Learning Forum

[inouzil]

Greetings,

I would greatly appreciate your support in understanding the problem with my simulation. I am trying to simulate 2D orthogonal machining of Ti-6Al-4v with Johnson cook plasticity and Johnson Cook Damage Model. Material cutting takes places , however there is no chip formation and my objective is to study the temperature distribution in both chip and tool. 

I have read through the previous discussions and accordingly tried all trouble shoot methods (as per my understanding). Below is the image of my boundary conditions and results: 

I have tried with smaller mesh size but no chip formation. I have attached the file without results for your review. Would greatly your response and apologies if the answer is already present in another discussion. I went through and tried all different discussions on the topic but couldn't figure it out. 

Secondly, I have seen studies were people say they conduct 2D studies at different feed rates (mm/rev). How do we simulate the effect of different feed rates in 2D? Softwares like AdvantEdge, which is specially built for machining, also has an option for setting different feed rates in 2D. However, I am unable to physical understand the meaning of this or how to simulate this in 2D. 

My ansys version is 17.2 with a research license. 

Gratitude for the support.

Regards

Ibrahim Nouzil

[inouzil]

Hi everyone,

Would greatly appreciate some support. 

Looking forward to a positive response.

Regards

Ibrahim Nouzil

[inouzil]

Hi.. Still awaiting some response from the Ansys community. 

I get the chip formation when I use Ansys library explicit material (Al-1100). However, no chip formation when using Titanium, also from the library. Why is this happening?

Further, as explained in my first post, Johnson Cook Model with Johnson Cook Failure also does not give chip formation (cutting takes places without chip formation).

Reading into some forums led me to try assigning Euler domain for the chip. However, I am unable to do that. I am doing a 2D explcit dynamics simulation and there is no option to set Euler reference frame. Additionally, Ansys 17 user guide says euler domain options not available in 2D. Does this mean I cannot simulate a chip formation for Titanium in Ansys explicit dynamics?

I would greatly appreciate an Answer to this question. 

For Aluminum 1100 2d cuttting simulation, I have chosen 'output contact forces' in the analysis. How do I see the results? Ansys version is 17.2. 

Looking forward to some response. 

Regards

Ibrahim Nouzil

[Wenlong]

Hi Ibrahim,

I am not an expert in chip formation simulation but I will attempt to provide some of my thoughts:

In Ansys Explicit Dynamics, the highly distorted or elements that satisfy failure criterion are eroded (deleted), and the eroded nodes are represented as red dots, as shown in your image. So your question boils down to why these elements that are supposed to be chipped get highly distorted or met the failure criterion? 

When an element gets highly distorted, it usually means the force acting on it makes it have extreme deformation. It can either mean the force is too large or the element is too soft. I would check if reducing the velocity of the cutter to see if it improves. I know this would change your boundary condition but maybe this can give you some ideas of the cause of the problem. Also, you mentioned you are able to see the chip formation using Titanium material other than Aluminum1100, I checked the yield strength of these two materials in the library, it is 500MPa(Titanium) vs. 40MPa, so this may give another glue that maybe the Aluminum material model cannot withhold the impact energy and reached the failure criterion defined by Johnson-Cook material too soon, or it simply has too much deformation. 

As for the Eulerian domain, I am not sure about version 17, but at least in later versions (I am using 2020R1), I am able to use the Euler domain in 2D.

 

Regards,

Wenlong Zhang 

[inouzil]

Thank you Mr. Zhang for your reply. Much appreciated. 

I have a few updates since I last posted my problem. First, a clarification, my simulation works for Al-1100. It does not work for Titanium. Apologies if there was any confusion earlier. 

Above is the AL1100 simulation image. The chip formation takes place. Below are the images from the Titanium Simulations. Earlier pictures posted are wrong. The default strain rate correction (first order) in the Johnson Cook model was active and therefore the material deformation was very large. However, after correction these below images are the current status:

Cutting takes place initially and then the tool starts to move inside the workpiece mesh. Why is this happening? some reading led me to believe it could be because of the mesh size. It already takes around 8 hours to solve. Is there any general strategy for contacting bodies that I must follow?

Further, regarding Eulerian reference frame, I have read online that ALE helps in chip formation and generally most studies in abaqus set chip as eulerian reference. Unfortunately I am unable to do this. The option to set the reference frame is missing in my model as shown below. Am i doing something wrong? Also attached is an image from Ansys 17 explicit dynamics user guide.

Further, in the Aluminum simulation, the temperature distribution in the tool is not shown? I inserted temperature from the worksheet after the solution was generated. Is there any other way to do it. 

I greatly appreciate your support Mr. Zhang. Thank you for enabling this discussion. 

Looking forward to your reply. Much gratitude and thanks.

Regards

Ibrahim Nouzil

[Wenlong]

Hi Ibrahim,

Apologies for my misunderstanding about the Eulerian domain in 2D (and thanks for teaching me this fact ). You are right, I just checked the document that even in the newer version these Eulerian domain controls are not available for 2D. (Sorry I got a wrong impression by looking at the Mechanical interface and saw the Eulerian domain in "Analysis Settings", shown below)

This may not apply to your case, but would it be possible if you can make it 3D by creating a small thickness, then only assign one layer of elements in the thickness direction, and constrain all the elements' z-DOF (It's like make it a plane-strain equivalent scenario)? By creating a 3D model with plane strain settings and only one layer of elements, you can still use your formulation in 2D and not significantly increase the number of nodes.

About the contact problem, I guess you are using trajectory-based contact detection in body interaction? You can find a description of the method if you search "body interactions in explicit dynamics analyses" (attached below, if you have trouble viewing the image, you can refer to the tip in this post:/forum/forums/topic/retrieving-full-resolution-images-from-posts/). I would try reducing the time step size to see if it helps. My feeling is that it may miss a contact due to too high of velocity or something, then all the elements behind it will miss because these elements have not formed an open surface yet. I would also try making the mesh size in two bodies relatively similar to improve accuracy. Moreover, since you are still in the debugging process, I would suggest not use that fine mesh to reduce the pain of waiting.

About the Johnson-Cook material model, I wish I have more insights but I am not familiar with that material model. However, the fact that your Aluminum model is working gives a big hope. Maybe if you continue tweaking with the material parameters it can work for the Titanium too, or at least find out the root cause of the problem.

Regards,

Wenlong

[inouzil]

Mr. Zhang,

I was trying out the different suggestions made by you and below are the results:

1) I tried with a lower velocity but the result was same. The tool mesh penetrated into the work piece after sometime and it stopped the cutting.

2) I tried with smaller time steps. I did this by reducing the time step safety factor. Still the same result. I have attached a video for the same with 0.7 safety factor and 1m/s velocity.

3) In the 3D model, when I set the chip to Euler Domain, I can no longer apply any boundary conditions to it. Since, we need to constrain all Z DOFs, I tired to apply a displacement condition on the face but I couldn't. Would the model be still valid as a 2D plain strain model if I am unable to constrain Z DOF? In abaqus (I only have the student version), it allows ALE meshing and constraints on a Euler domain. 

I would greatly appreciate your input. I have to make a decision on what FEM tools must I use going forward and do not want to exhaust resources on other licenses if I am able to generate required results using our existing ANSYS license. 

Looking forward to your response.

Regards

Ibrahim Nouzil

[Wenlong]

Hi Ibrahim,

For the penetration issue, have you implemented a smaller mesh on the rigid cutter side? Make the two bodies' mesh size similar may improve contact detection. Another thing you can check is mass scaling, make sure the added mass is not very large.

For the Euler domain in 3D, you can try changing the Euler domain boundary condition from "Impedance" to "Rigid" to prevent the movement in the thickness direction. However, whether this behaves exactly the same as plane strain needs to be proved. 

Another powerful Explicit Solver is Ansys LS-DYNA if you are interested, 

Regards,

Wenlong

 

 

[inouzil]

Mr. Zhang,

Thank you for your reply. Apologies for the very late response. Current events required lot of changes and took time to reorganize everything. I hope you are doing well in these times. Take care.

 I have some updates on the simulation problem. First, In the latest ANSYS 2019 R2 I am able to successfully run the model. I used the following suggestions made by you

1. Reduced the cutting velocity to 1.25m/s. My initial condition was for 2.5m/s. 

2. Time step safety factor was set as 0.7

3. I set the tool as rigid. 

4. used same edge sizing of 4e-5m on both cutter and chip. 

above images show the mesh and total deformation with temperature. 

However, when I increase the velocity of 2.5m/s, I again face the same problem. Very fine mesh leads to tool moving inside the workpiece (no cutting) and a coarser mesh gives no chip formation. how can I tackle this? Ansys 17 is unable to solve the model successfully for the low velocity condition. why is that? could it be that the latest version has better contact detection?

I have another query. In the above image with temperature distribution, why cant I see the temperature developed in the tool? I inserted the temperature result from the worksheet and chose all bodies. Still I am unable to see any result. Could you please help me out with this. 

I don't have ANSYS LS DYNA license. 

 

Gratitude for the support. Looking forward to your response. 

Regards

Ibrahim Nouzil

[Wenlong]

Hi Ibrahim,

Greetings! I was just thinking about you when I came across this post: /forum/forums/topic/time-step-is-too-small-error/

Please take a look at let me know if that's helpful.

Regards,

Wenlong

 

 

[Wenlong]

Hi Ibrahim,

About the temperature distribution in Explicit Dynamics, if you want to see the temperature distribution on the tool, please try changing it to flexible and see if it works. 

Regards,

Wenlong

 

[inouzil]

Greetings,

I have tried already with flexible condition and the result is still the same. No temperature distribution on the tool is shown.

Regards

Ibrahim Nouzil

[inouzil]

Thank you. I am reading through it. Will try some suggestion made by Peter. 

Regards

Ibrahim Nouzil

[inouzil]

Mr. Zhang, I hope you are well. I was working in abaqus for a short while and so was not into ANSYS much. However situation is once again changed and I am dependent on ANSYS again. I am facing two problems:n temperature distribution in the tool even when set the stiffness behavior as flexible (material properties defined for the tungston material is attached). But when I use the explicit library Tungston alloy material I get the temp distribution. But the material definition is not what I want. So when I change the property values of the library material, I still dont get the temperature distribution. What is happening. Kindly assist.nI was trying the 3D method as you suggested. To set 1 element thickness in the z direction. I was trying to set the Euler domain. But i get the error stating l The Euler domain does not contain any material. Check that the Virtual Euler bodies lie within the Euler domain or for any truncation of the Euler domain caused by Global Symmetry planes. What does this mean: I have attached below the image of the setup:nnn