What type of constraint should I use?

[yta10]

Hello,

There are two circular blocks with a bolt hole on the top and bottom. 

and there is a tube in between. They are held all together with a bolt.

What type of constraint should i use and where should i apply it to?

Thank you

[John_Holtz]

Hi @yta10 

1. What constraints have you tried?
2. What were the results? 
3. More importantly, how is this model restrained in the real world? (This is what you want to replicate in the analysis.)

The attached images may provide some ideas if you want the model to be "free" to expand and contract.

[yta10]

Thank you for your reply.

1. What constraints have you tried

I changed the models for the top and bottom circular ones to squares, and I used "fixed constraints" on the four sides at the bottom.

1. What were the results?

The result was the same as my calculation.

1. More importantly, how is this model restrained in the real world? (This is what you want to replicate in the analysis.)

The two flanges on the top and bottom are not constrained to anything else. they are compressed like a sandwich with the spacer in the middle.

but I thought I could use fixed constraints on the four surface at the bottom, because the stress mostly impact at the center where there is a bolt.

Do my answers make sense? 

1. 

[John_Holtz · Accepted solution]

Hi @yta10 

Your answers and approach make sense. 

• By holding one end, you are allowing the rest of the model to contract relative to the one end. 
• You recognized that the stress would be concentrated near the center, so you placed the constraints as far away as possible.

Here is how you can go one step further. Because there are minimal constraints in real life (it is either sitting on a table or held in your hands once the bolt is tightened -- neither provide much of a resistance), the top plate and bottom plate should bend exactly the same. The displacement and stress results should be the same magnitude but mirror image of each other. This probably works well near the center where the bolt is, but may not work as well near the edge where the constraints are. By fixing the faces, the bottom plate is acting like a fixed-fixed beam. The faces cannot rotate, so that may have an effect on the result. 

Instead of fixing the 4 faces, what happens if you only constrain the 4 edges (around the perimeter)? What happens if you only constrain the 4 corners? Both of these constraints allow the bottom plate to deform more, so the displacement and stress would be more like the result in the top plate. This same approach can be applied to the original circular plates. Of course, a circle does not have corners, but you can split the face into 4 quarters which provides vertices or points that you can restrain.

[yta10]

Hello

I appreciate your detailed explanation.

I actually have tried them, but I failed to run the simulation due to the reason as below.

Is there any settings I made mistakes?

Thank you

[yta10]

hello,

I managed to constrained like below.. but my hand calculation says the deflection is 0.27mm 

and i couldn't achieve mirror like image between top and bottom parts.. 

so I am trying to find what went wrong in the simulation.

Thank you

[yta10]

I used different computer to run the same simulation and I got the similar result as my hand calculation.

does simulation give different result sometimes?

I used Nastran 2020 and Nastran 2019.. Nastran 2020 had half of the number I had on Nastran 2019

.

[John_Holtz]

Why are you constraining the top AND bottom? The results do not look realistic.

You need to provide your hand calculations and the model. We cannot get the results that are required by looking at the images.

I assume that your hand calculations are for the contraction of the tube and end plates, meaning that one end moves 0.27 mm closer to the other. Your simulation is not setup to calculate that directly; it is giving displacements relative to the constraints. What is the displacement at each end of the bolt, for example? That difference should be close to your hand calculations. Does the hand calculation take into account that the plates are displacing a lot around the perimeter of the hole and less as you move away from the hole? I see a large amount of compression right at the hole in the simulation which may make comparing the simulation results to the hand calculations difficult. (Of course, this is why we do simulation. It shows the details that the hand calculations cannot include.)

[yta10]

Thank you for reply.

I think my hand calculation considered perimeter of the hole, it because the area that has stress is based on the cross sectional tube area that is close to the hole. the final simulation is very close to my hand calculation. I thought the max values of top and bottom is the displacements take place the most at the center, relative to the constraints (since the constraints will represent the initial position of the plates)  Therefore I added two max values to find out the total displacement. 0.136+0.1389 = 0.2749.(nastran 2019) but this value turned out to be different when i used nastran 2020. Nastran 2020 showed almost half of 0.2749.

Cross sectional area for tube

Ac = π * (OD2 – ID2) / 4 = π * (32.0042 – 38.12) / 4 = 335.643 mm2

Member Stiffness

K = E * Ac / L

L=Washer thickness * 2 + Flange thickness * 2 + Tube spacer height

L = 3.4*2 + 38.1*2 +38.725 = 121.725

E = 1.90*10^5

Ac= 335.643

K=523872.5 N/mm

Displacement = K/ Bolt Preload = 523872.5/144094 = 0.275057 mm

Do you think applying constraints on the eight edges better?

I attached the files. 

Thank you for your help!

[yta10]

Hello,

This time, I only constrained the four edges at the bottom. I thought I had to constrain both top and bottom. because I didn't see mirror-like result with constraints of 4 edges. for the displacements from the top of the bolt to the bottom, I couldn't see the bolt because I think I used bolt connection function which is connector. Is there a way to see the bolt displacement? 

Thank you

[John_Holtz]

Hi. You asked "Is there a way to see the bolt displacement? "

Yes, rotate the model so that you can see the beam element that represents the bolt. It is positions in the center of the hole.

[yta10]

Hello,

Yes I looked at the bolt displacement and it was similar to my calculation. I had thought it was the plate displacement value. thank you.