while 3D „snap-fit“ analysis works very well in FEMAP 11.3.2, I run into troubles using 2D-axisymmetric elements. Strictly speaking, I couldn’t find a method to overcome the well-known stress peaks in the contact region.
First of all, I want to show some pictures about the 3D model, which works perfect.
I use CHEXA20 elements with mid nodes projected to surface, Contact INITPENE = 0, friction coeff = 0 and „Large Field (All But Elements)“ in Bulk Data Options.
Dimensions of snap-fit (0.1 mm interference)
Solution of Mises stress using the equivalent element size
Solution of Mises stress using non-equivalent element size
--> Perfect results!!
Same problem using axisymmetric elements:
Boundary conditions and permanent constraint: Ty, Rx, Rz
Furthermore, I use CQUADX8 elements with mid nodes, Contact INITPENE = 0, friction coeff = 0 and „Large Field (All But Elements)“ in Bulk Data Options.
The Stresses in the contact region are not satisfactory. Are there any additional settings, to solve that problem? Any suggestions?
I would be very happy, if anyone can help me!
Big thanks in advance!
Solved! Go to Solution.
Your EDGE CONTACT definition for SOURCE & TARGET regions is not correct, the OUTPUT should be NODES, not elements.
But after performing this modification and solving the model using NX NASTRAN (SOL101) solver the stress results contour don't have a reasonable good aspect, then I suggest to send the FEMAP model to GTAC for investigation, OK?.
thanks for your reply. What is the meaning of the different output options and in which cases do you use each of them? I couldn't find something in the NX Nastran documentation.
Could you send this file to GTAC for investigation please.
The same problems also occur using plain strain elements.
Thx in advance
I sent the model to FEMAP developers and realized the nodes are not exactly in the XZ plane, but instead have an Y coordinate of 3.061617E-15. Simply use command MODIFY > PROJECT > NODE > select ALL > to XZ plane, rerun the analysis and stress results now are reasonable:
Also is good to have all QUAD elements correctly oriented, make sure to have the same orientation in both parts, this is important when you plot normal stress, use command MODIFY > UPDATE ELEMENTS > ORIENT PLATE NORMAL and use the option FIRST EDGE:
great. Big thanks for your investigations!
First, I imported the original geometry from Autocad to FEMAP in XY plane. After rotation to XZ plane, the surface with its elements didn’t exactly lay on the XZ plane (offset 3e-15). This caused this unreasonable stress state in contact region. With projected nodes to the XZ plane everything works fine. Obviously, all nodes have to be exactly in the XZ plane. Good to know for further investigations.