Explicit dynamics ERRORS

  • Last Post 10 hours ago
FernandoTorres posted this 2 weeks ago

I am trying to solve a 2d plane strain explicit dynamic analysis of material cutting (chip forming). I have densed the mesh near the cutting edges. The problem I am facing is that whenever I "solve" the system it says solver error see log files for more details. I have deleted the contact manually as it was saying bounded contacts are not valid in 2d explicit dynamic analysis so I deleted the contact manually. How to solve this problem? Thanyou

Order By: Standard | Newest | Votes
peteroznewman posted this 2 weeks ago

Two quick things to change:

1) Reduce the end time to a much smaller value, like 0.001 s

2) Under Output Controls, Increase the Number of Result Points from 20 to 200.

Attach a project archive to your reply for more help.

FernandoTorres posted this 2 weeks ago

Sir recently emailed you with the file. Kindly Check out please. Thanks

peteroznewman posted this 2 weeks ago

I got your email with the .wbpj file attached.  The reason you were having difficulty attaching that file to this discussion is because that file on its own is useless. The folder of the same name_files is required to open the project.  Some people zip that folder and file together into a zip file, which is allowed to attach here.

However, a better solution is to use the ANSYS Project Archive feature to create a .wbpz file that does this for you.  Read this for more info and try to attach your .wbpz file to your reply.

FernandoTorres posted this 2 weeks ago

I'm sorry , nevertheless 


Attached Files

peteroznewman posted this 2 weeks ago

One trick that allows for quicker testing of the effects of boundary conditions, materials and so on is to scale up the geometry by a factor of 1000 so that the simulation runs in 30 minutes instead of 500 hours.  I did that with this model to get something you can look at.


Attached Files

FernandoTorres posted this 1 weeks ago

Thanks Sir peter!

As far as we are concerned we want our teeth to remove the workpiece's material not to wear itself. The video is showing the wearing of the teeth, upper most mesh layer of teeth going inside the workpiece while no material is being removed from the workpiece. Which is a great headache. Now how to make such model in which, teeth doesn't gets into the workpiece and doesn't wear itself out rather makes the workpiece to wear out and material is removed in the form of chips?

Screenshot is attached in which some "patches" of tool are inside the workpiece and they are travelling inside without cutting and some "patches" on tool has been worn out. How to nullify both the conditions. Thanks a lot

peteroznewman posted this 1 weeks ago

Let's look at the materials you provided: 


Note that the stiffness of the specimen is five times higher than the broach. When those two materials push on each other, the broach is going to deform five times more than the specimen. In other words, the strain is going to be much higher on the broach when it pushes on the specimen.

Now look at the Erosion definition you provided:

The element will erode when the geometric strain exceeds 1.5.

The solution output is consistent with the model inputs, the more flexible material is eroding away. That makes perfect sense to me. If you want a different output, provide a different input.  : )

As to the elements of the broach that are "inside" the specimen, use a smaller element size and this problem will be resolved.

FernandoTorres posted this 1 weeks ago

Yes Sir you are right. It was in my mind while giving the material values but I thought 'density' may play its part there. Anyhow, I'm going to recheck the material data. But I am totally blank about Erosion controls. I have googled it but I still don't know how to 'fill up' the erosion control box. To be honest. I didn't even opened the erosion control box and let the system decide. May you please explain this. Thanks

peteroznewman posted this 5 days ago

Most of the materials in the Explicit Materials library in Engineering Data come with Material Failure definitions. When one of those materials is chosen, the Erosion Controls would set No for On Geometric Strain Limit and set Yes for On Material Failure.

Alternatively, you can add material failure conditions to a newly defined material.

peteroznewman posted this 4 days ago


Here is the link to your model that behaves differently to the one I uploaded. That archive included results so was 145 MB and beyond the size allowed for using the Attach button here.  You can either post a Google Drive link such as I did in order to include the results, or you can Clear Generated Data on the Model or Mesh item, which will clear the solution also. That archive file size will be the smallest possible.

If you study my model carefully, you will see that my displacement BC is only on the bottom edge of the tool, which allows the rest of the tool body to be flexible.

Your model applies two displacement BCs to the entire tool body, which prevents the tool body from deforming in any way, so no strain develops and no elements fail. This is equivalent to making the tool body rigid, only a lot less computationally efficient.  This explains why my model erodes on the tool body and your model doesn't. Is this what you want?

I don't understand why you are paying attention to the stress in the specimen. You are cutting it. That means you are taking the stress in the material to a point at which failure occurs. The current definition of failure is when strain > 1.5 and since stress = E times strain, and you provided the value of E as 2822 MPa, you can calculate the stress at failure as 4,233 MPa.   So what? Why do you care?

FernandoTorres posted this yesterday

Thanks sir ! But I am confused about 1. 'contacts' why are we supressing it ? 2. When I update the element size of mesh, tool's body seems to have gone into the workpiece's body (i.e. it doesn't keep distinctness between two bodies rather it seems to be merged with the workpiece body.

The file you have sended me is perfect , but i am trying to build my own file. Thanks

peteroznewman posted this yesterday

In Explicit Dynamics, the Body Interaction works at the element level to check contact.  Contact elements only work at the original surface they were created on, which is eroding away.

There is a defect in the meshing software that connects the mesh across two parts that don't share topology. Go into CAD and make a tiny gap between the vertex of one part and the edge of the other part.

Much respect to you for wanting to build these models from scratch. I'm glad to provide the "answer key".

FernandoTorres posted this yesterday

Thanks sir for your patience for this weak student.

I've completed the model, but in my model tool is going inside the workpiece, unlike in your model. May you please help me. I want two things here

1. I don't want to take my tool inside specimen ( see the picture attached) rather i want cutting (like your file, you sended me)

2. I don't want the elements of the tool to travel inside the specimen without cutting anything.



peteroznewman posted this yesterday

Please provide an archive that has a small gap between the tool point and the specimen to overcome the defect in the meshing algorithm. I think the solver is getting confused and can't tell that there are two separate parts.

FernandoTorres posted this yesterday

Sir, I've sent you an email.

peteroznewman posted this 10 hours ago

I looked at your model and made some observations.

1) You want an Axisymmetric model where 2D geometry is rotated about the Y-axis.  Your 2D geometry is for rotation about the X-axis so it not useful for an Axisymmetric model.  Reorient your radial cross section so that the rotation axis is the Y-axis. I changed your model to Plane Strain to do some preliminary work on it.

2) Your broach material has a Young's Modulus of 210 MPa, the same as your workpiece. Steel has a Young's Modulus of 200000 MPa. Are you confusing Strength with Modulus? I changed the broach to have the same Young's Modulus as steel.

Please reply with new geometry.