advice about Contact 1

[andreadelvecchio]

hello to everybody, I am attaching pictures of my problem.

the first picture is the undeformed of my first approach, a ribbon wound around a reel.
in the second picture I've try to applied several load to close the ribbon.
there is friction between the reel and ribbon. it work fine.
then I wanted to add another ribbon (figure 3 and 4) and do the same, but it doesn'd work.
the analysis does not increase. I dont'n know if it is a problem of mesh or contact or both of them.
any advice is welcome. thanks to all

 

[Dave442]

Hi,

You need to provide more details. What error message(s) did you receive when the analysis terminated?

Dave

 

[andreadelvecchio]

hi, the analysis does not calculate with any increase so the error is many attemps for this incremnt (1) or if I create some boundary conditions,but changes the problem, the errors is Time increment required is less than the minimum specified, but this is a fictitious problem , in my opinion does not depend by the size (that it is 1*-10),
i attach the file modified with boundary condition (abaqus 6.13)
I tried to activate on the second ribbon in a next step but the problem is always the bending of the two ribbons

 

[andreadelvecchio]

this file is the real problem

 

[rstupplebeen]

This reminded me of a post from a while back on the simulation of a CVT (Continuously Variable Transmission) If I remember correctly I did it in Explicit.

http://www.eng-tips.com/viewthread.cfm?qid=288995

Attached is the CAE file.

Hopefully this helps.



Rob Stupplebeen
OptimalDevice.com/blog
Rob's LinkedIn

 

[rstupplebeen]

Looks like the animation overwrote the CAE file which is attached below.

Rob Stupplebeen
OptimalDevice.com/blog
Rob's LinkedIn

 

[andreadelvecchio]

thanks rob, i try in next day, maybe is a problem of boundary condition after than i've seen your file. Maybe you saved me

 

[andreadelvecchio]

although with only ribbons works , for me the problem is with two

 

[andreadelvecchio]

dear rob, sorry to bother you.
I really do not understand why it does not work, can you help me?
the file momentaneo.cae work, it's with one ribbon.
the file momentaneo2.cae doesn't work, it 's with 2 ribbons, with the same bc/steps/load and mesh of previously file

I 'm going crazy

 

[andreadelvecchio]

this is momentaneo2.cae

 

[rstupplebeen]

Andrea,
I'm happy to help where I can. Here is an itemized list of change that I have made.

1. NLgeom=on
2. Maximum # of increments = 1000000 (prob not needed)
3. Use automatic stabilization.

I hope this helps.
Rob

Rob Stupplebeen
Rob's Engineering Blog
Rob's LinkedIn Profile

 

[rstupplebeen]

I forgot to mention that #1 at least needs to be done on the original single ribbon model as well.

Rob Stupplebeen
Rob's Engineering Blog
Rob's LinkedIn Profile

 

[andreadelvecchio]

Hi Rob, thank you for responding so promptly to my message.
after contacting you, I succedeed in finding a solution for the problem; I have also added more than 2 ribbons. But it works only if I toogle off in Non linear geometric. Do you think that it could go well? I think that it is a border line case. Then I have realized a sort of cantilever beam on another Fea and a hand calculation, and I have get comparable results (obviously cantilever beam resulted stiffer for the presence of the encastre)

 

[rstupplebeen]

My rules of thumb for enabling nonlinear are if there is contact or you can see the deformation without scaling then it should be on. I rarely do any simulations that don't have this toggle enabled.

The hand calculation and the other FEA are probably not factoring in the nonlinear geometry. Therefore you will get better correlation by not enabling nonlinear. This does not mean that it's a more accurate simulation though.

I hope this helps.

Rob Stupplebeen
Rob's Engineering Blog
Rob's LinkedIn Profile

 

[andreadelvecchio]

Hi rob, again thanks for your precious help.
I've tried to toggle on NlGeom, it works. I have tried both linear element (incompatible mode c3d8I) and Quadratic (red integration). finally they work, but the ribbons are very stiff. I've tested one ribbon, The ribbon have a section of 30mm x 1mm (E=210000 N/mm2) and if I apply a pressure of 0.01N/mm2 on the face near the end(the distance between tangent to the reel and the end is 400mm) (on an surface of 200mm x 30mm, so the force is 60N) the ribbon bend only for 7mm on the extremal edge...I think it is absurd. Meanwhile if i toogle off nlgeom the ribbons close as I want.

 

[cooken]

Andrea,

I think you may want to do some reading up on geometric non-linearity and large displacement - NLGEOM is not the source of your problems. The cause of the increased stiffness might be tension stiffening, or it might be poor mesh refinement / element selection, or it might be something else related to how you have established the contact. If you are concerned about the stiffness of the ribbon, you should run a separate, simplified analysis and resolve any issues there to gain confidence that your FEM is doing what you expect.

 

[andreadelvecchio]

thanks cooken,
I was doing all the evidence in the case, as you said.
Both you and rob have reason, i have resolved my problem, there was a boundary condition that with nlgeom stiffed all the ribbons in bending. Now I am using nlgeom on and incompatible mode, also I am trying the quadratic elements, but I think that the analysis time is fitting for little different results.
thank you very much, rob and cooken.
last stupid questions: How can I export the deformed shape in autocad? and, i've done a simply supported beam with pressure on bottom, and i want valutate the stress in the middle, why the stress increase if I reduce the size of the elements?i want the absolut stress in one direction, I dont'think that I have to consider the area...or no?

 

[andreadelvecchio]

i read in Probe>nodes it is wrong?maybe i have to read in integration point?i am confused