04-23-2018 03:04 AM
Dear Nx Nastran Users,
I need to carry out elastic-plastic analysis on surface hardened component. It is induction hardened upto few depth where hardness is a variable thereby mechanical properties are varied from case to core. How to define the stress-strain properties with respect to hardenss along depth in Nx Nastran? If possible provide some simple analysis files.
06-19-2018 05:23 AM
If model thickness is small, then try to use laminates. If you have, for example 100 mm plate with 0,5 mm hardened layer, then try to wrap solids with plates or neglect this layer.
06-19-2018 05:28 AM
i am trying to get the effect of heat treatment on the structural behaviour of transmission component / shaft.
06-19-2018 06:38 AM
1) You heat shaft and know relation Elasticy modulus-Temperature and temperature distribution in model
2) or you use cold shaft with hardened surface and you know relation Yeld stress-Model depth? For most structural steels E of hardened layer is allmost equal to E non-hardened part.
In first case you can use nonlinear mterial with temperature dependent properties.
06-19-2018 06:59 AM
But the hardness along the thickness is is varied and how to define elasti-plastic property with respect to the variation ?
06-19-2018 07:15 AM - edited 06-19-2018 07:23 AM
Again, what do you mean by hardness - Elasticity modulus or Yield stress or both?
Lets imagine that different perts of steel have different stress-strain curves and you know property distribution along depth.
Then make isosurfaces and mesh model with some number of materials - brake material dependence into distrete number of steps.
or use macro to change material property according to element position.
If your shaft is symmetrcal - you can use temp dependent material and apply temperature load according to geometry position, with theraml expansion factor is zero you dont get additional thermal stress but your material properties vill vary.
06-19-2018 07:23 AM
I just mean that the heat treatment induces variation in hardness along depth thereby changes the flow curve. i need to examine the interface of case-core for the stress distribution while loading. many article represent it by partitioning the component and assigning different material property for the small layers along depth to represent the case hardness. but how to distribute it uniformly with respect to measured hardness profile. as you have mentioned, how to use macro to define the property with respect to element position ? is there any text available to read ?
06-19-2018 07:39 AM - edited 06-19-2018 07:41 AM
Unfortanately I dont familiar with API.
If your model have complicated geometry, then the better solution is to splin model.
If model is simple and distribution of hardening is lineat or radial, then there are some tips.
And hardness distribution will be discrete because element can have only one stress-strain curve value.
06-20-2018 05:07 AM - edited 06-20-2018 05:07 AM
As I know, it will work for 601 solver.
1. Make as many isosurfaces in some CAD application as you need.
2. Import all surfaces to Femap.
3. Mesh each surface with plate elements - you need to create nodes on surfeces to store temperature value at location.
4. Apply temperature loads at nodes on each isosurface. For example Isosurface with depth 0 - t=10 - not zero it is important!, depth = 1mm - t=10+1=11 deg. And so on.
5. Run steady state heat transfer analisys - with all nodes loaded with temperature - in results you get allthe same temperature as in loads. Now you get distribution of mterial properties in 3D. The temperture value is actualy value of depth from surface.
6. Open your solid shaft mesh, use tool Data Surface Editor -> Output Map Data Surface - and map temperature values from isosurface mesh to your model. Now you know depth of each node in structural model. Create temperature load from data surface.
7. I asume, that you know stress-strain curves for different depth. Make stress-strais curves for each depth in Femap. use type of function 13..Stress vs, Strain. Number functions like: 10 - 0 depth, 11 - 1mm depth, 12 - 2 mm depth and so on.
8. Make additional function type 5..Function vs. Temperature. Enter "temperature-depth" value as X and function id as Y.
9. Create nonlinear material, select type - Plastic, and select Function vs. Temperature in field - Function dependence. Set Thermal expanson coefficient to zero so temperature dont produce additional thermal stress and only affect the material properties.
06-25-2018 01:57 AM
You mentioned the iso surface of thermal distribution to mesh the model ? any idea how to use iso surface of thermal analysis to split body and mesh ?