Explicit dynamics ERRORS

  • Topic Is Locked
  • Last Post 2 days ago
  • Topic Is Solved
FernandoTorres posted this 13 May 2018

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

  • Liked by
  • Tabrez
Order By: Standard | Newest | Votes
peteroznewman posted this 13 May 2018

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 14 May 2018

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

peteroznewman posted this 14 May 2018

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 15 May 2018

I'm sorry , nevertheless 


Attached Files

peteroznewman posted this 15 May 2018

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 17 May 2018

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 17 May 2018

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 17 May 2018

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 19 May 2018

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 20 May 2018


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 23 May 2018

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 23 May 2018

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 23 May 2018

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 23 May 2018

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 24 May 2018

Sir, I've sent you an email.

peteroznewman posted this 24 May 2018

I looked at your model and made some observations.

1) You want an Axisymmetric model where 2D geometry is revolved 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.

FernandoTorres posted this 25 May 2018

Sir I inboxed you on gmail.

peteroznewman posted this 25 May 2018

I already ran your model as Plane Strain with the workpiece set to your specification of Young's Modulus at 210 MPa. This is 338 times more flexible than aluminium (71000 MPa), which you now tell me is the material of the workpiece. It's no coincidence that 210 MPa is the ultimate tensile strength of a particular type of aluminum.  If you don't understand the difference between Strength and Young's Modulus, you need to learn that before you work on a model of the complexity shown below.


This video shows that you need small elements to form chips from the workpiece.  I put the small elements along what I thought was the cutting plane, but due to the extremely flexible modulus, the workpiece deformed away and the tool point was pressing on larger elements and began to pass through rather than cut.  The best practice is to have a very uniform element size, which I did not in this video.

Explicit Dynamics Body Interactions will automatically take care of all the contacts.

Reread 1) in my last post.  Your ppt file shows the axis is along the Y-axis in SpaceClaim, but the 2D geometry you provided in the workbench archive still has the axis aligned with the x-axis.  Please provide new 2D geometry with the axis on the Y-axis. The displacement of the tool will be along the Y-axis.

Look at the materials in the attached archive that was used to make the above video. You see that I have added Plasticity in the form of Bilinear Isotropic Hardening and Principal Strain Failure. You don't have any plasticity or failure theory in the Aluminum in your archive.

What do you know about the properties of the aluminum of the workpiece? There are many types of aluminum, you need to provide detailed mechanical properties. You should obtain an actual stress-strain curve for an aluminum, then you can get the plasticity closer to reality.

Attached Files

peteroznewman posted this 25 May 2018

Here is the animation with the workpiece as aluminum.

FernandoTorres posted this 26 May 2018

Sir I accept my mistake, I was just using hit n trial method for material properties. Now I have exact values from experiment. Should I put them directly or change them to true stress and true strain before pluging in for plasticity ? Can I couple this broaching process to transient thermal if I know the heat condution and specific heat values of broach and workpiece. Actually I want to check out broach's surface temperature just after cutting. Thanks

peteroznewman posted this 26 May 2018

Do you have Engineering Stress vs Engineering Strain data from a tensile test in an Instron-type machine? Did it use an extensometer to record the displacement of a gauge length on the test sample?

Then yes, you convert that to True Stress and True Strain and break out the Elastic and Plastic Strains in order to create a Multilinear Plasticity model. I used that in Static Structural.  Not all material models work in Explicit For example, Bilinear Kinematic Hardening won't run in Explicit, only Bilnear Isotropic Hardening will run.

I believe Explicit can include thermal properties during the solution, though I have not used these capabilities myself. You need to spend a lot of time researching what is available in ANSYS and how you populate the data needed to use the feature. 

FernandoTorres posted this 27 May 2018

How to add rockwell hardness c value to material properties?

peteroznewman posted this 27 May 2018

Rockwell hardness is not a property that is used in any material models I know of.

There is a relationship between Rockwell hardness and yield strength, so if you convert it to yield strength, then you can use the information that way.

FernandoTorres posted this 27 May 2018

Sir inboxed you on gmail. Kindly checkout

peteroznewman posted this 27 May 2018

I see you have geometry along the Y-axis, so now you can perform an axisymmetric 2D model. This will include hoop stress that was not in the 2D plane strain analysis done previously.

You need to do research on plasticity models that include a thermal effect. Remember what I suggested in January? I mentioned the Johnson-Cook (JC) Strength material model. What have you learned about that?

FernandoTorres posted this 27 May 2018

Sir to be honest I downloaded many research papers and seen many videos related to it but I didn't get it. It was having too much variables now where to get all these values from ?

peteroznewman posted this 27 May 2018

Please attach a zip file of a few of the better research papers on JC. 

Did you read the ANSYS Help file? 


It says JC material model requires an Equation of State model. Here is one for Aluminum.

B.2.24. Null Material Gruneisen EOS Example: Aluminum

MP,ex,1,100e9 ! Pa

MP,nuxy,1,.34 ! No units

MP,dens,1,2500 ! kg/m3


TBDATA,1,-10000 ! Pressure cut-off (Pa)

TBDATA,3,2.0 ! Relative volume in tension

TBDATA,4,.5 ! Relative volume in compression

TBDATA,16,.5386 ! C

TBDATA,17,1.339 ! S1

TBDATA,18,0.0 ! S2

TBDATA,19,0.0 ! S3

TBDATA,20,1.97 ! γ0

TBDATA,21,.48 ! A


FernandoTorres posted this 09 June 2018

Sir emailed you. Thanks

peteroznewman posted this 10 June 2018

Fernando asks:

Sent you a DEFEATURED BROACH geometry. Concern is about the stress distribution across and inside gullet radii so I defeatured the teeth. Please answer:

1. Is it ok to simplify it as I'm not concerned about the teeth in my static analysis?

2. Which mesh technique should I use to solve this? I've once selected proximity and curvature but it ends up with very large set of nodes and elements as I have to do MESH REFINEMENT STUDY too.

3. I've gone through your article about "how much refinement should I do " but I didn't understand that as some CFD terms were there. May you please explain that how much should I refine this model.  


1. Yes, if you're not concerned about the teeth, you can simplify.

2. Once you simplify the teeth, the geometry becomes axisymmetric. That means you can have a 2D mesh instead of a 3D mesh and you can use a very fine mesh without creating a very large number of nodes.

3. In the axisymmetric model, you can easily plot the maximum stress vs. element edge size and you will see when the points form a nice trendline toward a zero element edge size.

  • Liked by
  • FernandoTorres
Tabrez posted this 2 days ago

SIr, i am also doing explicit dynamics for doing simulation of turning operations. I am unable to get chip formation. Would you please send me your file for chip formation? I will be thankful to you.

Show More Posts

Topic Is Locked