Novice Question - ‘total load at point’ Hex Driver

[IE_1]

Hello All,

I’m trying to simulate torque applied to a ¼” hexagonal driver to a reduced A/F set screw. I have set the simulation up but getting very high stresses in the results.

My question is does applying the ‘total load at point’ effectively divide the moment load by 6 in this case, the point created is at the centre of the hex? Due to the stress reported I suspect I may have to divide the torque value by 6 manually when setting the load up?

[KenFarley]

If it was me and I were trying to represent the reality of the situation, a point load is not what I'd use to represent things. I'd start with:

(1) Make a model of a hexagonal bar, the end of the allen wrench.

(2) Assemble this hex in the head of the screw in your analysis assembly.

(3) Apply a torque or moment load to the "wrench". If it's easier, when modeling the wrench, model a blend to a cylindrical shape at the end so you can apply the moment to the cylindrical surface.

You might have to look at the contact definitions for the wrench, otherwise it will be assumed that it is perfectly bonded to the interfacing  surfaces, etc.

I haven't done this, so don't know if it's the best approach, but maybe someone with much more experience will have better suggestions.

[IE_1]

Thanks for the reply.

I modelled the hex 1/4" then with a reduced hex to represent the socket A/F.

I did all the analysis within a single part.

I created two volume regions at either end to represent the constraint and load areas.

I fully constrained the contact region (socket screw end) in all degrees of freedom, then applied the load in terms on Nm torque to the contact region (driver end) then added a centre point for the torque moment to act around.

But as mentioned the stress is very high so unlikely to be representative.

In CREO simulate I am very new to this and haven't touched FEA in over 25 years, was pro mechanica back then. So I'm not sure I'd be able to action your approach just yet. 

[skunks]

Please upload the STP data.

[IE_1]

File attached - Thanks.

[skunks · Accepted solution]

Here is a testpart1.

[IE_1]

Thank you for taking a look, I see you have applied the torque to the socket end (grub screw) over the entire length of the 0.9mm AF? Would this not be a volume region at the engagement height? 

Also you have constrained the flat face at the top, would this not need to be another volume region at the driver engagement height?

I also thought this would be the other way round, i.e. the torque is applied to the driver end and constrained at the allen key end?

I'm not saying you are wrong I would just like to understand why it is best practice to do it this way?

I'm trying to simulate putting 0.3Nm through this driver. 

[skunks]

The thin end of the tool is soft, so do not clamp it there (this will distort the results).

You also need the exact material properties here, so please check the material and set the correct values.

[SweetPeasHub]

Hi,

These are great questions and so here are a couple things to improve your understanding.

1. Newton's Third Law of Motion and also St Venant's principal is why we want and can have the rigid constraint away from the stress area of interest. Everyone doing FEA needs to understand what this principal means to their analysis.  We can do loads at both ends or constraint and load at either end and have static equivalence. Constraints inherently also rigidize so keep them away from where the high stress might occur.

2. Get a gut check with a generic case. For this a rod in torsion. If you apply a torsion on a constant section bar the stress is exactly the same at every cross section. So for your real case, the general torsional shear stress only slightly changes with different depths of screw engagement. If the depth is very shallow then local effects may override the general torsional stress. For an ideal 1mm solid circular rod in torsion of 50N-mm the calculated shear stress is 255MPa and the von-mises stress is about 441MPa. For @skunks model we get 419MPa max von-mises stress. and a maximum shear stress of 242MPa. It is therefore within engineering tolerance to assume a 1mm round rod instead of the hex rod. Also model setup is confirmed. We can then proceed to evaluate varying the depth of screw engagement to find when local effects might be significant. A detailed study would include the screw in the analysis and model the actual contact forces, since they will not be as uniformly distributed as the even forces in the current model. Also since hardened tool steels can take upwards of 1000MPa we might have a maximum allowed torque near 200N-mm by the shear stress as a criteria.