Jump to content

Pull Out Sandwich Analysis

Recommended Posts


I am simulating a pull out test.

I built my model in accordance to some tutorials using a 3D mesh with mat9ort and PSolid to the honeycomb and two 2D mesh to the carbon fiber layers with mat8 and Pcompp.

After the model is running i made a test specimen and test it. The problem is that my model is much more rigid than the real life (see the graph).


To apply the force i use an eye screw and a backing plate that i had modeled too and used some contacts between the test rig and the plate and between the backing plate and the sandwich plate. These are the only constraints applyed to the sandwich plate.


Could someone help me with this? I dont know why there is this difference between the model and the real test

Attached is the model





Share this post

Link to post
Share on other sites

I believe you have some modelling inconsistency in your model.

Upper arm thickness coincide with parte cima.

Define contact between puxator and upper arm or honeycomb.Try all with freeze contact.

Not sure about the graph.Is that Displacement vs Force graph?

In above shared screenshot force magnitude is 3000 however in shared file it is 2500.


Can you also share .out file of the run?


Define contact.JPG

Force 2500.JPG

JFormiga14 likes this

Share this post

Link to post
Share on other sites

Hi @Rahul R yes it is force vs displacement graph.

This is a pull out so i'm thinking that the upper part of puxator could leave the surface with a really big force so because of that i put the contact only in the low part of puxator.

So you think that i should take into account the layup thickness when making the contacts?

Share this post

Link to post
Share on other sites



the sliding contact is the key for correlation IMHO.

Sliding contact might not work using linear static analysis. In linear static analysis, the contact status does not change, does not slide and the contact stiffness is constant throughout. 


I tried with non-linear quasistatic (NLSTAT) and got slightly larger Y displacement (0.21 vs 0.19).


Share this post

Link to post
Share on other sites



the model is attached.


It is possible to perform laminate optimization using a non-linear quasi-static analysis. This model is not best suited for NLSTAT, because it takes a long time to solve a single run and optimization takes a number of iterations. CNTSTB is used for automatic contact convergence. Sliding contacts are computationally expensive- even more so if friction is considered. Using linear static analysis with freeze contact would be much more computationally efficient.


  • If the objective is to maximize stiffness subject to volume/mass/mass fraction constraint, using linear static analysis would give satisfactory results.
  • If the objective is to minimize mass subject to stress or displacement constraints, NLSTAT would be recommended to capture nonlinearities thereby predicting stress and displacement more accurately.



JFormiga14 likes this

Share this post

Link to post
Share on other sites

The DISPLACEMENT and GPFORCE have to be requested in ANALYSIS>CONTROL CARDS-GLOBAL_OUTPUT_REQUEST. Incremental result output is defined by NLOUT. If user wants to maintain the increment size, PARAM>EXPERTNL should be turned off.


Then you can plot force vs displacement using cross-plot

Use the following simplified model for practice:


Share this post

Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

  • Create New...