Bolt Pretension in Ansys Workbench

[flyingmike]

Morning all,

I am working on a static analysis in Ansys and have included the models of the screws so I can add pretension.

At first I added the pretension to an outer face on the screw shank. (the screw has multiple split faces on as the screw bolts 3 plates together)
Running the analysis gave me the most deflection in the bolts themselvesdue to the pretension and on investigation I could see that a hollow cylinder was stretching out from the screw. I have attached a pic to make it more clear.

I have since tried adding the pretension to the body and setting up a coord system for each bolt. The result of this was that the hollow cyclinder now stretches out of the top of the screw rather than the bottom.

Has anyone seen this before? What does it mean?

Thankyou in advance for your help

Mike

 

[ansysfreak]

Regards

I thick this is because of the auto scaling of the results.
Set is to true scaling.

Regards

 

[flyingmike]

I think your right, but shouldnt the entire model deform in a proportional manner even if it is scaled up? why this thin walled cyclinder appears looks a bit odd and the part would never deform in this way under load even in a much reduced scale....maybe?

 

[ansysfreak]

Take a look at the contact between de bolts and the parts. I believe the contact is not in initial contact.

Regards

 

[flyingmike]

There are three parts in the assembly plus the bolt. I put split faces on the bolt shank to add the contacts too. This was done as I was having initial problems of parts penetrating through each other.

The bottom block (which in real life the bolt screws into) has a hole in it the same diameter as the bolt. The inside wall of the cylinder has a bonded contract to the outer face of the bolt (via a split face the same depth as the threaded hole)

The second block is an intermediate with a clearance hole so it is not in initial contact with the bolt. I added a no separation contact to this as the bolt was penetrating through this part during unitial simulations.

The third part is what the bolt clamps down on. There is a no separation contact between the bolt shank and the inner face of the bolt hole and a bonded contact between the underside of the screw head and the base of the counter bore.

Hope this makes sense, thanks for you help

 

[ansysfreak]

Dear

Did you use any other loads?
Thers is a restiction on the bolt pretension:
1 loadstep pretension the bolt (don't use any other loads in this loadstep)
2 loadstep lock the bolt pretension and apply all other loads
Hope this help.
regards

 

[flyingmike]

There are two other loads on the top plate.

I run the simulation with all the loads and the bolt pretentions applied.

What do you mean by loadstep? I'm quite new to ansys having only used Cosmos before.

 

[ansysfreak]

Dear
Under the analyse setting you need to define 2 loadstep.
Then look at the details of the bolt-pretension, a table will be availeble, load the pretension in the first loadstep a lock him in the second one, then go the the forces and set the force in the first loastep to 0.
Regards

 

[flyingmike]

I have added a second step. how do I lock the pretention in the second step? it has currently defaulted to 0 for the second step.

 

[ansysfreak]

Click on the cel in the table on the right and choose lock

 

[flyingmike]

I dont seem to have lock, screen shot added of the options I have.

 

[ansysfreak]

NO offcourse not, you are looking at the force table!! Here you should set the force in the first loadstep to 0 and aplly the load in the second loadstep.

 

[flyingmike]

gotcha, I went to the bolt pretention and for step 2 selected lock in the left hand table in the 'define by' options.

I'll do them all now and re run the simulation.

Thanks for your help!