×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*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.

Students Click Here

Jobs

Composite Failure Analysis using MSC Nastran / HyperMesh

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
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

(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.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members! Already a Member? Login


Resources


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:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close