Check every bar in truss for buckling failure

  • 42 Views
  • Last Post 16 September 2018
Drbn posted this 15 September 2018

Hello!

I'm simulating a 3D truss in ANSYS Static Structural. Every bar has a circular tube cross-section and transmits only normal forces. My goal is to reduce the total mass of the truss by optimizing every bar's outer diameter using an ANSYS DOE.

I have a problem where most optimized bars would withstand the stress as a result of the normal force, but would fail due to buckling. I tried using the Eigenvalue Buckling module and using the Load Factor, but it didn't help me as some bars are still buckling.

Is there a way to reliably check every bar in my truss for buckling?

Order By: Standard | Newest | Votes
peteroznewman posted this 15 September 2018

 Hello Drbn,

What version of ANSYS are you using?  Have you tried using the DesignXplorer Direct Optimization component?

Can you Attach a Workbench Project Archive .wbpz file to your post so I can look at your model?

Regards,

Peter

Drbn posted this 15 September 2018

Hello!

I'm using ANSYS 19.1. I'm currently using the ANSYS Response Surface Optimization to optimize the diameters of my geometry. The problem is that I've found no way to include a buckling analysis. Since the diameters calculated by ANSYS withstand stresses, but will buckle under given loads, some sort of buckling analysis will have to be taken into account to generate useful results. And I've found no way to accomplish this yet.

The project is part of a running research program, so I'm afraid I sadly won't be able to make this file accessible, sorry.

peteroznewman posted this 15 September 2018

Hello,

Okay, no problem, I can make my own test case. Are you using beam elements, shell elements or solid elements for the tubes in your 3D Truss?   What is a typical beam diameter, wall thickness and length?

Regards,

Peter

peteroznewman posted this 16 September 2018

Hello Drbn,

My test case consists of three tubes modeled using beams that come together at a common point where a load is applied that puts two of the beams into compression and one of the beams into tension. At three support points, each beam has a zero displacement and the axial rotation is zeroed. A remote point on one beam is used to apply a force.

The remote point is scoped to one beam and two spherical joints connect that remote point to the other two beams.

In DesignModeler, three Parameters are created for the OD of each tube.

The wall thickness of all tubes is set to 0.5 mm by subtracting that value off the OD to define the ID.

The Workbench Project schematic includes a Buckling analysis and a Direct Optimization.

The Parameter Set shows two Outputs selected from the Static Structural and one from the Eigenvalue Buckling solution.

The input parameter upper and lower bounds are shown below.

Optimization was defined as shown below: minimize mass, keeping Load Multiplier > 1 and Stress < 250 MPa.

The Direct Stress Maximum was to keep the tension member from exceeding the yield strength.
I could have added a Direct Stress Minimum to keep the compression members from exceeding yield strength.

The buckling Load Multiplier applies to both beams. So if R1< R3 the first beam will buckle.

But if R1 > R3, the second beam will buckle.

The scoping for the buckling Load Multiplier is to All Bodies, so the constraint keeps the beam most likely to buckle from having a Load Mulitplier < 1.

The Direct Optimizer solved the model 48 times to come up with an optimum solution.

I hope you can apply this to your research.

Attached is the ANSYS 19.1 archive.

Regards,

Peter

Attached Files

Close