IMPACT/CONTACT Analysis 1

[iyj]

Dear All

After Rob's suggestion I am making this a new thread and including the original question and answers from the previous thread.

Before I start my question, I would like to appreciate the efforts of people helping each other, thats reallt great.

My question is that I am trying to model a 2D contact problem (indentation of a steel sphere on rectangular Alimunium plate). Now as I am a beginner. I have modeled the plate with Aluminium properties and steel with its properties. Made contact with each other and defined steps and applying displacement load on top of the indentor. The application runs successfully. But what I am trying to achieve is that it shows the deformation when applying load on it. But i also want to see when we remove the indentor how much deformation remains after unloading. So the problem is unloading and do i have to create a seperate step for that, and if i do, both part will still be in contact so how do i do that.

please do help me in this regard as I am really struggling.


Thanking you in advance






rstupplebeen (Mechanical) 28 Jan 10 9:19
For future reference this should be in a new thread.

You can do this a couple of different ways. Create a new step and have the displacement go back to zero. Or, Create an amplitude that the displacement references that ramps from 0-1-0 for time points 0-.5-1.

You will need to include plastic deformation for the aluminum plate otherwise you should have no residual stresses.

I hope this helps.

Rob Stupplebeen



iyj (Mechanical) 31 Jan 10 2:20
Dear Rob

I thank you alot for these helping comments and suggestions. I will try these out and will let you know the outcome too. Once again thanks alot and really appreciate your effort.

Best Regards


iyj (Mechanical) 31 Jan 10 7:04
Dear Rob

It really worked I am so happy, thanks alot really thanks. While attempting the case there was a minor issue and that was when it was unloading it was not going to its original place. like fist displacent i gave was (U2= -0.05, ), and the second BC was U2 = 0, rest remain unchanged. i wanted to to see the final force comning back to zero. The plastic thing really worked, thanks.

Please do let me know where i am wrong.

Regards


iyj (Mechanical) 1 Feb 10 6:11
Dear Rob

In the second step which is the unloading, instead of force going back to zero it actually increases. I already gave the displacement(U2=0) for the final step, but still this problem occurs. Do I have to disconnect both the parts so there is no contact in between them. if yes How do I do that?. Can you please let me know.

Or if not plz can you correct me where I am wrong

Thanking you in advance


Regards

 

[rstupplebeen]

What force are you calculating? Could you post your model or provide some pictures. At the end of the second step is the indentor sill in contact with the plate?

Rob Stupplebeen

 

[iyj]

Dear Rob

I thank you for replying. Ok I have attached the CAE file for the model please do have a look. Also I will de sending you a graph in the second post of which type of graph I want to acheive.

After your suggestions I am able to remove the contact by removing the load in the second step. Also I am calculating the applied force to this plate in terms of giving displacement value. Is this correct. Please do let me know.

In this problem I am using the indentor as a rigid body.I wanted to ask that if i can give steel properties to this same indentor and remove rigid body, will that work. because that is what i want to acheive at the end. Steel indentor and Aluminium plate.

I thank you in advance and await your response


Best reagrds

 

[iyj]

here is the second attacment for the graph i am trying to ger.

Best reagrds

 

[rstupplebeen]

For your reference point you are translating it in the U2 direction for step 1 and then holding it there for step 2. Additionally in step 2 you translate the same point to 0 for U2. Instead just modify the displacement of the first constraint in step 2.

The force displacement methodology looks good. The indentor can be deformable.

I hope this helps.


Rob Stupplebeen

 

[rstupplebeen]

I just ran your model with the suggested change above. There is very large deformation of the mesh which is causing poor aspect ratios. I would reconsider the fixed constraint on the bottom face. My guess is that it can translate in the 1 direction. If these loads are accurate then you will need to use adaptive remeshing to get a valid solution. I hope this helps.

Rob Stupplebeen

 

[iyj]

Dear Rob

I thank you alot for the effort you're making for me. I have tried doing what you have suggested, but when i try to use adaptive remieshing rule, it does not let me do it and gives a message of (that orphan meshes cannot be changed) and it does not let me delete the mesh for some reason i dont know.

Also can you tell me which type of part i can use to model the indentor with. like if i use deforemable type part than how should i model it. i want to model this indentor with steel properties, so will i use the shell-homogenous properties. Please help

Best regards

 

[rstupplebeen]

You have an orphan mesh. Create the rectangle in CAE.

Deformable shell with steel properties.

I hope this helps.

Rob Stupplebeen

 

[iyj]

Dear Rob

Thanks alot, Yes I have created a new rectangle and modeled the indentor with the deformable shell with steel properties. All goes well, thanks to you. There is a single question that i need to ask you that is where will i apply the load on this indentor and how will i remove it.
As previously it was a reference point in the rigid body now in this case i applied in the middle of the indentor, but when i use the same location for the unloading and error comes. I have chosen end points of the indentor which does not make sense.

I have attached the new CAE file for you to look and if possible can you please identify where shall i apply and remove load on this indentor.

Really thanks man

Best regards

 

[rstupplebeen]

In the boundary condition "Applyload" for the second step return the indentor to 0 or even a little above the original position. "removeload" is not needed. The constraint at the bottom of the plate I still believe should just constrain in the U2 direction. I hope this helps.

Rob Stupplebeen

 

[rstupplebeen]

I would also apply the displacement to the entire top face of the indentor. Applying to a point usually if not always creates locally large deformations.

Rob Stupplebeen

 

[iyj]

Dear Rob

I couldnt thank you more. I have made changes according to your input. I have applied load to the top face of the indentor and also removed the second (remove load from the boundary condition). The analysis runs fine, but when i animate the indentor actully goes inside the plate and the deformations are not that are required really. I have attached the new CAE file for you to look at.
Please just run it and see the deformations. Also i have only constraint in U2 direction as you suggested.

Thanking you in advance

Best regards

 

[rstupplebeen]

I have looked at the model and here are my thoughts.
1. BOT should only be in the U2 not U2 and U3.
2. Try using second order elements for the plate.
3. Do you have an appropriate displacement? The deformation seems small but I am unfamiliar with the actual test.

I hope this helps.


Rob Stupplebeen

 

[iyj]

Dear Rob

Thanks alot for these gelpful tips. I have tried using your suggestions, but you know it is still overlapping and going inside the plate. I know you are right its to do with the type of element i have to choose. For the element bit as you suggested to use second order elements for plate. What i did i selected the element type and ticked the option of second order, is that the correct way of doing it or something else. please do advise.

I also have a question relating to impact of the indentor to the plate, in the same model that is attached with this post. Can you please tell me if i want to give velocity to the indentor and want to see how it impacts with the plate and rebounds, do i have to use Abaqus Explicit analysis for that. and where do i give the velocity, as i have to give around 2.5 m/s to the indentor.

Really grateful to you


Best regards

 

[fehrich]

Dear All,

I have a Impact/Contact problem too.

I impact a composite shell plate with an analytical rigid impactor. but instead of a smooth acceleration during impact, the graph shows an edgy oscillating curve. I use the general contact definition.

 

[fehrich]

Is there a way to apply a density and a stiffness to the rigid part?

Many thanks for your help

Fabian

 

[rstupplebeen]

CAE calls second order elements quadratic and can be accessed in the element type dialog.

For impact you will need to use explicit and provide the indentor with an initial velocity. This will be a much harder problem to solve and should probably be a new thread.


Fabian,
Sorry I do not have time to look at the models. This should be a new thread instead of adding on to iyj's. A rigid part has infinite stiffness.

I hope this helps.


Rob Stupplebeen

 

[iyj]

Dear Rob

Thanks alot. I will do as you suggested. I will start a new thread for the impact analysis and will let you know.

Best regards

 

[iyj]

Dear Rob

Just a quick question, I wanted to know if the units i am using are right, Please check my model and do let me know if I have inputted them rightly.

I am using the dimensions in meters

indentor Radius = 0.0828m
length of plate = 0.090m
Youngs Modulus E = 7.9 Gpa
Density = 1580 kg/m3 ( I have input it just like this)is this correct).
Yield Stress = 202 MPa
load applied in Boundary Condition is = 0.001093 m

so the resulting force and displacement is in Newtons and meters? Please do let me know.

Also can we give steel properties to the rigid indentor?

Thanks alot


Best regards



the resulting graph co

 

[rstupplebeen]

Attached is the units cheat sheet I use which I got from

http://www.PolymerFEM.com.

I believe that it was recommended on this forum at some point. I'm sure everyone on this forum has been tripped up by units at some point. I hope this helps.

Rob Stupplebeen