Stress analysis with moving parts

[flyforever85]

Hi all,
I have to check the stress distribution on a bellcrank. I attached the picture. The bellcranck can rotate around the pin (the + sign) and at a certain angle (that I know) it will stop. Shall I apply the load with the final angle on a pin and fix the second pin? The input and output load are the same but different distance from the pin

Any help is appreciated

https://files.engineering.com/getfi...-4449-8b15-aa31292a42bf&file=106C1812-003.tif

 

[FEA way]

If it's static analysis you should constrain the middle pin through kinematic coupling leaving only the rotation about its axis as free. Then fix one of these small pins and apply load to the other one.

 

[flyforever85]

what if the the input and output load are different? Shall I use the higher load and constraint the other pin?

Thank you!

 

[FEA way]

Yes, I think it’s a good idea. For static analysis you have to assume some static scheme of your part (even though it’s moving in real life). You can’t leave the rotation of the middle pin free and apply forces to both lateral pins because the rigid body rotation about the middle pin would make the analysis fail. You could fix the middle pin in all degrees of freedom and then apply forces to both lateral pins but I would choose the first option.

 

[flyforever85]

What is the best way to apply the load on RP-1? There is a bolt there and a rod pushes in z direction so although the bolt is fixed with the component, it's free to rotate.

I thought of creating a reference point and couple it with the top and bottom hole surfaces, see the pics. I then applied the load at the reference point. I'm not sure this is the best approach. Any opinion or different ideas?

https://files.engineering.com/getfile.aspx?folder=8ea2891d-beba-420c-a067-c4cb8469048d&file=part.tif

 

[FEA way]

You did this correctly. Reference point in the middle with coupling connected to the cylindrical surfaces. Since the bolt is free to rotate fix all degrees of freedom at this RP apart from rotation about its axis and the direction of applied force. Then apply load to this reference point. This should work .

 

[flyforever85]

Ok great, thanks! I was worried because with a generic load of 1000 lb and considering that component in AISI 4130 (yield strength around 97 ksi) yield was reached locally.

Yesterday I had the same problem when I used two different reference points for the top and bottom holes and applied load/2 on each node. The stress was more than 100 ksi (different geometry). but when I used a single reference point for both surfaces, stress was 40 ksi. Do you know why that happened? I'm reading the documentation but I can't find an answer.

 

[FEA way]

Coupling constraint works in such way that it transmits forces and moments and distributes them evenly on all selected surfaces. So if you use a single coupling with 1000 N load in reference point and apply it to 4 separate faces each one will get 250 N. Maybe there was some error in your analysis setup. If you ever have doubts regarding force transmission in your model then just measure reactions at supports. Their sum should be equal to the sum of applied forces in each direction. To sum reactions either integrate nodal output or, if BCs are applied through coupling, request it at a reference point.