I am attempting to perform a linear contact analysis on a cantilever set up. I was able to run the analysis after entering PARAM, BAILOUT -1 in the dat file (the grids on top plate wanted constraint in R2 region which is the axis about which rotation due to bending should happen)
1 Setup, BC & Loading Conditions:
2. Contact Regions
3. Deformation: The magnitude is excessive. Way too excessive...definitely in the Non-linear Range.
4. Contact Pressure contour on Bottom Plate:
I am not experienced enough to determine if the above looks realistic. I would appreciate any suggestions to improve the model set up so that output looks more realistic.
More info. This is a test setup currently to get myself familiarized with contact process & results interpretation.
Thx in advnace...
Solved! Go to Solution.
The reason why the results aren't realistic is that the modelled condition is not physically feasible. A static analysis requires a single unique equilibrium solution. Equilibrium is only possible for this case if you use glue, in which case the force (and moment) can be transferred at the "contact" interface.
As a "contact" problem it is impossible for the moment inferred by your cantilever force to be transferred across the contact interface. A (manual) free-body diagram shows that both compressive and tensile contact forces are required at the contact interface to balance the cantilever load, but by its very definition, tensile forces cannot be transferred across a contact. It is impossible, thus, to reach an equilibrium solution to this problem, hence the need to use BAILOUT, which should NEVER be used to judge results - it can only be used for diagnosing modelling errors. For a static analysis to run, sum of forces and sum of moments must be zero for the structure as a whole, and for every sub-structure (ie. each part); and for every individual element and node in the model.
If it could run an analysis, the plate at the end would simply flip off the restrained plate and fly off indefinitely from the unbalanced loads.
Edit... the essential requirement for equilibrium for the model and all the elements is that the calculated reactions (and forces through the structure) form part of the equilibrium which must be established. It should also be noted that equilibrium must be mathematical as well as practical. Even though your applied forces are vertical (therefore no horizontal reaction), a horizontal constraint is compulsory (a) to provide a single unique solution; and (b) to provide a reference zero from which horizontal deflections are calculated.
So, eg. if your fixed constraint had only been TZ and RY (to support the cantilever moment), this would be insufficient (even if your contact were glued), even though the net reactions in the four other global Degrees of Freedom are zero.
Aha...thanks for that explanation EndZ. Makes sense now why Femap was showing singularity in R2. No way the end internal moments could be generated to balance out the moment generated due to external vertical load. As you have rightly mentioned, end moments are generated due to a couple (tensile & compressive).
Contact condition cannot transmit tensile forces.
Would more info about contact be available in the NX Nastran User's Guide?
Appreciate your insight. Was very valuable.
Like you suggested, I tried enforcing a Glude contact condition between the top & bottom plate in a cantilever condition.
Still getting a Rigid Body error (all 6 motions) for the grid on the top plate.
Any suggestions on how to proceed further?
I was also experimenting with plate contact. I got some excellent tips from the Femap community. Also you can find the model the that ChipFricke built as an example.
Make sure you press the "defaults" button on the glue property. Then, also make sure the glue search distance on the glue property is slightly larger than the midplane gap between the two mid planes of the elements, otherwise it won't find the interface as a glue zone.
And for good measure, check your material has a Youngs Modulus. And Possions Ratio (OR sensible shear modulus, but don't bother having both Poissons and Shear)
And plate contact/glue has "sides", ie "top" and "bottom". You can see the top and bottom side of an element via F6 -> Labels, Entity and Colour category -> Element Directions -> Normal Vectors, tick "Show Direction". This will draw an arrow on the top (positive) side of the plate elements. Make sure your region is properly defined so that the correct sides (positive or negative) are interacting with each other. If you don't get the proper sides, then the contact or glue interaction will also fail to be created. "Sides" are critical for plate contact problems because it is necessary to correctly calculate whether (intended) interference or clearance is or is not occurring.