Simulation related help required

[mufadal89]

Hello guys ,

I am building a couple of designs for which I need to do some simulations - Static stress analysis.

I am really stuck at the part where I have to decide the boundary conditions, 

for eg. For Bolt fastening - should the hole feature be clamped in all 6 dof or some 3 

How do I consider the preload of bolt into the simulations

Whether the whole mounting face needs to be constrained. etc etc.

I have seen alot of posts in which seasoned simulation experts have guided others in such problems.

If you can guide me to any source from which I can learn more about simulations , i would be very grateful.

Like any common guidelines or case studies would be great.

My back ground is mostly design so I have not much worked on simulations although I can learn very quickly.

Thanks Mufaddal

[John_Holtz]

Hi Mufaddal,

Just to be clear, the bolts that you are asking about are connecting your model to the "ground" or some other rigid item that is not modeled. These are not bolts that connect one component of the model to another component of the model. Correct?

There are various ways to model the connection of the model to the ground. Which one you choose depends on how accurately you need the connection to be modeled and how complex you want to make the model. (The more complex, the more likelihood something will not work ) So the basic methods of bolting the model to the ground in a Fusion simulation are as follows:

1. Constraint the bottom of the model. The purpose of the bolts is to keep the "base plate" in contact with the ground, so this type of constraint is the one used most often. Assuming the friction prevents sliding, you would constrain all three directions. (Note that Fusion does not have rotation constraints because there are no element types yet that calculate rotation.)
2. Constrain the bolt holes; contact with ground. In a more accurate analysis, you would need to model the ground as a part, and define separation contact (or rough contact to prevent sliding) between the model and the ground. The contact will allow the model to lift off of the ground in places where it does not maintain contact. Constrain the perimeter of the bolt holes where the bolt head makes contact. The ground can be fully constrained on all sides.
3. Model the bolts; contact with ground. The most accurate approach is to model the ground, including the holes to match the bolt holes in the model. Define separation contact (or rough contact) between the model and the ground. Use simulated bolts ("Constraints > Bolt Connector") to model the bolt. The simulated bolts are beam elements, so they have the stiffness of the bolt and also have a preload. The ground can be fully constrained on all sides.

Let us know if you have any other questions.

[mufadal89]

Hello @John_Holtz

thanks for the reply. 

I have attached the model of the simulation .

Actually I found out that there is an utility for giving a bolted connection.

I did the same and I gave a specified torque value at the joints (4 ) but I am getting max stress at the joint that too very high.

This project is just for trial to get a feel of simulation so its not related to any real life application.

But I guess the stress value should be much lower at the joint as I had given only 1 Nm torque 

Like you said I fixed the block to the ground and gave bolted connections of bracket to the block 

Please advise

Mufaddal

[John_Holtz · Accepted solution]

Hi Mufaddal,

There are a number of reasons for the high stress (1495 MPa = 217 ksi).

• The bolt preload creates a stress of 796 MPa (=115 ksi), so it is a fairly high bolt load.
• The simulated bolts use beam elements to connect the shank of the bolt to the perimeter of the hole. (Think of spokes on a wheel connecting the shaft to the perimeter of the wheel.) So this tends to create a point-load and stress concentration around the perimeter of the hole. Such stress concentrations are normally ignored because the simplifications are not expected to calculate accurate stress in that area.

In other words, the simulated bolt is much simpler than the image that is shown. I tried a much finer mesh around the perimeter of the hole, but the stress went up. (smaller load per node, but smaller element too. So stress concentration remains about the same.) Notice how the stress drops off rapidly over the span of 1 element. This is an indication of the stress concentration (or a mesh that is too coarse).

Note that you probably want to use separation contact between the bracket and base block. I noticed that you had bonded contact, so the bolts are not doing much in the analysis.

And this brings to mind option 4 for modeling a bolt. (Continuing with the three suggestions I gave previously.)

4. Model the bolts as solid; contact with ground. The most accurate approach is to model the ground, including the holes to match the bolt holes in the model. Define separation contact (or rough contact) between the model and the ground. Model the bolts as solids (but without the complication of the threads and rounds on the bolt head/nut -- that is just crazy). Perform a thermal stress analysis to shrink the bolts the amount necessary to create the preload. (Edit) When defining the contact between the bolt head and the model, use the "Penetration Surface Offset" to stretch the bolt the distance necessary to create the desired preload. (Note that this may require trial and error to get the preload accurate since stretching the bolt will also compress the model and reduce the theoretical preload.) Use a fine mesh around the bolt head to capture the Hertz contact stress that occurs. The ground can be fully constrained on all sides.

[John_Holtz]

Hi @mufadal89

I wanted to check with you to see if you completed this analysis, and if so, what you ended up doing. Or do you have any other questions.

[mufadal89]

Hello @John_Holtz ,

Greetings

Sorry for the delayed response .

I was figuring out , the basic stuff . as I m totally new to simulation 

I have modelled the parts as per your guidelines.

1. Removed the bolt connections

2. Modelled the block and bracket with seperation contact like you said

3. Modelled seperate bolt elements with rough contact  and surface seperation - 0.25 mm

Here are the results.

I Suppose these are accurate results . predicting max stress on the rib.

and some of the stress appears to have been transferred on the block as well .

I have attached the file . Please have a look sir. 

have learned alot from your inputs.

Looking forward to learn more in more future projects.

Thanks & regards,

Mufaddal