Problem with the results in abaqus

[lem0n23]

Hi, i'm new to abaqus and i am trying to make some tests in a wheel. The wheel is made only by carbon fiber.
I think that i made everything right, choosing the material, the composite layups for the rim and for the wheel walls, the load. However i'm not so sure about the BC's that i choose, they might not be the right ones.
So, when i run the job, in the result the deformation doesn't match with the expected...the expected is the rim to bend on the extremity's due to the applied pressure. But the result shows an expansion of the wall near to the rim as i show in the picture

http://alojaimagens.com/images/u1cu6n16n7p2aomvjyia.jpg

http://alojaimagens.com/images/qecm6sqqx1o9nxzgu6zd.jpg

I appreciate all the help

Tiago Carrola

 

[rstupplebeen]

In your results image the deformation scale factor is 3e-5. Basically I believe you have a units issue unless you expect this to deform quite extremely which is unlikely with carbon fiber. I hope this helps.

Rob Stupplebeen

https://sites.google.com/site/robertkstupplebeen/

 

[lem0n23]

The problem its not the scale nor the units. The problem is that the rim doesn't deform...expands. And i need to know the values of deformation and tensions on the rim, witch i can't because the rim doesn't deform.
What am i doing wrong?
Thanks for the reply

 

[mechfeeney]

Looks like your rim is made up of multiple components (tube carriage and side walls?) Are you applying tie constraint between them? You need to give more details about the problem...like how you are applying the nodes, your material values, etc.

 

[lem0n23]

I made the wheel on SolidWorks and then imported to Abaqus by *.igs, so i don't think that i have a problem with multiple componentes because in abaqus it's only a part..but that it's just me thinkin, what do you guys think?
No, i'm not applying tie constrain between them.
And the values for the material are:
E1=E2=70 GPa
Nu12=0.1
G12=G23=600 MPa
G13=570 MPa

I'm making seed, and then mesh instance..i'm not distribute the nodes by myself.
I need a result like these one

http://alojaimagens.com/images/y7y7o7oll6yoiq6kl86k.jpg

 

[mechfeeney]

Sounds like you are trying to rush to a solution rather than fully understanding how to model the problem properly. It tends to be a big mistake to try to warp your results. I still have no idea what's going on in your model because I don't know what the boundary conditions are and how the loads are applied.

 

[lem0n23]

No, i'm not trying to rush, but i'm trying to make this work since a few weeks ago and still can't figured why is not working.
In the pictures you can see, i applied a pressure to the internal part of the rim

http://alojaimagens.com/images/toi4xbzohkfdjlr4l7.jpg

then i made the BC's, a displacement for the center wheel, where will be the bearings

http://alojaimagens.com/images/toi4xbzohkfdjlr4l7.jpg

and finally a encastre where will be the fixation of the wheel that permits the rotation of the wheel.

http://alojaimagens.com/images/7to6dqt1wu8b7y5kc6jz.jpg

i don't understand what i'm doing wrong..maybe some kind of propertie that doesn't allow me to see deformations on rim.

When you apply pressure to a rim, the rim it's suposed to bend due to pressure, not having the results that i'm getting

 

[mechfeeney]

Uhhh, "and finally a encastre where will be the fixation of the wheel that permits the rotation of the wheel." What do you mean by this? Encastre fixes all degrees of freedom (not just rotation). What kind of BC is applied to the center where the bearing would go (Which degrees of freedom did you constrain)?

 

[mechfeeney]

If I had to venture to guess, I'd say your problems are stemming from your BCs. I could be wrong though.

 

[lem0n23]

i mean..the rotation of the wheel is caused by those 4 wholes. In those 4 holes will be a screw that transmits the power from the hub to the wheel, so i made it encastre. you can see the real wheel in the picture but with 6 screws instead

http://alojaimagens.com/images/ho0xjv9s8klavyu4qcu.jpg

To the center of the wheel i applied the displacement/rotation BC and i constrain the U2 and U3

http://alojaimagens.com/images/1zukghykjcapafhttg9f.jpg

 

[mechfeeney]

I think the combination of those boundary conditions is a bit redundant. Could you attach your model (if it's not too big of a hassel). We could probably go back and forth for a while before arriving to a solution.

 

[lem0n23]

http://www.fileserve.com/file/E8JZjkE/Desktop.rar

here goes the file, feel free to check it

 

[mechfeeney]

Looks like you have a units problem with your thickness. When I rendered your wall thickness it took x1000 scale factor to see anything. Check your wall thickness units, material units, and the units you used in your cad model.

 

[mechfeeney]

Also your mesh is way too coarse. Look at the difference between your model and the example one. See how small his elements are? You have a very high aspect ratio for your elements in the areas with the issues.

 

[mechfeeney]

One other thing. The warning message you are getting suggests what is shown in the attached image. The picture shows an 4-node shell element viewed on the side in 2D. The angle between element normal and node normal is larger than 10deg at because the shell has to wrap around the really sharp corners of your model. This is where the area where the model is having issues as well.

 

[mechfeeney]

image

 

[mechfeeney]

Sorry for the multiple posts but let me summarize the problems with your model:

1. Material properties are in meters. Your model is ~400 units in diameter. If you use meters for your material...then your model is 400 meters in diameter and your thickness is 0.00018 meters thick. In other words, you have a lot of unit inconsistencies here that are leading to a very unrealistic/incorrect model. (abaqus is unitless, it's up to the user to stay consistent)

2. You have a curvature based mesh that has the nodal normal and element normal issues as described in the picture above. You may need to do local mesh refinement in those areas to prevent the elements from wrapping too much.

3. Overall your mesh is too coarse.

 

[lem0n23]

ohh ok. I know that abaqus is limitless. I put wall thickness 0.00018 m because that is the value of a layer of carbon fiber. So the wall thickness it's suposed to be the value that i expected from the sum of all layers of carbon fiber. I will fix that.

And i will try to do local mesh on the rim, where is the cause of all trouble. Not so sure if i'am able to do the right thing on the mesh though due to my inexperience with meshing.

But i really appreciate all your efforts to help me!

 

[lem0n23]

I changed the values of thickness, so now all vallues are in millimeters. Changed the elements in the mesh, so now the mesh in the rim area is much more fine than previuosly as you can see in the picture..but still the same problem persists.

http://alojaimagens.com/images/zbph5kdrg40fradha8.jpg

do you think my problem still is the mesh, or maybe i'm having another kind of trouble?

 

[lem0n23]

Done. I managed how to fix the problem. It was the mesh, now it's ok. Just give me a tip..how can i change the "efects" of deformation, to not see it so exagerated?