I am having problems with simulating the resonance frequency of a component in NX 8.5 with Advanced Simulation. I am using the SOL103 Flexible Body. The result of the simulation, the .rfi file, will be used in a Motion Simulation. The component is for a test setup. The test is used to check if we can use a linear motor to put the component in its own resonance. The test setup looks like bellow.
If the motor change direction 15 times per second then it shouldn't be that the components will be in his own resonance.
The component is 60 mm in height, 90 mm wide and 50 mm in length. The flextures are 0.8 mm thick. The two solid blocks are 5 mm thick and the distance between the flextures is 28.4 mm.
The component is fixed by 4 bolts of the size m4. Around the the holes of the bolts I sketched a circle and divided the face so I can simulate a bolt connection with a 1D connector.
I started with Advanced Simulation and created a new FEM and SIM, with the following aspects. See the image bellow.
Following the creation of the new FEM and SIM I made a new SOL 103 Flexible solution. I left everything untouched. Case control looks like follows.
Then I mashed the component via 3D Tetrahedal Mesh. The mesh setup looks liks:
Then I added a material to the mesh. The material I added is ABS. The material properties are down below.
nformation listing created by : 446041
Date : 04/12/2018 14:46:54
Current work part : D:\Test_0001\test_0002\test_0003\Test_Flextures_0001_fem2.fem
Node name : czc517399x
Library Material : ABS
SubCategory ABS Polymer
Library Reference physicalmateriallibrary.xml
Category : PLASTIC
Sub-Category : ABS Polymer
Material Type : IsotropicMaterial
Version : 3.0
Mass Density (RHO) : 1.05e-006kg/mm^3
Young's Modulus (E) : 2000000mN/mm^2(kPa)
Poisson's Ratio (NU) : 0.4
Type of Nonlinearity (TYPE) : 1
Yield Function Criterion (YF) : 1
Hardening Rule (HR) : 1
Yield Strength : 40000mN/mm^2(kPa)
Thermal Expansion Coefficient (A) : 7e-0051/C
Thermal Conductivity (K) : 170microW/mm-C
Specific Heat (CP) : 1800000000microJ/kg-K
After assignen in the material I added 4 1D connector to simulate the bolt connection. The connection looks like:
Then I added the fixed degree of freedom constraints with all the DOFs fixed.
I did this to all the 1D connections.
Finally I solved the solutions. I do get results but the results seem way off. The following results were created.
I The component seems to got lose from the constraints. Also the frequencies are way to high for such small and light product. 130 Hertz, while my college using other software got around 36 hertz.
Sorry for the long post, but I spend quite a bit of time trying to solve this to no avail. Can anybody please help me?
Solved! Go to Solution.
what does the hand calc give you? see blevins Table 6.2, case 24 for example
At the moment I don't have access to Blevins. But the person in charge of the test already did the test in the past. And according to him the resonance frequency should be around 36 hertz.
Try to reduce element size. Use 3 elements per thickness, especialy here.
Also try to change your constraints. Your model should not have rigid body modes.
Can you share geometry in neutral format, like .x_t?
Model on screenshoots dont look like 60x90x50 mm.
Make plate model, give simple constraints (fixed on edge) and get first frequency 26,5 Hz.
Model have dimensions 60x90x50 but dont look like your model for some reasons.
Change dimensions to 90x60x50 - get 16 Hz.
40Hz, first try with brick elements with MSC Nastran and NX Nastran, built from your dimensions. I eyeballed the fillets at 2mm radius... All holes fixed (connected to a center node by RBE2, no different)
Apart from TET elements, your mesh is very coarse in the fillet region, I'd refine that at a minimum... But 136Hz given your dimensions is more than off, it is plain wrong. If I use your element size, I end up with 48Hz, 30% off, not 3000%, something elese is going on...
From the picture you posted, looks like your rigids are extending to the fillets, and there might be some other issues too...
There should be a note about back to basic: Is tet element (even tet10) really appropriate for such model!
PS: @TENTECHLLC: Is that MSc. Apex used?