Eng-Tips is the largest engineering community on the Internet
Intelligent Work Forums for Engineering Professionals
-
Congratulations waross on being selected by the Tek-Tips community for having the most helpful posts in the forums last week. Way to Go!
assembly
- Thread starter kotawsu
- Start date
FEMAP operates on properties and materials, not really "groups" as you might see in a CAD file. You basically install the entire assembly, whatever it may be, into FEMAP and mesh the assembly with each part being a different "property" and/or "material". You associate the mesh with a particular property and material either during the meshing process, or you may change it by updating the mesh to a new property and/or material.
For instance, if I bring in an FE model from another software package, it will have groups that FEMAP understand and it will characterize those groups as "properties" and "materials". Look up "Create Group" in the FEMAP documentation and it will tell you how to group the different properties for visualization, but this does not alter the (virtual) physical characteristics. You may also select individual elements or entire groups and update their properties and/or materials.
Hope this gets you headed in the right direction.
Garland E. Borowski, PE
For instance, if I bring in an FE model from another software package, it will have groups that FEMAP understand and it will characterize those groups as "properties" and "materials". Look up "Create Group" in the FEMAP documentation and it will tell you how to group the different properties for visualization, but this does not alter the (virtual) physical characteristics. You may also select individual elements or entire groups and update their properties and/or materials.
Hope this gets you headed in the right direction.
Garland E. Borowski, PE
- Thread starter
- #3
It depends on how many parts you have, and how many people are doing the work.
If you have a reasonable complex project, with more than thirty parts, you may want to develop some modeling guidelines. Things to consider are 1) nodes from different parts lining up, 2) the consistent resolution of details (curves, holes, thickness changes, etc), and 3) the fastening of the different parts. Also, detailed models of multiple, assembled parts don’t make much practical sense due to the large volume of output and the run times required. You may want to divide the assembly into sub assemblies based on loaded area. Or, develop a total assembly model using a reasonably coarse grid with the ability to transfer internal loads from the coarse model to detailed models of the parts.
Also, if you have a lot of parts to assemble, you may want to generate the part finite element models programmatically, in case you have to change some of your guidelines. Pick an area of your assembly with five to ten parts in multiple planes, connected with different types of fasteners, in order to evaluate/develop the modeling guidelines.
If you have a reasonable complex project, with more than thirty parts, you may want to develop some modeling guidelines. Things to consider are 1) nodes from different parts lining up, 2) the consistent resolution of details (curves, holes, thickness changes, etc), and 3) the fastening of the different parts. Also, detailed models of multiple, assembled parts don’t make much practical sense due to the large volume of output and the run times required. You may want to divide the assembly into sub assemblies based on loaded area. Or, develop a total assembly model using a reasonably coarse grid with the ability to transfer internal loads from the coarse model to detailed models of the parts.
Also, if you have a lot of parts to assemble, you may want to generate the part finite element models programmatically, in case you have to change some of your guidelines. Pick an area of your assembly with five to ten parts in multiple planes, connected with different types of fasteners, in order to evaluate/develop the modeling guidelines.
- Thread starter
- #5
There are two reasons to "tie nodes." One reason is to transfer loads from one part to the next, in which case you could use a rigid element, possibly with some of the rotation degrees of freedom released. A second reason is to evaluate the stresses internal to the fastener (bolt, weld, rivet, surface contact, etc), in which case you make a appropriate finite element model from beam and/or solid elements.
In summary, to tie the nodes, use rigid elements if you just want to transfer load, or use bolt / solid elements if you are concerned about the failure of the fastner.
In summary, to tie the nodes, use rigid elements if you just want to transfer load, or use bolt / solid elements if you are concerned about the failure of the fastner.
- Thread starter
- #7
SWComposites
Aerospace
No, there is no feature in NE_Nastran/FEMAP similar to the assembly module in Abaqus. You can connect parts together by simply using common nodes or by connecting individual pairs of coincident nodes with MPC's or rigid elements. You should not try to connect groups of nodes with rigid elements unless you have a very good and detailed understanding of how rigid elements work and their effect on the model - they are easily misused and can add excessive and unrealistic stiffness to the model.
- Status
