Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Laminate post process
- Thread starter Irwin
- Start date
Hi Irwin,
When l use NASTRAN with laminates l get the forces and moments for the elements where l want to check. NASTRAN gives you directly N/m for the forces and N.m/m for the moments.
These values corresponds to the forces and moments of the laminate.
In order to check the lamina you can use the values of the forces and moments obtained with any software for laminates (the laminator gives good results).
Good luck,
Esteban
When l use NASTRAN with laminates l get the forces and moments for the elements where l want to check. NASTRAN gives you directly N/m for the forces and N.m/m for the moments.
These values corresponds to the forces and moments of the laminate.
In order to check the lamina you can use the values of the forces and moments obtained with any software for laminates (the laminator gives good results).
Good luck,
Esteban
- Thread starter
- #3
Irwin
I'm running an older version of NASTRAN (CSA), and here is some guidance from the User's Manual, Vol 1, Section 1.3.15, "Composite Material Structural Analysis".
"The action required on the part of the user to access layered composite analysis capability is very minimal. The user must insert the appropriate PCOMP and MAT8 data which describ e the composite laminate into the bulk data deck. Ply data recovery options are automatically performed in static analysis based on case control keywords of STRESS and FORCE. Stresses in individual lamina of the laminate, forces on the laminate and failure index tables for composite laminates will be provided in static analysis if STRESS and FORCE case control keywords are present."
In using CSA NASTRAN, I have found that you need to write the output to the .f06 file in order to recover the ply data. This means using STRESS = ALL and FORCE = ALL in the case control, instead of STRESS(corner,plot) = ALL. Then you have to import the analysis results into FEMAP by reading the resulting .f06 file. Once you read the .f06 file in, you will have the option to plot the ply failure criteria.
Another suggestion is that if your laminate has a core, you should model the core with brick elements, and the face sheets as composite laminates. That way, you can recover the XZ and YZ core stresses to compare with core shear allowables.
Regarding the ply failure criteria, you select the failure type on the property card in FEMAP.
Good Luck
J. Vorwald
P.S. I'd be interested in knowing more about the problem / application you are working on.
I'm running an older version of NASTRAN (CSA), and here is some guidance from the User's Manual, Vol 1, Section 1.3.15, "Composite Material Structural Analysis".
"The action required on the part of the user to access layered composite analysis capability is very minimal. The user must insert the appropriate PCOMP and MAT8 data which describ e the composite laminate into the bulk data deck. Ply data recovery options are automatically performed in static analysis based on case control keywords of STRESS and FORCE. Stresses in individual lamina of the laminate, forces on the laminate and failure index tables for composite laminates will be provided in static analysis if STRESS and FORCE case control keywords are present."
In using CSA NASTRAN, I have found that you need to write the output to the .f06 file in order to recover the ply data. This means using STRESS = ALL and FORCE = ALL in the case control, instead of STRESS(corner,plot) = ALL. Then you have to import the analysis results into FEMAP by reading the resulting .f06 file. Once you read the .f06 file in, you will have the option to plot the ply failure criteria.
Another suggestion is that if your laminate has a core, you should model the core with brick elements, and the face sheets as composite laminates. That way, you can recover the XZ and YZ core stresses to compare with core shear allowables.
Regarding the ply failure criteria, you select the failure type on the property card in FEMAP.
Good Luck
J. Vorwald
P.S. I'd be interested in knowing more about the problem / application you are working on.
AdrianSonelly
Materials
J.Vorwald,
You mentioned that "Another suggestion is that if your laminate has a core, you should model the core with brick elements, and the face sheets as composite laminates. That way, you can recover the XZ and YZ core stresses to compare with core shear allowables."
I'd be very intersted to learn more about this - what would you suggest if core is honeycomb material?
Thanks
You mentioned that "Another suggestion is that if your laminate has a core, you should model the core with brick elements, and the face sheets as composite laminates. That way, you can recover the XZ and YZ core stresses to compare with core shear allowables."
I'd be very intersted to learn more about this - what would you suggest if core is honeycomb material?
Thanks
Most composite post-processors will give you out-of-plane core shear stresses when you model the plate as a laminate. If the core is a honeycomb material, you can still input the properties as orthotropic and apply them to the proper layer in your laminate. When you post-process, you can see the out-of-plane shear in that particular layer.
Garland E. Borowski, PE
Garland E. Borowski, PE
I have modeled Aramid honeycomb core with solid elements (CHEXA) using anisotropic material cards (MAT9). I specified appropriate values for G33 (Ezz), G55 (Gyz), and G66 (Gzx), and entered small values for G11 (Exx), G22 (Eyy), and G44 (Gxy). Please make sure that the material orientation is correct for the solids and plate elements, and the same for all the elements.
- Status
Similar threads
- Locked
- Question