-Rightclick on connection , choose "automatically"
-choose at least 2 solids, confirm with "ok"
-choose connectionproperties : "contact"
-choose connectiontype: "surface to surface"
-confirm with ok
-Rightclick on properties , choose "new"
-choose maximum contact search distance : 0,1
-confirm with "ok"
-Rightclick on Region, choose "new connectionregion"
-choose "surfaces", than select the contact surface on your solid and confirm with "ok"
-same process for the other contact surface
-Rightclick on "connections" in the folder connections and there on "new"
-choose your propertie
-choose your master and slave surfaces
-confirm with "ok"
I´ve tried both of this ways:
analysis with the automatically connection --> no problem
analysis with the manual connection --> 3 fatal errors : 316 , 9002 and "one or more fatal errors has been occurred"
can somebody explain this ?
Solved! Go to Solution.
I prefer always to use manual connections method with command "CONNECTION > SURFACE", is quite far superior to automatic way when dealing with 2-D Shell models because FEMAP reorient properly surfaces on SOURCE/TARGET regions to make them oriented against each-other.
When dealing with solids is not critical because surface orientation is always outward the solid body faces.
Post your model here to take a look to it see what is really happening, OK?.
A picture is useless, we don't see the internal contact definition how is done, simply post your FEMAP file (*.modfem).
Compress your file using WinZIP or WinRAR and you will be able to upload your FEMAP file.
NX NASTRAN NONLINEAR analysis (SOL106) do not support surface-to-surface contact, here you need to use explicitly node-to-node CGAP 1-D contact element. You need to have matching meshes between both parts in the region of contact (simply split both parts) in order to create CGAP contact 1-D elements (use command "Mesh > Connect > Closets Link" to generate the CGAP elements).
Ahh!!!, I see the problem, after revising your contact property now I see the problem (I reported this error to FEMAP guys last week, the same error coming from one of our customers!!): in the NX NASTRAN linear contact property you have ZERO values!!. This is an slip from FEMAP guys, the default values should not be zero, this is the cause of the error.
But the problem has a very easy solution: simply click on DEFAULTS button and the empty fields will be filled with reasonable values!!.
Please remember this is valid only for Linear Static Contact surface-to-surface problems using NX NASTRAN (SOL101), for nonlinear analysis (SOL106) not matter the value you enter is useless, the only contact element available for 3-D problems is the CGAP element (apart of slide line contact).
Here you are the contact problem solved as linear static: please note the solution is useless, not valid at all: the resultant displacement has a value of 23.73, but the arm height dimension is only 5.0, then the problem is as minimum highly nonlinear by the geometry (large displacement effect), then the linear static analysis is useless, simply colors ... not real at all.
To account for surface-to-surface contact you need to run the ADVANCED NONLINEAR module of NX NASTRAN (SOL601).
Please if you look for accurate results try to mesh with CHEXA elements with minimum three elements in the thickness, forgot at all tetrahedral elements, only use them when the geometry is complex and not remedy, but in simply parts HEX meshing should be dominant!!.