First of all, try to solve with the direct solver instead of the iterative one.
You will see in the f06 file that there is some nodes that are not constrained and rigid body motion appears.
This is because you split a body but you did not verified if the mesh was continu between the splits.
Use the command "duplicate node" to identify where mesh is not conntiue (two nodes at the same position and from different meshes).
Here is a solution:
-Unfreez all your meshes (right click on the mesh and unlock)
-delete all the 3D meshes (right click on the meshes and delete)
-use the command mesh mating and select all the bodies and OK: this will alloy mesh continuity between splitted parts!
-use the command 3D Swept mesh, with option multi body target. And select the parts in the right order ( first the part at the center , select like a snail shell). make sur the collector is the one you already created.
Then just launch the analysis.
Your fem should be like this (made with NX 11):
Wazy, you have elements in your model which are too long (those near hole) - their length is greater than width about 4 times of more, this gives inaccuracies on the solution. You should make them appear more square.
There is no difference using NX or Abaqus. Both will do the job. The real question is : Is the mesh fine enough to have a real stress value? And this does not depend of the solver but the mesh size.
Personnaly, i prefer NX because mesh control is far better but one more time the question here is not the solver but the mesh.
We know that the main stress will appear near to the hole, so the main point of this analysis is to have a fine mesh around it.
To do so, open the fem file and refine the mesh around the hole. The value of the stress will then converge to the real value.
A simple method to verify if the mesh is fine enough is to compare the "elemental node" stress with (These are extrpolated stress from gauss point to nodes) the "elemental stress" (these are the mean of the gauss point stress for one element).
An another way to improve quality is to mesh with HEXA 20 instead of HEXA 8 element (higher order). Edit your meshes and change the element type.
It is really a pain. I give up for almost most the day trying. do the same with 2D model but it did not works.
I used modal analysis and the part works as one piece. I can see their displacement but for the whole body.
I hope to know what basics I am missing to get stuck in this issue all that time.
1-create mode (NX)..draw the simple mode 2D and extrude to the 3D.
2-mid surface pair faces-
3-partition the midsuface to the required parts.
4-FE-mesh 2d elements>material+thickness defined
5- duplicate node (there is no duplicate!)
6-mesh mating (glue-coincident is not supported for shell element)
7-mesh mating (glue-non-coincident assigned)--did not work to select all the body and mate--so each two faces mated together (one face be master once and the slave another)
DOF1 of node 2862 has been found in both the M-set DOF's and in the S-set DOF's. The DOF
has been set by mesh "RBE3 Collector(2):manual_mmc_3_mesh" and by constraint
SUGGESTION: Set parameter "AUTOMPC" to "YES" in the "Solution Attributes..." dialog.
failed to solved with or without mating. fo6 file refers to the rigid body motion error.
Thanks in advance
With 2D mesh the continuity is ensured by the fonction "sticth edge", since the continuity passes through edge and not face (mesh mating wont work as you saw).
Delete all the MMC connector created with the mesh mating you tried (in the simulation navigator, after the 2D collectors). And delete all the RBE3 element that are created too.
Then hide the meshes and display only the midsurface, click on the command "stitch edge ", the unstitched edge will appear in red. Select the automatic method, then edge to edge and click on all the surfaces.
Update the mesh and relaunch the analysis. This will work.