happens.
If the symptom is that the point appears, but the mesh does not use the point, then if you are using the Meshing Toolbox, then you need to check the Advanced Option -> Use Internal Points as Mesh Locations.
If that provides no hint of the problem, then try using Mesh -> Geom -> Surface, which meshes to Mesh Points by default.
If there are truly no new points being created via the Add Mesh Point option in Feature Removal (might not work if the curve does not have a constant flat radius), then...
(a) Create all the points manually via Geometry -> Point using whatever method is most convenient (if Method -> Centre does not work, that probably indicates why it does not work for Feature Removal)
(b) Mesh -> Mesh Control -> Mesh Points on Surface ... Select Surface -> Use Existing Points.
(c) then Mesh the surface by your preferred method, making sure to check the Advanced Option as indicated above if using the Meshing Toolbox to mesh the surface
Thanks for the replies. I am still having issues. Let me illustrate it with images.
Blas, thanks for illustrating the procedure. But I was aware of the same and it has worked for me many times in the past.
EndZ, the strange thing is that I can create a point at the center of the circle using Point->Center command but somehow the Feature Removal tool is not placing a mesh point at the center.
I have checked the active layer & stuff and the appropriate layer is indeed active.
Most of the images are self-explanatory.
I wanted to see if there are multiple surfaces in that region. But there is only one surface.
May be I can do Midsurface->Intersect command or any other similar commands to make sure that FEMAP recognizes where to place the surface mesh point?
Would appreciate additional inputs...
Perhaps try a Geometry -> Solid -> Cleanup in advance of doing the feature removal (tick all four basic options, unless you have geometry printed on the solid, in which case you could untick "Remove Redundant Geometry"). This sometimes helps tidy up the internal paranetric definition of the surface(s).
If that doesn't work, there are the tiniest collection of cicrumstances where true 3D commands can still be influenced by the orientation of the workplane. Not sure if this is one of them, but I suggest you try the Tools -> Workplane in a substantially different orientation, eg. the global XZ plane if it hasn't been moved from its default XY position.
It's similar to a Cleanup, but... File -> Export -> Geom -> Parasolids... and choose the sheet solid. Then reimport to a new model and also give it a try. This may have more of an effect if the geometry started as STEP or .SAT or other non-parasolid origin.
Finally, I assume all your solid/surface geometry fits in the magic Parasolid cube of 500 units (multipled by File -> Preferences -> Geometry -> Solid Geometry Scale Factor ) centred at the origin. Eg. if your scale factor is set to inches, then the geometry needs to sit in ~20,000 unit cube centred at the origin. Thus, it is unwise to install Femap, change no Scale Factor preferences, and then start working on models that are supposed to be mm - unless they are reasonably small structures (ie. less than 20,000 units). This last option is a real long shot... as I would have expected substantially different symptoms.
I think Solid-> Clean Up command worked. I am able to get a surface mesh point bang right in the hole center.
Such a simple command which was overlooked and costed me some time. Oh well, its all a learning process.
Thanks for replying. Appreciate it...
Revise your settings in FILE > PREFERENCES > GEOMETRY, because this is an error very common that I see between our FEMAP users and customers: to mix geometries with different scales factors!!. In fact, some users after installing a new version of FEMAP forgot at all to run FILE > PREFERENCES command, importing geometry in the default solid scale factor, (ie, inches) believing that they are working in millimeters, then the error. But when the user perform any operation with the geometry (for instance, midsurfacing) FEMAP always use internally the SOLID GEOMETRY scale factor set in PREFERENCES, then the resultant geometry generated by FEMAP is not correct. This could be a reason that surely in your model the points are created, but at another scale.
The command SOLID > GEOMETRY > CLEANUP performs an important task (between others) that is "Matching Model Scale Factor": If you have a model containing geometry in more than one scale factor, this command will take all selected geometry and adjust the geometry’s internal scale factor to the Solid Geometry Scale Factor that is currently set in File > Preferences > Geometry.
Before you run this command you may want to see the current scale factor of your solids, simply run command "List > Geometry > Solids > SELECT ALL" and you will see the following listing (if your scale factor dons't mach, then you have the answer!!):
List Solids 1 Solid(s) Selected... Solid 2 - Subtract Body Address: 78 Scale: 1000.