Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

Ansys Workbenck beam structure FEA

N

Natasha

New member
Hello,


I am analyzing a small airplane engine mount with beam elements, and I am having trouble transfering torque from the propeller and engine to the structure. What I would like to do is to transfer it thru rigid beams, but I can't figure out how to do it in workbench, further more it will not let me add remote forces if I don't have surfaces.


Anyone has ideas?


thx,


Nat
 
Hi,


so here is my geometry and a more detailed explanation,


1- if i use solid elements the model takes over 2h to run versus the 10 sec with beam modeling. Almost since my structure is made up of beam (in real life) it is the best choice to represent reality.


2 - for the moment I created beam with very high rigidity to simulate rigid links. I know this is something that should never be done but I can't find a way to insert rigid links or MPC.


3- forces acting on the engine mount is engine torque, propeller inertia, propeller gyroscopic moment, propeller weight, engine weight, aewrodynamic airplace forces all transfered to the engine center of gravity. As a side note point masses need to attach to a surface (line and points are not recognized) the same goes for remote forces.





View attachment 4881


originally this model was done under nastran, and I have tried to run it thru Ansys ''classic'' where I don't have the above issues. However when I do that Ansys does not let me recuperate my stresses (displacements work fine) and pops an invalid table message.


thx,


Natasha
 
Natasha,


Are you just planning on conducting static analysis, or dynamic as well?


I was going to recommend you do this in Ansys classic because it allows you to select nodes directly, and utilize RBE3/CERIG commands without having to directly select geometry. I've used mass21 elements with both of these commands in classic, and have correlated it to test results to my satisfaction (shock/vibe). Perhapsit's worth it totroubleshoot your ansys classic analysis.


Back in workbench however....


I agree, 1 & 2 are acceptable approachs.If you're just doing a static analysis on the engine mounts, you should be able to just apply your forces (sum them all into 1 vector) to the intersection point of those rigid beams you've created (which I presume is the engine CG?). If you do this, the mass of the engine does not come into play, just the stiffness - which you've simulated as perfectly rigid.


I propose you don't need a point mass for the engine, because you can add the force due to gravity into your single force vector. Make sense?


If you're doing shock/vibe (and thus need to account for the engine's mass), then I'd focus on getting stresses out of your Ansys classic analysis... but that's just my own comfort zone.


Jim
http://www.linkedin.com/in/shawengineering
 
Hi,


I'm doing only static analysis, I do need either mass or equivalent force because of accelerations.


beam modeling falls under line bodies so rigid behavior (solid bodies)cannot be selected in workbench


When I did my model undel Ansys classic, I am unable to recuperate the stresses in my elements (Beam 188 does not have stresses in nodes). I get the following warning: S is an invalid label. The ETAB command is ignored.


thx,


Natasha
 
Natasha,


In Workbench:


1. Remember: Mass * Accel = Force applied at CG. Use this to replace the mass of the engine with a force at it's CG for each load case (accel vector).


2. Replace your line bodies with actual solid bodies, for example model cylindrical pipes in your CAD model. If it makes you feel better, give them very low density, although this is not needed for a static analysis. Now they can be made rigid.


In Classic:


3. Yes, Beam188 does have stress. It says so in the help... (See here). ETAB is for the "etable" command, which is only needed for certain types of post processing. Are you using somebody else's APDL code or something? You should be able to just create a stress plot, or list the stresses for each node. (make sure you have all nodes selected first). In APDL this would be PLNSOL (PLot Nodal SOLution) or PRNSOL (PRint Nodal SOLution), respectively.


Jim
http://www.linkedin.com/in/shawengineering
 
Design engine has put together a six day Ansys class. three days one month and three days the next month. http://proetools.com/courses/fea/ansys-level-1

I just had surgery on my hand and the surgeon uses Pro/E and Ansys to solve stresses inside hips before he goes in to replace joint parts. I was hoping to create a model similar to that as example.

Any suggestions for solving assemblies please email me [email protected]


Edited by: design-engine
 
You must log in or register to reply here.

Sponsor

Articles From 3DCAD World

Back
Top