Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in
  • Congratulations waross on being selected by the Tek-Tips community for having the most helpful posts in the forums last week. Way to Go!

Meshing gears in Abaqus - contact analysis 5

Status
Not open for further replies.
vjantarajunior

vjantarajunior

Materials
Feb 15, 2016
12
0
0
GB
Hello everybody,

I am new to Abaqus and have been trying to do contact analysis of a pair of spur gears some time now.
If anybody has performed such analysis, please let me know. I would be really grateful!
What I have done so far:

1. Created and imported a Solidworks file for the gears;
2. Created the material, section, and assigned section to parts;
3. Meshed the parts;
3. Created a kinematic constraint on a reference point (in the center of the gear) to its inner surface, in order to emulate the shaft;
4. Created a contact interaction (friction coefficient of 0.12)
5. Created the interaction (my gears are on the YZ axis, therefore:)
BC1 - pinion - angular velocity - able to rotate only on UR1
BC2- gear- angular velocity - able to rotate only on UR1

The thing is, if I apply a torque to the gears, they will not rotate. I know that this may be a dumb question, but shouldn't they rotate only with a torque applied?
I have already checked my units, and they are consistent. I apply the torque on the reference point at the center of the gear since it is constrained to the inner surface of the gear. Am I doing it right?

If a do apply an angular velocity to the pinion (changing the BC1 to 1 rad/s on UR1 for example) then both gears will rotate. But when I apply a torque to the other gear, I get no difference in the S stress results! I've tried both small and huge values, and I get no difference. It's as if torque makes no difference on the analysis!

Should I just change the angular velocity and calculate the torque based on it? If so, how do I calculate?

>>>My goal is to understand how varying the torque will affect the contact stresses.<<<

Here are my files:
Thanks a lot!
 
Replies continue below

Recommended for you

Sort by date Sort by votes
There are rigid body motions in the model.
Coupling on contact area is not a good idea.
Gravity without mass (density) is also useless.
And some other questionable definitions...

You should consider doing the analysis in 2D, if you don't want to wait a long time for the result (asuming you get it running).
 
Upvote 0 Downvote
Hi Mustaine,

Thanks for answering.
Just now I realized that I have uploaded an old version of the simulation that I was trying to do. This is how a colleague of mine made the simulation work, and I agree with you, it has very questionable definitions.

I have already dropped the rigid body, and the gravity, but I do not understand why do you say that coupling on contact area is not a good idea.
You mean I should do the constraints in other way?
If so, how would be the best way to do it?

Thanks!
 
Upvote 0 Downvote
Hi,

I started the model again, this time with two equal gears.
This is the new assembly:


(Same link as before but it is the new assembly inside)

On the first step, I apply an angular velocity of 0.5 rad/s on gear A.
On the second step I should apply the torque on gear B, however, I get an error.
If I supress the torque, the model runs again.

Any idea of what I might be doing wrong?

I also get the following warning: "There are 2 unconnected regions in the model." What could I do to get rid of it?

Thanks!


 
Upvote 0 Downvote
Hi vjantarajunior. Unconnected regions could either mean that the parts are not given appropriate boundary conditions or that solid regions in a part could be disconnected. I would suggest performing a check for any surfaces or solids with gaps and any degrees of freedom that are not constrained properly.

Is gear A driving gear B? Why are you applying angular velocity in one step and torque in another?

 
Upvote 0 Downvote
In casual terms, something is freely floating in free space. You need to constrain sufficient number of DOFs before the solver can solve the system of equations. Chances are you may need to use displacement control to bring bodies in to contact first and then switch to load control.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

 
Upvote 0 Downvote
tkks2040, IceBreakerSours,

Thank you for your help.

My line of thought is the following, as I saw in this thesis, page 60:
Divide the problem in 3 steps

1st step: make contact by introducing a displacement (rotation) boundary condition in one gear, while keep the other totally fixed
2nd step: apply the torque (ramped), while "freeing" the restrained gear to relieve the tension that may have been build due to the 1st step
3rd step: maintain the torque (now at full power), and apply the angular velocity (now with both gears free on the rotation DOF)

So for the first step, I have tried to apply a small rotation on one gear, while leave the fixed on all 6 DOF. However, I do not know exactly "when to stop", it is, the actual clearance between the gears. Therefore, the rotating gear will get "inside" the fixed gear. Then, when I start the second step, the model obviously aborts.

(If I try to do this, with the "fixed" gear free on the rotation direction, the model simply crashes on the first 5 attempts for the first increment! That is why I have restrained all 6 of them.)

This is why, tkks2040, I was applying angular velocity first and then the torque after. I was trying to overcome this obstacle with angular velocity. But I do not think this is the best approach.

Is there a way I can "tell" Abaqus to stop when the contact is made between the gears?

Thanks again for the help guys.
 
Upvote 0 Downvote
Hi StefCon,

The model looks very good. I am also using a similar friction coefficient (0.12), but eventually I will have to decrease this, since the actual coefficient for lubricated gears is much lower.
Would you still have the CAE and JNL files around? It would be great to see how exactly you placed the boundary conditions, as well as the amplitudes for the loads.
That's what I am having the most problem with.
Thanks a lot, this was of great help already!
 
Upvote 0 Downvote
Hi,
You are right about the friction. 0.1 is a lot for lubricated gears. I used it out of old habit. :D

I am afraid I do not have the .cae anymore. If you import model into CAE you can view how things were made (it doesn't look as nice as the .cae but it works).

I think I used Dynamic implicit step, general contact (no initial overclosure, otherwise there might be some strain free adjustments (unless you change the contact initialization settings)), applying the rotation velocity amplitude 0,0;0,1 with a "smooth" amplitude. At the same time you can ramp up the torque with the same amplitude. I also added beams as axles so that it would give my system some more flex.

Checking energies is important. I didn't do that. Maybe the "moderate energy dissipation" in the step is too much to give accurate results.


Good luck!
 
Upvote 0 Downvote
StefCon,

Thanks again. I did not know one could import an .inp file, I had opened it with the notepad app. I would like to ask you about:

1) I do not really understand the purpose of the axle. My guess is that instead of using a "reference point" to constrain the inner surfaces and emulate the shaft, you actually used the axle, and fixed it in the X and Y directions. Am I right?

2) Constraints:
I've noticed a lot of constraints. Are all of them needed, or only constraints-1 and -2 would do the trick? It is, if I am not using a axle as you are. (They are the ones that constrain the reference point to the inner surface, emulating the shaft)

3) Boundary conditions:
Also, I've noticed a lot of BCs.
I believe that these 3 are sufficient, right?

** Name: BC-1 Type: Displacement/Rotation
*Boundary
Set-24, 1, 1
Set-24, 2, 2
Set-24, 3, 3
Set-24, 4, 4
Set-24, 5, 5
** Name: BC-2 Type: Displacement/Rotation
*Boundary
Set-23, 1, 1
Set-23, 2, 2
Set-23, 3, 3
Set-23, 4, 4
Set-23, 5, 5
** Name: BC-3 Type: Velocity/Angular velocity
*Boundary, type=VELOCITY
Set-25, 6, 6, 62.8

4) There are also 2 predefined fields. Did you use them in the analysis?

5) Just out of curisosity, regarding the parts, did you draw them or did you use a library such as the ones there are in Solidworks, for example? If so, which?

Thanks again and sorry for bothering with this. It's been a huge, huge help!
 
Upvote 0 Downvote
Hello,

1) I made the axles to simulate the effect of having a slightly softer setup (more realistic). A softer setup could lead to having the axles bend and increasing the center-center distance between the gears (guess). Also, since I was feeding my system with a constant rotational velocity, an unrealistically stiff setup might give me unrealistic variation in the transferred moment (and maybe contact pressure).

2-3) If I remember correctly, there should be 4 boundary conditions in .cae (when you read the input file each constrained DOF will become its own constraint). The constraints should represent two radial supports per axle and one axial support per axle (see attached). About constraints: I wanted to mix it up a bit and I think I used shell elements for the gear hubs. Solid-to-shell couplings were used to connect the two.

4) The predefined fields were used to make the analysis start at a rotational velocity and not from a standstill. This makes what I wrote before about ramping rotational velocity wrong. I only ramped the torque I guess. Note the magnitudes 62.8/52.33 ~ 18/15 (gear ratio).

5) I got the gears from grabcad. I did not have patience to make them myself. The involute shape (right terminology?) looked good. If it was correct or not I cannot say.

Cheers!
 
 http://files.engineering.com/getfile.aspx?folder=753933bf-8367-452f-9d68-1219bd6d3294&file=gears.png
Upvote 0 Downvote
Hi guys,
It is me again. I did not know if I should open a new topic, but since it is related to the same model/topic, I thought that it would be best to keep it all on the same place.

First of all, I would like to thank you all for your help. I followed you advice and developed a 2d model first, in order to understand the simulation better.

I was able to make it run smoothly – and figured out that it was time to go to the next step – 3d modelling.

I’ve kept all the variables the same: it is the same pair of gears (I drew them in Abaqus itself, by a python script. The only thing that changes is the last line of code – instead of making a planar shell, I then extrude the part), it’s the same boundary conditions, load, steps and incrementation, etc, etc.

In 2d, the model runs smoothly, and when one teeth is starting to finish its interaction, another teeth starts the interaction at the same time. When I then switch to 3d, it runs as if one teeth is separated from the other. It is as if only one teeth were in contact at each time. Please look at the attached screenshot and you will understand it.

I have attached the models and python script if want to take a closer look:

It looks like a geometry problem, but how can it be, since it is exactly the same drawing?
Do you have any suggestions on how to solve this?
 
Upvote 0 Downvote
Hi,
Have you checked the torque that you apply? What did you set it to in the 2D model and what did you set it as in the 3D model?

Cheers!
 
Upvote 0 Downvote
Hi Stefcon!
In fact, I had not checked the torque: I was applying the same 500 N/mm for both the 2D and the 3D.
I have just made a test, putting 5000 N/mm for the 3D model, and I have got the average stress numbers very close on both models, and better yet, the contact problem was solved! Now there is continuity in the movement.
Thank you a lot, again!
 
Upvote 0 Downvote
Hi,
I think that the 2D model is given 500 Nmm per unit depth. So if the 3D gears have a width of lets say 15 mm, the torque should be 15*500 N/mm = 7500 Nmm*.

*I could be wrong on this one. I haven't worked that much with 2D models. If I am wrong, please correct me.

Best regards,
 
Upvote 0 Downvote
Hi vjantarajunior,

i'm new in abaqus. have been month looking for this setup.
your thread was soo helpful for me.
thanks a lot.

how's your full analysis progress....
have u publish any paper on what u been doing?

tq
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

mj345
  • Question
Hybrid Meshing in ABAQUS
Replies
1
Views
40
FEA way
FEA way
robertt3
  • Locked
  • Question
What's the default contact damping value in ABAQUS/Explicit
Replies
6
Views
69
Marekcom
Marekcom
Sakthiiitm
  • Locked
  • Question
Moving load analysis in ABAQUS
Replies
3
Views
15
FEA way
FEA way
Maria Kxr
  • Locked
  • Question
Abaqus Explicit - Error in restart analysis
Replies
5
Views
11
FEA way
FEA way
FEA_User
  • Locked
  • Question
Heat transfer analysis with abaqus
Replies
5
Views
30
FEA way
FEA way
Back
Top