Buckling Simulation Study providing weird (and incorrect) Results.

[mallerya]

I'm trying to learn how some of the Simulation stuff in Fusion 360 work. I watched a few tutorials, followed the steps, but my study is showing buckling deformations that should not be naturally occurring-- especially for the forces applied.

Here you can see I have a plank-shaped object. This is to become one of the carriage platforms for the heated bed on my 3D printer. Bearing-blocks will be installed on the underside of the plank which move it along the Y-Axis. I am trying to simulate the load on the far end of the plank to see if it is rigid enough to support the weight of the new bed.

Currently, I get this as a result. This is with only 1 lb of force applied. See how it is bending sideways? That is not expected. I would expect normal buckling to go down the Z axis only in a real world scenario.

First, I made sure to select the proper material which I will be printing (PETG -- or just 'PET' in fusion). I extruded out a small rectangular block underneath where the bearings will attach, then applied a normal fixed constraint to it.

Then I extruded a small tap inside the holes for the far end of the plank which is where one of the corners of the bed will rest. I did this so I could select face and apply a downward force along the Z-axis, while trying to rule out the possibility of the inner most faces of the hole causing miscalculations during the simulation. I tried doing it without the extrusion on the inside and applying the force to the inner faces of the hole instead, but that seemed to make no impact to the fixing the end results I am getting.

I also tried increasing the mesh resolution, and filleting the edges of the rectangular block (heard this can cause issues sometimes during simulations). That seemed to make no difference as well.

I would expect to see while using this thick of PETG material (6mm) in combination with a C-shaped support rail, is little-to-no buckling when using 1 LBS of force. I planned to scale this force upward for fun to test the simulation aspects of Fusion, but I could not even get this small force study to simulate correctly.

What am I missing?
(Included Fusion file for reference)

Thanks 🙂

[MikeSmell_ADSK]

Hi @mallerya - 

Please take a closer look at the results legend. You will see a drop-down that will allow you to look at the 3 buckling mode shapes that are calculated by default. In this drop-down, you will see that a multiplier X load amount is provided. In your model, the multiplier is 4947, which means buckling should not occur until the total applied load is larger than the total applied load multiplied by 4947. For more details on the buckling load factor, check out our help. https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-294956C9-1D54-49A9-8636-618816C85A93

Thanks, 

Mike Smell

Sr. Product Manager, Fusion 360 Generative Design

[mallerya]

Mike, thank you for your reply.

I am somewhat confused as to how these multipliers work. You mentioned that buckling should only happen when the force is multiplied as high as 4947 lbs. Is this when the very first symptoms of buckling would occur or is this when it would be at it's breaking/snapping point?

I am not too sure how these numbers could be correct.. 6mm thick PET plastic could not possibly resist 4000lbs, right? I 3D printed an earlier prototype of this model (with 3mm thickness) and added a load of 1 lbs on both ends of the plank. With 20% infill, it definitely had some minor flexing on it. I also printed one with 100% infill which was much more rigid which did not show any signs of flexing/buckling.

I want to determine at what weight would signs of flexing occure in the object, then make adjustments to the model as appropriate (thickness, supports, etc). I am assuming that Fusion 360's engine assumes that the body of the object is injected-molded with 100% infill. Is did not see a way to change the density/distribution of the material.

I am still learning CAD so I apologize for my ignorance in advance. I've attempted some research but had little success in finding answers to such questions.

[John_Holtz]

Hi @mallerya 

I can provide some help with your questions.

"Is this when the very first symptoms of buckling would occur?" Yes. Buckling is when something becomes unstable. Breaking/snapping is not buckling; it is the after effect of the buckling in the real world. The simulation does not calculate what happens after it buckles.

"6mm thick PET plastic could not possibly resist 4000lbs, right?" You are not analyzing PET plastic. You are analyzing a material with the same modulus of elasticity as PET plastic but with infinite yield stress. A linear analysis type (such as the buckling analysis that you are performing) ignores any changes in materials properties due to the loading. That is, the material does not yield, the stiffness does not change, the directions of the loads do not change, and so on. The displacements are assumed to be small.

I did not open the model, but just based on the description (6 mm thick) and the visual, this part is very thick (1/4 inch) compared to the length that is unconstrained (a few inches). Buckling is a phenomenon that occurs in long, thin parts. I would not expect your part to buckle before it yields or breaks, so a buckling analysis is not the correct type of analysis. I would suggest a static stress analysis to see how it is bending. If twisting is a concern, then apply 60% of the load to one size and only 40% to the other side. Based on the results, you can change the design and compare the differences.

"I am assuming that Fusion 360's engine assumes that the body of the object is injected-molded with 100% infill. I did not see a way to change the density/distribution of the material."  You need to find the material properties for your actual material (the modulus of elasticity and Poisson's ratio are the only properties that matter) and enter them.

Your mesh is also very coarse compared to the thickness. You should have at least 2 elements through the thickness in order to accurately capture the bending/twisting that occurs. Try a mesh size of 3 mm to see if that gives 2 elements.

Let us know if you have any other questions.