bolt simplified simulation

  • 53 Views
  • Last Post 6 days ago
jonsys posted this 2 weeks ago

Hello Community,

I want to simulate a situation in which a connection is done with a bolt. The tighter the bolt hex head, the higher is the force applied to the body by the bolt. 

How can this model be simplified for an analysis?

1

Regards,

Order By: Standard | Newest | Votes
peteroznewman posted this 2 weeks ago

Hello Jon,

Make two plates with a hole in each. Make a simplified version of the fastener: a cylindrical shaft with a cylindrical head on one end and a cylindrical nut on the the other end is good. This can be a single solid. You would have three components in SpaceClaim (or three parts in DesignModeler). The head and nut of the fastener have to be touching the plate surface.

Use a fixed support on the bottom plate sides and apply a force to the upper plate sides. You need three frictional contacts. Create frictional contact between the nut face and the bottom plate, frictional contact between the plates, and frictional contact between the head face and the upper plate. Add Bolt Pretension to the cylindrical face of the shaft.

A 2 step solution is usually used where the Force is zero in step 1, while the Bolt Pretension is applied.  Then in step 2, the Bolt Pretension is set to Locked, and the Force is applied to the plate.

I have done this type of model many times. You can simplify it slightly by using Bonded Contact of the nut and head to the plates, but I don't usually do that.

Let me know if you have any questions.

Regards,

Peter

 

  • Liked by
  • SandeepMedikonda
  • jonsys
jonsys posted this 2 weeks ago

Hello Peter,

thank you for your reply.

Does the pretensioning of the bolt, represent how tight is the bolt head tightened? How can I add a pretension?

I was more thinking of a 2D model. How would it be in this case?

Regards,

peteroznewman posted this 2 weeks ago

Hello Jon,

Yes, bolt pretension is the tension force in the shaft after the threaded fastener has been torqued tight. Bolt Pretension is a load in the list, but it may only apply to 3D models, I don't know about 2D.

Regards,

Peter

akhemka posted this 2 weeks ago

Hi,

Pre Tension works by splitting the mesh into two parts; an upper and lower section of the bolt. It then applies a downward force to the upper section followed by an upward force on the lower section. This allow the remainder of the model to equilibrate, deform due to the bolt load, and let the force in the bolt shank to relax because of the deformation of the remainder of the model. 

 

For Plane Stress, Plane Strain, and Axisymmetric just apply the pressure. In these, Ansys knows the area, and computes the correct force value.

 

Regards,

Ashish Khemka

 

  • Liked by
  • jonsys
jonsys posted this 6 days ago

Hello Peter,

I tried to simulate it, but my model does not seem to work. It also takes a lot of time for one iteration. In case you have some time to look at the model and give me ssome feed back, i would be thankful. attached is the proj

Regards,
Jon

jonsys posted this 6 days ago

thank you Ashish,

your explanation on how the bolt pre-tension works was really clear.

For Plane stress and so on, do you mean do only apply a pressure where the bolt head is supposed to be?

Regards,

peteroznewman posted this 6 days ago

Hello Jon,

I had a look at your model.  You had good mesh controls that you suppressed. I unsuppressed them.  I changed the Mesh Details to have Proximity put 2 elements across any part of the model.

You need a two-step solution to use Bolt Pretension. Step 1, Load to a pretension value. Step 2, Lock.  In step 1, the force you want to apply to your bolted assembly needs to be set to zero, in step 2, it becomes non-zero (20 N).

You have to be careful with the automatically generated contacts that are created on each Attach.  Those are nasty.  I had to suppress those in your model.

Step 1 needs a large number of Initial Substeps to let the contact be established, like 100.

The solver does seem to be making progress.

A look at the N-R Force Residual Plot shows the problem is on the bolt. You have an interference. This should have been a clearance hole.  I will suppress the contact between the bolt shaft and the hole, since the friction will hold the parts from moving with the low shear force you applied.

The contacts that are not to the bolt head will have the Normal Stiffness reduced, because they have such a large area and a low pressure.

I also turned Small Sliding on which is an ANSYS 19 feature that speeds up contact computation.

With the above changes, the model has started to converge and I expect it will run to completion.

Regards,

Peter

  • Liked by
  • mekafime
  • jonsys
jonsys posted this 6 days ago

Hello Peter,

firstly thank you very much for the time and effort you put on this forum,

I initially had 2 step solution, with the 1st step applying only pretension and 2nd step keeping the pretension locked & applying the load as well (as you suggested on a previous comment). But since analysis was not converging I thought to first make it run, then add the pretension.

The automatic contact was created when I saved the file as back-up before archiving it, so in the file that I run there was no automatic contact.

 

From your suggestion I am running the model again with the following:

I reduced Normal Stiffness for the contacts that are not to the bolt head.

I íncreased shear force magnitute (I chose the shear force low only in beginning to see if the model runs) but it still does not converge (I kept the contact between bolt shaft and hole). What do you mean there was an interference? Probably that might be the problem that my analysis is still not converging.
By the way, how did you see that there was a problem at the bolt by N-R plot, did you change Newton-Raphson Residuals number or what?

Regards,

peteroznewman posted this 6 days ago

Hello Jon,

Auto Detect Contact On Attach is a pernicious behavior that is best turned off,
which can be done from the Workbench Tools, Options menu under Mechanical.

I let the solver run with the 8000 N Pretension load, but it only got 22% of the way until an Element distortion error stopped the solver after 112 iterations, taking 69 minutes on 8 cores using 18 GB of RAM.

If you entered a pretension < 1700 N, then it would have converged at that load without getting this error. I just made up 8000 N, maybe that is way too much. I didn't put much thought into that number.  If you do need a pretension > 1700 N, then you will have to make smaller elements on the el around the hole where the N-R plots are showing a Maximum.

The shear force should be 0 in step 1 while the Pretension load is being applied.

There were two clues that the bolt shaft in the hole was original problem. Most of the N-R plots showed the maximum on the bolt, but also, all the contacts were shown as closed and if the bolt shaft had clearance to the hole, it should have shown as Near not Closed in the Contact Tool Initial Information.

Regards,
Peter

 

jonsys posted this 6 days ago

Hello Peter,

thank you for the reply.

yes, I keep the shear force 0 on the 1st step.

The model is still running, but I have the following questions out of curiosity:

  • Is the running time normal? What might be the reason that it takes so much computational time?
  • How do the N-R plot show the maximum on the bolt? how can you see this, I don't understand

Regards,

peteroznewman posted this 6 days ago

Hello Jon,

The running time depends on your computer's Clock Speed, RAM and # of Cores. I have a 3.4 GHz clock, plenty of RAM and 8 cores, so it solves much faster than on a computer with a 1.7 GHz clock, 4 GB of RAM and 2 cores, which might take 10 times longer.

Look at the details for the N-R Force Residual plot and it says which body has the Maximum.

If you have 4 N-R plots and 3/4 show the maximum on Bolt, then pay attention to the Bolt.

Regards,
Peter

  • Liked by
  • jonsys
Close