# effect of reverse torque on a jig

• 97 Views
• Last Post 06 September 2018
• Topic Is Solved
malay_shankar posted this 04 September 2018

The attached para solid file is a jig (1/3rd of the full geometry). It has a torque hinge (aluminum alloy) joined to the vertical arm (nylon 66 30% glass filled). The forward and reverse torque values for the hinge are 14 in-lbf and 24 in-lbf respectively. The two screws holding the hinge are made of stainless steel. The arm also has two Keenserts made of stainless steel.

I need to know the deformation and stresses developed in the parts when the arm will be pulled to flat.( initial position is as in the parasolid file and flat position is when angle b/w the hinge and arm is 180 deg.

Will this be solved using static structural module or rigid dynamics?

Also, are the keenserts safe?

Attached Files

SandeepMedikonda posted this 04 September 2018

Hi,

Can you please explain your problem using images? That way more ANSYS engineers will be able to answer/give suggestions.

Regards,

Sandeep

• Liked by
peteroznewman posted this 05 September 2018

Hi Shankar,

The stress results from my model showed the highest stress was in the thin handle at the top, not around the hinge at the bottom, but that is because I assumed the user holds the part at the top. If that was the wrong assumption, and say, for example, the user grabs the arm around the thicker part near the rectangular hole in the middle, then the highest stress would probably be near the hinges. It's important to identify the worst use case and analyze that. If I made the right assumption, then the simple model I described above has adequate detail around the connection.

However, anytime there is a hinge, there is likely to be a worst-case load compared to simply operating the hinge as designed.  What does the arm stop on, in either direction?  How much force can be applied to the end of the arm when the arm hits the stop? Those load cases probably generate much higher stress levels in the part than the normal rotation of the arm against the hinge torque.

Bolt pretension requires some geometry prep work, but in this case, I don't think it will be helpful. The reason is that the keensert is level with the face of the part, so Bolt Pretension will only serve to squeeze the steel keensert against the aluminum hinge. Since we are not concerned with those parts failing, the bolt pretension doesn't provide a benefit.

To your question on cycles to failure, you need fatigue data for the glass filled Nylon to answer that question. This data is sometimes available at the material supplier's website, but most of the time I look, it is not there. Contact the material supplier and ask for it. It takes the form of a table of Stress Amplitude vs. Cycles to Failure and has many data points over a range of stress values. This will only tell you about a failure due to cracking.

Another analysis you can do is thermal cycling. Since the steel kenserts and the gf Nylon have different thermal coefficients of expansion, if this assembly experiences frequent large thermal cycles, a cyclic stress will be created at the interface between the keensert and the Nylon. That stress could be larger than the stress due to rotating the hinge against the torque load.

Regards,

Peter

• Liked by
malay_shankar posted this 04 September 2018

i have updated my problem with an image

SandeepMedikonda posted this 04 September 2018

Hi Shankar,

If you want to look at the stresses and deformation in the parts, I would expect to perform a structural analysis and it looks like you might need those keenserts as well to establish contact, you can also alternatively use contact offsets or bolt pretension if having those is significantly slowing down your model.

Regards,

Sandeep

peteroznewman posted this 04 September 2018

Hi Shankar,

What do you mean 1/3rd of the full geometry?  That is not useful. You can use Symmetry if you cut your full model in half. Go back and cut it in 1/2.

I opened the attached iges file. The holes in the Nylon part are not large enough to take the insert. Increase the diameter of these holes to match the size of the insert.

Use a Static Structural analysis. I recommend simplifying the model and initially leave out the inserts and the screws. Create two Fixed Joints between the sides of the larger hole and the inside of the hinge hole. That way, there are only two parts in the model, the Nylon part and the half of the hinge that is fixed to it. You can leave out the screws and the other half of the hinge.

At the top of the part where the fingers would wrap around the end, hold two faces Fixed, and apply the Moment on the Hinge.

Now the model will solve and you can get a first look at the stress in the part.

Attached is the cleaned up Parasolid file inside a zip file.

Regards,

Peter

Attached Files

malay_shankar posted this 05 September 2018

Thanks a lot Peter. I will do as instructed above and will surely let you know the results and questions if any.

Clarification: 1/3rd of the model

- actually we should be considering it as a full geometry and not 1/3rd as mentioned in my previous statements.

malay_shankar posted this 05 September 2018

I solved it and got the stresses in the parts.

Can you also guide me on how many cycles until the arm breaks at the connection point? how to proceed with this type of analysis?

malay_shankar posted this 05 September 2018

Hi Sandeep, I solved and got the results. I also applied the bonded connection for the keenserts. I will apply bolt pretension now and will let you know in case any problem arises.

Thanks.

malay_shankar posted this 06 September 2018

Hi Peter, this part will never be subjected to cyclic or thermal loads. So, no question of fatigue or thermal cycle effects.

And so far i have got the required results. Will surely ask you in case any other scenario arises.