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

 

[iyj]

Dear Rob

Thanks alot, this was really helpful and made life alot easier. Thanks once again.

I have been tring the same problem again with complete sphere in 2D making contact with the rectangular plate. I have designed the sphere(indentor) rigid with steel properties, as u can see in the attached file. once i apply displacement it goes into the plate without making a deformation or permanent deformation. I even gave plastic properties to the plate material too. It worked with the rigid wire, but this is the actual problem, an di have seen in some of the papers they have done similar model.

I know you have suggested earlier that i need to use the second order element, itried but still it did not work, i dont know why,is it the interaction between both surfaces?

Please do check the model please do let me know where the problem lies as i have tried ven refining the mesh but it still goes inside the plate and not showing the deformation. if this is acheived than we can unload it too. Right now I am only trying loading case.

Thanks alot Rob

Best regards

 

[rstupplebeen]

Once you make the indentor rigid it is not steel anymore it is infinitely stiff allowing only RBM (rigid body motions).

I believe your lack of deformation is that your mesh is very large compared to your displacement. Your mesh is 2.5 and your displacement is 0.02.

Make sure that on your deformation plot that you do not have a scaling factor applied. That can be real confusing if you don't notice. Options>Common>Basic>Uniform 1

I hope this helps.

Rob Stupplebeen

 

[rstupplebeen]

You are currently modeling this as Plane Strain. So basically you are modeling a bar indentor instead of a sphere.

Rob Stupplebeen

 

[iyj]

Dear Rob

I thank you for yuor helpful advice. I am sorry i could not reply earlier it was due to holidays in this part of the word for national day.

I have tried using plane stress elements and also refine the mesh density and i can see some deformation but not complete only in the middle node and the the one below, you can see it too, i have attached the CAE file with this post. All i did was used plane stress and quadratic elemts in the plate and used linear for rigid indentor.

What seems to be the problem, do i have to make the mesh more coarse or is there a problem with the element defination.

I have modeled the sphere with deformabls shell and than make it rigid, is this the problem. please advice.


Best regards

 

[rstupplebeen]

Plane stress elements are for sheet metal like parts such as a car hood or airplane wing. You need to use axisymmetric models for geometries that could be turned on a lathe. So if you want a 2D model of a spherical indentor then you need to model this as axisymmetric.

Only draw the +X half of your model and convert to axisymmetric for the part instances and the element types.

I hope this helps.


Rob Stupplebeen

 

[iyj]

Dear Rob

I thank you for the suggestions. I have tried the way you have suggested and have designed the model as axisymmetric and used axisymmetric elements too. The analyis runs fine and is successful but i get this message when it comes to see the results.

"Results for current deformed variable are not available for one or more nodes constrained in the model.Deformation of such nodes are assumed to be zero"

I dont know why this message appears. Any suggestions on that. I have attached the new model please do have a look if I am somewhere wrong than please do guide me.


Thanking you in advance

Best regards

 

[rstupplebeen]

Reduce your initial step size. Basically for a nonlinear analysis a single step is never appropriate.

Mesh:
Try changing your plate's mesh to sweep instead of structured.

Boundary conditions:
The fixed constraints are still probably not appropriate. Review my previous posts.

I hope this helps.

Rob Stupplebeen

 

[iyj]

Dear Rob

I have tried the model with your suggestions. But it is still giving me the same error.

"Results for current deformed variable are not available for one or more nodes constrained in the model.Deformation of such nodes are assumed to be zero"

Is it to do with the constraint that i have used i wonder. As I have modeled the sphere with rigid body. I am confused and cannot seem to find the problem. I have attached the model with the changes you suggested. I am really grateful to your effort in this regard.


Best regards

 

[iyj]

Dear Rob

I hope you are fine and in best of health. Actually i wanted to update on my progress. I have got rid of the error that was appearing agaian and again, the one mention in the last posts. Thanks to you really.

Now that i can see the results, i cannot see deformation, instead the sphere is sliding on the plate and not bending or deforming the plate. Please do let me know why is that happening now. I have fixed the left edges of both sphere and plate and still the sphere moves in the opposite direction, i dont seem to figure out how and why. please see the attached CAE file.

Please do guide me on this

Thanks alot really

Best regards

 

[rstupplebeen]

I am not sure where you model is going wrong without really digging into the details so I made a test case. I hope this helps.

Rob Stupplebeen

 

[rstupplebeen]

Now attached.

Rob Stupplebeen

 

[iyj]

Dear Rob

Thanking you will be a under statement. I think you just have saved my job and i am really grateful to you, for the effort you have made for me. It really works they case you did and that was exactly what i was looking for.

Now I can move to Impact of these two parts and as you suggested i have to use dynamic explicit steps for that and have to give velocity to the ball.

Once again Rob you are a saviour and a good teacher to me. Now I will start the impact problem and as you suggested will make another thread for it too.

I will let you know about the new thread once i have started the problem.

Best reagrds

 

[rstupplebeen]

I'm glad I could help and you are very welcome. Thank you for your kind words. Good luck with the explicit analysis.

Rob Stupplebeen

 

[iyj]

Dear Rob

I hope you are fine. I just wanted to know that the dimensions you used for this example, are they in meters or millimeters. I checked the radius of the indentor its 0.5 so is it in meters or millimeters?

As the corresponding force -time graph and displacement graph that i draw i am gettin a bit confused, I remember you sending me the reference list to follow, but if you could tell me the initial units it will be easier to follow.

Thanking you in advance


Best regards

 

[rstupplebeen]

I just put in arbitrary values for geometry, materials, and displacements. You should be able to go back into the model and change them to your values with little effort. Modify the: sketches, material property, displacement and remesh. I hope this helps.

Rob Stupplebeen

 

[iyj]

Dear ROB

I hope you will be fine and in best of health. Long time no contact as i was abroad and now back to work.

After your helpful guidance i was able to make the model to work according to my specification. Now if i want to run the same thing like still a static case but in 3D, will the procedure be same. And all i have to do is to model both objects with 3D elements and use the same technique as the one you used. please do let me know.

Thanking you in advance

Best regards

 

[rstupplebeen]

I believe so. It will take a lot longer to solve though. Pay attention to constraining the additional degrees of freedom.

Rob Stupplebeen

 

[iyj]

Dear Rob

I hope you are fine and in best of health. I have started working on impact analysis and staright away some questions. I am using the same geometry that i used for contact analysis, the axisymmetric model using axisymetric elements. Now what I am doing is that I have changed the analysis to dynamic explicit and instead of displacement i have given a initial velocity with the poin mass to the analytical rigid part.

It works fine but But i want to see the impactor to impact the thick plate and than bounce normally as it happens in the real time.

Do I assign gravity to the impactor or whats the slotion. I want to see the force Vs indentation of this impact.

I know you said I have to use different thread. I will make a new thread and post this on that too.

Please help

Best regards

 

[iyj]

Dear Rob

Just a quick question, I am using this same contact analysis using elastic plastic material of the plate. the forces seems to be too hight as compared to the analytical solution and thats not right. I may be giving the wrong plasticity module from the material list. The Yiled stress is 202E6 MPa and i normally give the plastic strain a value of zero. please guide me on this. As the elastic case compared well and but this ealstic-plastic case there must be something wrong that i am inputting. please have a look at the attached cae file.


thanking you in advance

Best regards

 

[rstupplebeen]

I usually leave the plastic strain blank if I am just using yield stress.

I believe that you may have a units issue. Is your model in mm? If so pressures should be in MPa (modulus, yield stress). I hope this helps.

Rob Stupplebeen