We would need your help in providing us the required steps to perform “static and dynamic analysis” of meshed spur/helical gears.
We are very keen if you can cover the below list of topics and any other useful analysis steps ( for high rpm up to 9000 and automotive grade).
Tooth contact analysis ( including AGMA/Hertz techniques)
Stress, strain and deflection analysis of gears
Crack formation analysis
Frequency, buckling and wear analysis
Thermal and Noise analysis
We want to ensure we are running the simulations( following the right steps) in a right way before we develop the gears and gear box.
PrePoMax is a pre- and postprocessor for CalculiX. Not all CalculiX’s features are currently implemented in PrePoMax and they require adding keywords manually (this applies to fracture mechanics analyses). CalculiX also has some limitations and, for example, it doesn’t support coupled structural-acoustic analyses so you may need another tool for noise analyses. The rest should be possible using CalculiX and PrePoMax but those are general-purpose FEA tools so they don’t have any built-in procedures meant specifically for gear analyses.
Thank you for your reply. Can you please share the instructions/video for what we can accomplish please?.
I understand the limitations of what we can’t cover in Prepomax + Calculix.
I will be eagerly waiting for your feedback/guidelines.
Sure please take your time to prepare the gear analysis.
In parallel shall we share the steps we are using for motor shaft, and meshed gear analysis. I hope you can give review and give us feedback. (If we are running the analysis in the right way i.e. following the right steps in Prepomax.).
Sure, describe your approach with as many details as possible - we will try to give some advice. And if you have some questions regarding CalculiX itself, this place might be better to ask: https://calculix.discourse.group/
I am not an expert in gear design, so I don’t feel I can offer much help in this regard. As was already mentioned, it would be much easier for us to help if you had a more detailed question and an example.
CalculiX as a PrePoMax FEM solver can mostly offer help in the field of static contact analysis. You can compute the contact stresses using a Static step with a 3D model and contacts. Using a Mortar contact (supported in the next PrePoMax version), the contact stresses will be much more accurate and smoother, even for coarser meshes. You can get stresses, strains and deflections from such an analysis.
Then you can perform a frequency (Frequency step) and bucking (Buckling step) analysis. The wear analysis (Slip wear step) is based on a very basic wear model and was not tested on a gear wear analysis jet. So I can not answer the question if it will work and how well it will work. But it is worth a try.
Thermal analysis is possible. The question is, what kind of thermal analysis do you need? The Noise analysis is unfortunately not possible using CalculiX.
I would agree with @SzPeter79 on this topic. Gear design is a very complex field and there are some great commercial solutions out there. On the other hand if we could developed some tools inside PrePoMax that would also be great.
Thank you for your feedback.
Well we have good expertise in Shaft and gears design and gear box. we are in the process of verifying if our designs make sense using FEA analysis ( i.e. Prepomax + CalculiX) before we take it to production. Any way I will share the steps for your review feedback.
Load to be transferred is 30Nm ( driver gear =20 teeth and driven gear =63 teeth)
We have applied load on to face of a tooth ( Ft= up to 2500 N)
We are not able to apply load onto the edge of a tooth ( i.e. we don’t know the process of how to configure in your tool). Can you please provide us with the steps?
All right, so for now you are analyzing gears individually, without modeling contact between two gears.
I would change the boundary condition at the back face of the gear since now it’s fully fixed and thus not very realistic. Of course, the choice of BCs depends on how the actual structure is supposed to be supported.
When it comes to applying a load to an edge, you could use concentrated force for that and calculate the necessary magnitude (the specified value will be applied to each node in the selected set).
Thank you for your feedback. I have applied concentrated force but not sure how to verify the load parameters related to 30Nm (load to be transferred) with an equation. Can you share any reference literature that we can refer.
One more link to simulate contact analysis between gears
Can you please review and let us know what is missing Iam getting too many warnings.
End of the day Iam trying to generate as per the analysis in you pic provided on your website
(Features – PrePoMax) next to Geometry based mesh creation section
If you want to simulate torque applied to the gear, you can also do it using a rigid body constraint. This approach will be easier. Just create a reference point in the middle of the gear, select it for rigid body constraint, pick a face or an edge to which the load will be transferred and define Moment load assigned to the reference point. Like in this tutorial: https://youtu.be/2upPxL45OZg
When it comes to the analysis with contact, I would do it differently, using the procedure described here:
You already have refined mesh and contact pair so just consider running a plane stress analysis for a start and use rigid body constraints (necessary to operate on rotational degrees of freedom for solid elements) to apply BCs to gears - you can make one gear free to rotate and apply angle of rotation to another gear. Torque will be worse for convergence.
Here’s a modified version of your model:
In addition to the aforementioned suggestions I made the following changes:
removed unnecessary faces from contact pair
replaced two sections with one since you have a single material
removed tie constraint (not needed here)
removed centrifugal load (not necessary when actual rotation is simulated)
Thanks a bunch and your quick turnaround is very much appreciated. I have tried using rigid body constraints but I was not sure if this is the right way of doing it.
