×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Are you an
Engineering professional?
Join Eng-Tips Forums!
• Talk With Other Members
• Be Notified Of Responses
• Keyword Search
Favorite Forums
• Automated Signatures
• Best Of All, It's Free!

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

#### Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

# 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

### RE: Composite Failure Analysis using MSC Nastran / HyperMesh

(OP)
Update:
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
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

(OP)
Hi everyone,

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...

#### Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

#### Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Close Box

# Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

• Talk To Other Members
• Notification Of Responses To Questions
• Favorite Forums One Click Access
• Keyword Search Of All Posts, And More...

Register now while it's still free!