Composite Failure Analysis using MSC Nastran / HyperMesh
Composite Failure Analysis using MSC Nastran / HyperMesh
(OP)
Hi all,
I am new to this forum and have a question concerning composite failure analysis. I wasn't able to solve my problem with the existing threads, hence this new one.
I am currently working on a sandwich structure which is made from an aluminium honeycomb core and carbon fibre UD/epoxy faces. I have created different types of models to analyze deformation under load using Hypermesh (v2017.3) as a pre-processor, MSC Nastran (v2018.2) as a solver and HyperView (v2017.3) as a post-processor. This particular model of the sandwich is a rectangular 2d shell mesh, onto which I applied the PCOMP property. Within PCOMP I specified a 17-ply Laminate, where plies 1 to 8 and 10 to 16 are the face plies and ply 9 is the honeycomb core. I set Failure Theory (FT) to HOFF (Hoffmann) and also specified Bond Shear Strength (SB). The ply material is MAT8 (orthotropic), for the core I am using MAT2 (shell anisotropic). I specified all the required material Parameters (max. stresses etc).
Using Sol 101 I get my deformation and stress results "ply by ply", as desired. I am now trying to get an output of ply-by-ply failure indeces (FI) / strength ratios (SR), preferably the latter, but whichever is fine. I have set PARAMS,NOCOMPS,1 as others have pointed out on the forum. I am unable to locate any failure-related results in the .f06-file.
What am I missing?
Please note that I have only started working with Nastran and Hypermesh a month ago.
Kind regards
I am new to this forum and have a question concerning composite failure analysis. I wasn't able to solve my problem with the existing threads, hence this new one.
I am currently working on a sandwich structure which is made from an aluminium honeycomb core and carbon fibre UD/epoxy faces. I have created different types of models to analyze deformation under load using Hypermesh (v2017.3) as a pre-processor, MSC Nastran (v2018.2) as a solver and HyperView (v2017.3) as a post-processor. This particular model of the sandwich is a rectangular 2d shell mesh, onto which I applied the PCOMP property. Within PCOMP I specified a 17-ply Laminate, where plies 1 to 8 and 10 to 16 are the face plies and ply 9 is the honeycomb core. I set Failure Theory (FT) to HOFF (Hoffmann) and also specified Bond Shear Strength (SB). The ply material is MAT8 (orthotropic), for the core I am using MAT2 (shell anisotropic). I specified all the required material Parameters (max. stresses etc).
Using Sol 101 I get my deformation and stress results "ply by ply", as desired. I am now trying to get an output of ply-by-ply failure indeces (FI) / strength ratios (SR), preferably the latter, but whichever is fine. I have set PARAMS,NOCOMPS,1 as others have pointed out on the forum. I am unable to locate any failure-related results in the .f06-file.
What am I missing?
Please note that I have only started working with Nastran and Hypermesh a month ago.
Kind regards
Talk To Other Members
RE: Composite Failure Analysis using MSC Nastran / HyperMesh
I got the Failure Indices to appear in the F06-File. The reason for them not appearing was that under "Load Steps > Subcase Options > DISPLACEMENT" and "Load Steps > Subcase Options > STRESS" I had "FORMAT" set to "PLOT" instead of "PRINT".
However, I am still unable to view the failure indices in HyperView. I have seen other people access them via the Contour tool and then choose "Composite Failure" from the drop-down menu.
Ideas?
EDIT: Here's my BDF file Header.
---
Executive Control Cards
---
SOL 101
CEND
---
Case Control Cards
---
ECHO=NONE
$
$HMNAME LOADSTEP 2"Lastfall A Einzellast"
SUBCASE 2
LABEL= Lastfall A Einzellast
SPC = 1
LOAD = 2
ANALYSIS = STATICS
DISPLACEMENT(SORT1,PLOT,PRINT,REAL) = ALL
STRAIN(SORT1,PLOT,PRINT,REAL,VONMISES) = ALL
STRESS(SORT1,PLOT,PRINT,REAL,VONMISES) = ALL
---
Bulk Data Cards
---
BEGIN BULK
PARAM,NOCOMPS,1
PARAM,POST,0
PARAM,PCOMPRM,1
PARAM,SRCOMPS,YES
$HMNAME SYSTCOL 1"Local System"
$HWCOLOR SYSTCOL 1 5
$$
$$ SYSTEM Data
RE: Composite Failure Analysis using MSC Nastran / HyperMesh
I have found a solution. In HyperMesh, I set PARAM,POST,-1 and GLOBAL_OUTPUT_REQUEST,STRESS(SORT1,PUNCH,REAL,VONMISES) and GLOBAL_OUTPUT_REQUEST,STRAIN(SORT1,PUNCH,REAL), so that .op2-file is created.
To make sure that all Nastran results are kept, I entered "scratch=no" when running the .bdf-file in Nastran (not sure if this is really necessary, as it should only affect the .DBALL and .MASTER-files).
I then opened the .bdf and the .op2 in HyperView, choosing "Advanced" from the "Results-Math template" drop down menu. I can now choose "Failure Index (s)" in the Contour Panel.
Maybe this might be useful for somebody in the future...