# Spur gear analysis

• 400 Views
• Last Post 10 October 2018
muzamil_k posted this 02 October 2018

Hi,

I tried to simulate spur gear using Stuctural Analysis in ANSYS 19.1 Student version. I already calculated contact stress between spur gear using AGMA equation and Hertz equation. The value is 738.21 MPa and 856.12 MPa respectively. Below is the specification of the spur gear:

I have tried the same boundary condition based on Spur Gear Analysis discussion (noted that I did not use the symmetry plane yet on the simulation) but there is error in the solution.

I hope anyone can show me the correct way to run the simulation.

Thank you.

Attached Files

peteroznewman posted this 02 October 2018

What is your goal for running this simulation?  Is it to practice building a contact model with a known answer? If that is the case, I recommend you select another problem with a known answer that has simpler geometry. There are lots of textbook problems with Herztian contact with known values of stress with simple geometry like a sphere on flat, or two crossed cylinders.

The issue with your chosen problem is that gear teeth are not made from simple geometry. Gear teeth use involute curves. What CAD system made your STEP file? Most CAD systems can represent the space a gear takes up, but use some approximate curve that is not an involute.  With some extra effort, some CAD systems can draw an involute curve, but you have not provided all the gear tooth design parameters that the gear designer uses to cut real gear teeth.

Regards,
Peter

• Liked by
muzamil_k posted this 03 October 2018

Hi Peter.

My goal is to compare the stress calculated using Hertz and AGMA equation with simulation. The reason I am using the spur gear is because my research required me to do so. Finite Element Analysis of Stress Variation along the Tooth Depth for Steel and Plastic Gears is my research title. For CAD, I am using PTC Creo Parametric 3.0 to create the gear geometry.

For your information, Frictional Contact Stress Analysis of Spur Gear by using Finite Element (attach below here) is one of the article I used to validate the calculation. Picture below here is my the calculation to validate the theoretical calculation.

Regards,
Muzamil

Attached Files

peteroznewman posted this 03 October 2018

Hi Muzamil,

Can you find out if the gear tooth geometry is a true involute or an approximation in PTC Creo 3.0.  I know SpaceClaim can draw a true involute curve.

Review the following discussions and see if you can figure out the steps you need to follow.

Regards,
Peter

Guidelines for posting

• Liked by
muzamil_k posted this 03 October 2018

Okay Peter. I will confirm back whether the gear tooth geometry is a true involute or not.

Regards,
Muzamil

peteroznewman posted this 03 October 2018

Muzamil,

A requirement to have the solver start successfully on a contact model is that the two faces that you want to press on each other have to be just touching in the geometry editor before you mesh and solve. It can happen that the parts in the geometry editor are perfectly tangent, but after meshing, a tiny gap appears between the faces of the elements. This tiny gap can be closed by using Adjust To Touch in the Contact definition.

Another consideration is that the gear teeth make contact along a line. The stress varies on one tooth from when the tooth first makes contact, to the point when the contact point is on the centerline between the gears, to the last point of contact.  Your calculation above shows only a single value of stress.  You must also specify where the contact point is when you report that value of stress.

Regards,
Peter

• Liked by
akhemka posted this 05 October 2018

Hi,

Just a suggestion - In case adjust to touch does not help then please see if using a rotation via remote displacement helps.

Regards,

Ashish Khemka

muzamil_k posted this 10 October 2018

Dear Peter,

I checked my assembly in the CAD. The contact was at the pitch circle of the gear (in the red circle).

Also, I tried to run the simulation. I remove the excess geometry to reduce the number of nodes and elements. Is there anything that I should do to make the simulation be as good as previous one ?

Regards,

Muzamil

peteroznewman posted this 10 October 2018

Muzamil,

It looks like you have a good model working.

Since the Max Stress is at the center hole and that is not relevant to this study, I suggest you split that body into two bodies. You can put those bodies into a single Part to make a Multibody part and use shared topology to connect the mesh. Then when you plot stress, you can do so for the body with the gear teeth and don't include the body with the fixed support or revolute joint.

If the revolute joint is on the left with the Max stress, maybe simply changing the behavior from Deformable to Rigid might make that Max stress go away.

Regards,

Peter

• Liked by