I have designed underwater ROV which has a few sealed containers to accomodate payload etc.
These containers are rather simple and have to withstand pressure of 540 kPa (50 meters deep with 10% safety margin).
With simulation I would like to determine if they can handle this depth and what is the maximum pressure they handle before failing (probably due to buckling).
I have never used Femap before and I would really appreciate if somebody could explain how this kind of analysis should be done in Femap environment.
Is there some guides available for Femap newbies that would cover this kind of simulation or teach how to use Femap overall?
I tried to follow this tutorial, but got to a point where I don`t know where to add constraints https://www.youtube.com/watch?v=7FKZEiA-rMc
Should separate parts be used in simulations instead of assemblies?
In terms of simplicity I guess I could just leave dome, bolts and cable penetrators out because there is not much extra stress on them and they can withstand that much of water pressure anyway (all 300m pressure rated).
If I would analyze only main bodies of enclosures then I could add constraints to open faces just like in that tutorial.
Or should I cut assemblies to half and then add constraints like in this tutorial?
I did search internet and forums for similar cases without much luck.
I have attached pictures of my enclosure assemblies.
Thanks for any help!
If you are new (I hope to FEMAP, not to engineering using FEA) then you can start studying part by part: take the main body, apply external pressure and perform both linear static & buckling analysis to compute the buckling load and the maximum stress that can support the part. If you have symmetry of loads & geometry, use it in Linear Static Analysis, not Buckling, this will stabilice the part and reduce the total computing time.
You can study the assemblies as well, then you will have to define surface-to-surface contact "no penetration" between parts, or GLUE SURFACE-TO-SURFACE, if both contacting parts are going to state together for sure.
I suggest to start with one of your examples and you will learn how to solve problems.
Also take a look to FEMAP VIDEO LIBRARY here:
Thank You for such a quick reply!
I`m going to experiment as much as I can. For me the most confusing part is adding constraints.
For example where and what kind of constraints should I add to my cylindrical tube or rectangular enclosure assemblies (they are not 100% symmetric because of bolts, penetrators etc)?
These parts will not be mounted using bolt, screws - they will just sit inside main hull.
Do I understand correctly that with 100% symmetric part defining constraints is not required in Femap if pressure/force acting on body is the same all around (like hydrostatic pressure is) ?
Only with inertia relief option, without this option you must constrain model or you get error 9137. You can run modal solution - SOL103 before linear static and check eigenvalues with near zero values - like 1e-3 - 1e-6 - there are rigid body modes, unconstrained model have six rigid body modes coresponding to six DOF`s and properly constrained model dont have any rigid body modes.
You need to define always a set of constraint, of course!, if not the solver will give you error, you need to define the minimum constraints to stabilize your model, this is the reason why when both symmetry on loads & geometry exist you can study 1/4 of model, prescribing the corresponding symmetry boundary conditions. Here I have created for you the case of cylinder to mesh with 2D SHELL CQUAD4 elements and an external pressure load applied: because symmetry in loads & geometry exist you can study 1/4 model only, the model this way has a reduced size and at the same time is stabilized
Thanks for this explanation!
I have no trouble understanding how symmetric body with equal pressure distribution can be stable.
However I still can not understand how to constrain nonsymmetric body (like my watertight enclosure) that goes underwater. For my purposes pressure is constant because bodys are small and I only need to verify that this body can handle one critical depth.
For example this electronics enclosure (photo attached). In Femap how would You approach simulating 540 kPa fluid pressure acting on this body underwater?
Should I just make some small connections underneath this container and add constraints just as if it was bolted onto something?
I did manage to do some simulations with sylindrical tube assembly. I used inertia relief option as Karachun suggested. Athough in some other topics some said that this will not provide accurate result. Instead of fluid pressure I used pressure as load. I dont have any idea if this makes any difference.
Now because of this constraint thing I´m not sure if result are reliable or not (photos attached). They look reasonable to me and infact I`m getting similar results in Solid Edge simulation when using just main housing of this enclosure with constraints added to the open face. But hey as I understand validating/understanding FEA results is the most difficult part of simulation.
I apologize if my questions sound silly. I have background in electronics with very little experience in mechanics.
If all of your load is pressure on all internal surfaces - ther resultant force will be near zero due to roundoff error. Try to add to model a couple of "weak springs" with low stiffness compared to stiffness of model and constrain one node of this spring. If you attach spring to solid remember that solids have only translational dofs, so you must attach springs at least to 3 different nodes that dont lie on line. These springs add some changes in model stiffness and results but you can experimentaly find stiffness that produce small changes in results but suficient to prevent crash of analisys.
Share your specific geometry problem here and we can talk with the example, post your FEMAP model here, each problem is a world and it can involve different stratregies depending what the user really needs, the solution type, etc..
I still can not understand how to constrain nonsymmetric body (like my watertight enclosure) that goes underwater.
In this case you will agree with me that the quality of mesh is really bad, if I use command TOOLS > CHECK > ELEMENT QUALITY you have 3D solid CTETRA elements with TET COLLAPSE (ie, aspect ratio) = 43 times bigger one side than other. Also you have in some areas only one element in the wall thickness, this is wrong, with 3D solid models you need to mesh minimum with 3 elements in the wall thickness to capture accurately the stress gradients in the wall, OK?.
Element Quality Quality Check Number Failed Worst Value Aspect Ratio 122 14.3742 Taper 0 0. Alternate Taper 0 0. Internal Angles 11106 104.561 Skew 5083 3.989238 Warping 0 0. Nastran Warping 0 0. Tet Collapse 312 43.09303 Jacobian 522 0.915142 11106 Elements Failed out of 16243 Checked.
In this problem you can study 1/4 model because symmetry of loads & geometry.
Here I will show you the workflow of how to mesh with HEX elements.
• First prepare the geometry, my trick is to project all curves to a plane and split the surface with command GEOMETRY > Curve - From Surface > Project".
• Next using splitting commands like "point-to-edge", "point-to-point", etc.. define regular surfaces where 2-D mapped quad mesh is easily achieved, the target is to have surfaces of 4-sides. When more than 4 edges then use MESH > MESH CONTROL > APPROACH ON SURFACE > MAPPED - FOUR CORNER in faces with more than 4 edges.
• Apply mesh size on surfaces and mesh properly using 2-D PLOT PLANAR quad mesh (not need to apply any property to either the geometry or 2-D mesh, simply is a 2-D mesh to use later to generate 3D HEX by extrusion).
• Next using command MESH > SWEEP > ELEMENTS select ALL the above 2-D quad plot-planar elements and sweep them along the curves to form the new 3-D HEX8 elements. Assign a new property to all the created elements, for instance COVER, and make sure to activate the option to delete the 2-D mesh, we don't need it anymore.
• Next the trick is to associate all the generated 3-D HEX elements to the solid body using command MODIFY > ASSOCIATIVITY > AUTOMATIC. Make sure to activate the last option "Detailed Associativity Summary ..", and you will see the following:
Automatic Associativity 16690 Element(s) Selected... 16690 Element(s) Selected... 16690 Element(s) Selected... 1 Solid(s) Selected... Attaching to Solid 2... 50 Nodes associated with Point(s). 801 Nodes associated with Curve(s). 4049 Nodes associated with Surface(s). 11874 Nodes associated with Solid(s). No geometry associated with 0 Nodes. 14230 Elements associated with Geometry. No Geometry associated with 0 Elements. UnAssociated Nodes and Elements No geometry associated with 2498 Nodes. No Geometry associated with 2460 Elements. Automatic Associativity
To get rid of unassociated nodes & elements (we need to delete) in the DRAW/ERASE toolbar activate the mode ERASE, then select the previously solid body and both geometry & mesh will be erased from screen.
Simply delete the above mesh using DELETE > MODEL > MESH selecting mesh by a window and you are done!!. The mesh quality is good, we have an ASPECT RATIO = 3.5, this is a reasonable good value for a 3-D solid model (the target should be always 1.0!!) and max Jacobian = 0.4, well below the 0.6 max.
Check Element Quality 14230 Element(s) Selected... No Elements Outside of Maximum Allowable Value. Quality Check Number Failed Worst Value Hex AR 0 3.48241 Hex DetJ 0 0.0117615 Hex Warp 0 1. 0 Elements Failed out of 14230 Checked.
For the main body the procedure of meshing preparation will be the following:
This is the resulting 2-D PLOT PLANAR quad mesh, the next step is simply sweep 2D mesh to form the 3-D solid HEX8 elements following the previous procedure explained before, don't forget to associate mesh to solid bodies, OK?.
To avoid the creation of WEDGE elements around the Y-axis in the center of the body after sweeping 2-D mesh around Y axis I will mesh instead the bottom of the body with 2-D QUAD PLOT PLANAR mesh an perform extrusion in the Y axis. Because the combination of meshes in two different directions the command TOOLS > CHECK > COINCIDENT NODES should be performed to merge nodes to have mesh continuity in the base.
Finally this is the complete 3-D Solid mesh with pressure loads applied and GLUE surface-to-Surface performed, as well as symmetry constraints.
Because the maximum nodal vonMises stress is located in the bottom of the body then better change the constraint in the Y-axis to the top of the body, in any point or edge of the cover. The final results of resultant displacements & vonMises nodal stresses are practically similar no matter the point or edge you choose to constraint the Y-axis displacement, top or bottom. The deformed shape will change, then the best recomendation is to select a point in the region the stiffness is bigger.
Inspecting results we can see that locally a penetration exist of the cover in the main body wall: you need to define surface-to-surface contact there to avoid penetration and improve results, OK?.