Creo Simulate - Advice on constraining model for mechanical stress calculation

[EddyVE]

Hi all,

Using Creo 4.0 

I would like to ask some advice about how you would constrain this (red brownish) U shaped bracket for the shown load situation.  

The bracket has 2 holes with a pin in it (so it can rotate). Both holes are loaded with force F/2.

Force F is applied on a bolt that is placed in a screwthreaded hole in the bracket.

I have modeled the bracket like this:

For the pin hole, I use a bearing load with force F/2.

I use a displacement constrain to implement symmetry on the cutting surface:

I use a surface region to constrain in the axial direction of the screw hole. (cylindrical CS).

This model calculates fine, but as can be expected, I have a stress peak at the side of the surface region.

Not sure if that is entirely realistic.

A slightly different approach is to exchange the screw hole by an 'embedded' bolt, and constrain the tip of the 'bolt':

This results in a (lower) stress peak at the indicated spot below. Perhaps a bit more realistic than my first attempt above.

Would you model this in a different way?

PS.  Part file attached in case you want to have a go at it.

[ChrisKaswer]

To keep things as simple as possible and model the best set of BCs, I would constrain the screw hole from your first example, in both the radial and axial directions, and remove the small washer shaped constraint region meant to act as the screw's constraint. This will closely-enough mimic the situation the screw will impart on the threaded hole - it limits it's deflection radially and axially. More accurately, the screw thread engagement is not along the entire length of the hole, so you could play with that region a bit too. Of course, keep the symmetry condition on the cut half. You will always get a result with concentrated stresses, as in your first set-up, due to the fact that your constraint boundaries have a sharp edge to them and create singularities. Removing these assumptions with actual parts in contact is the only way to improve the accuracy and minimize (almost eliminate) these BC stress risers, but that is a more involved model.

I hope this helps!

[EddyVE]

Hi Chris

I made the changes as you suggested, by placing an axial and radial constraint on the screw hole itself. Did not really make a significantdifference.

I also limited the depth of the screw hole (actually the depth of the constraint on the screw hole). Also not a huge difference:

Adding rounds on the hole edges, just for the heck of it ...:

The stress is concentrated on that edge, right at the symmetry plane.
Let's place the symmetry on the other plane...:

Let's round those edges again and use finer mesh size there:

Still high stress concentrations there. But perhaps realistic ....

[ChrisKaswer]

Unfortunately, we'll never eliminate stress risers at BC edges, so results will always need to be observed with that "filter". Your vM values may not have changed much as a straight-up number..,but also take a look at how the stresses are distributed because of the change in BCs. Also be careful when comparing results with and without rounding AND, always look at maximum principal stress and its distribution along with an animated magnitude displacement result. This will indicate where your material is in compression and tension (min prin can be reviewed as well) - this will have very likely changed from your original model and it can often provide a significant insight to how your part will behave. Remember, von Mises is an "absolute numeric" stress value and does not indicate compression or tension.

[skunks · Accepted solution]

my suggestion attached, still without mesh refinement

[EddyVE]

Thanks for your suggestion! 

Interesting idea to model the screwthread so detailed!

Unfortunately, I don't have the required Simulate license to run a simulation on it ...

[skunks]

OK, V2 att.

[EddyVE]

Thank you so much! That worked!

Strange that Max Principal so small is in the spot where VM peaks ...

[skunks]

"...Strange that Max Principal so small is in the spot where VM peaks ..."

please look for Min Principal

[EddyVE]

"please look for Min Principal"

Oops! Right you are!

VM            :  168 MPa
Max Principal :  155 MPa (on different location)
Min Principal : -176 MPa (same location as VM peak stress)

[EddyVE]

Redistributing material also helps ...

[SweetPeasHub]

And stress relief ~10% less stress.  😀

[EddyVE]

Stress relief features.... Great suggestion! I will check that out!

Keep those ideas coming..! 😊