Compression molding of molten plastic

  • Last Post yesterday
  • Topic Is Solved
RosarioAnsys posted this 22 March 2018

Hello to all,
I must realize for the school a study on the behavior of a material with crushing.

In fact, I have a material that is Polyethylene that has just been crushed between two standard steel blocks:


The crush material is 180 degrees, and I do not know how to handle the fact that the material is 180 degrees.

I am currently using the module static structure, I have a fixed support on the lower block and a displacement on the upper block (displacement of 32mm), my material is a cylinder of ø36 with a thickness of 2mm.

That's what I'm getting for now:

And here is what I have in terms of my material values:

I have the impression that my material is not 180 degrees and suddenly I do not get the desired result because normally the material should be completely erase, I do not know how to tell Ansys to manage the material to this temperature.

I thank you for your future help and sorry for my english

Order By: Standard | Newest | Votes
peteroznewman posted this 22 March 2018

Hello Rosario,

Low Density Polyethylene, LDPE, melts at 110 °C (230 °F). When you say 180 degrees, I assume you mean Fahrenheit otherwise the part would have melted.

You need the properties of the material for the temperature you are testing at. These can be measured using a properly shaped test sample of the material in a controlled environment tensile testing machine.  Here is a paper with some data. Figure 3 has the data needed to estimate material properties at 80 °C, which is close to 82 °C (180 °F). You could create a multilinear plasticity material model.

Are the steel blocks also at 180 °F? If not, then they will rapidly cool the PE they come in contact with and that would imply the need for a transient thermal analysis coupled with the structural analysis.

How fast do the steel blocks move? Because of its viscoelastic nature, the response of PE pipes to loading is time-dependent. The effective modulus of elasticity is significantly reduced by the duration of the loading because of the creep and stress relaxation characteristics of PE. On the other hand, the effective modulus of elasticity is significantly increased if the loading is very rapid. You can add a viscoelastic property to the material in ANSYS. 

Did the crushing machine have a force sensor to record force-displacement data while the pipe was being crushed?  If you have that data, you can adjust your material parameters until your model agrees with the experimental data.

  • Liked by
  • RosarioAnsys
RosarioAnsys posted this 22 March 2018

Thank you for your reply.

I think I misspoke, my material is high density polyethylene.

The material is at a temperature of 170/180 ° C, it comes out of a heating machine at this temperature and just be crushed between the two blocks of steel at room temperature (23 ° C).

Indeed, there is thermal simulation that I will perform once my material crush, but I block at the first stage.

The closing speed of the mold is 0.1m / s, and indeed it is a value that I forgot to take into account and currently I do not know how to enter this value in Ansys.

I really thought that Ansys was able to give the characteristics of the materials according to the temperature of the material.

On this link, there is a pdf that shows more or less what I want to do, only I try to put it into practice on blocks of unmachined steels as in the photos of my previous post and then applied my overwriting complex blocks like on pdf documentation:




peteroznewman posted this 23 March 2018

Thank you for the clarification and the article. 

The heating machine is to melt the material which comes out of an extrusion die and onto the blocks. I suggest you edit the title of this discussion to "Compression molding of molten plastic" so that members will get the right idea. Also, use the word "molding" rather than "crushing" to clarify that the material if flowing and not fracturing.

Do you have a full Research license of ANSYS or only a Student license?  The article describes using ANSYS Polyflow which is not included in the Student license. If you don't have a Research license, then perhaps AIM could be used.  I don't know that you can do what you want with AIM but it has several systems that seem relevant and can be linked.

I am also disappointed in the limited predefined materials that come with ANSYS. You are expected to create your own materials with the extensive tools that are available.



  • Liked by
  • RosarioAnsys
peteroznewman posted this 23 March 2018

Look at Figure 6 in the paper you cited and you will see that the shape of the material used in their model of cooling is shown in b) and is a flat solid, not a hollow tube.

RosarioAnsys posted this 23 March 2018

Thank you for your return and you are right, I had a bad understanding of the subject.

I have a full Ansys license.

This weekend I will put in place the changes you made me and I'll get back to you as I advanced in the modification of my 3d and performed a simulation on Ansys

Basically, I must get the same results of the study on the crushing part of matter, for the moment the thermal part and the dissipation of heat does not interest me.


Thank you and see you soon

RosarioAnsys posted this 26 March 2018



I made the necessary changes:

First of all I now have a "plate" of HDPE at 170 ° C that has just been crushed between two blocks having profile.

The goal is to give the shape of the imprint to my HDPE:

I am still using the module static structure, with the data below that I was able to retrieve on the internet:

Currently, to realize my simulation, I have a fixed support on the lower part of one of my blocks and a displacement on the other of 8mm, so that the two blocks come into contact.

When I run the resolution an error occurs:

"An internal solution magnitude limit was exceeded. (Node Number 2556, Body Profil Bas\PartBody/Pocket.13, DOF UZ) Please check your Environment for inappropriate load values or insufficient supports.  You may select the offending object and/or geometry via RMB on this warning in the Messages window.  Please see the Troubleshooting section of the Help System for more information."

I do not know if this problem comes from my simulation, the completeness of my room, a bad setting.




peteroznewman posted this 26 March 2018

Hello Rosario,

I assume you have contact defined between the bottom face of the HDPE and the imprint faces of the bottom block and contact on the top face of the HDPE and the imprint faces of the top block.

Contact can be difficult to use successfully. In a Static Stuctural model, a body can "pass through" another body before the contact algorithm had a chance to start pushing back. There are several ways to get to success. The first one is to insert the Contact Tool into the Connections folder and obtain the Initial Contact Status. If you find that the HDPE has a small gap to the imprint faces of the bottom block, there is a setting in the contact definition called Adjust to Touch. That will make sure that some contact elements are initially "closed" so that the contact algorithm has something to start with.

I would also move the top block down until it is touching the HDPE also. You want contact established on both sides of the material before the displacement starts.

Another method to be successful with contact is to change Auto Time Stepping from Program Controlled to Manual. Then you can bring the top block down in very small increments that allow the contact to evolve. If the displacement occurs in large increments or all-at-once, then the penetration is too great and the contact algorithm cannot resolve the penetration.

You show a material that has only elastic properties. That means when you squeeze it with the imprint faces, you will see it deform into some shape, but then when you retract the top block, the material will return to a flat rectangle because it is elastic! 

You could add plasticity to your material model. At a minimum, you need one more material property, and that is yield strength. I have used plasticity to model the ductility of metals.

You could also add a viscoelastic material property. I haven't used that before, but would be curious to see it used.

If you attach a .wbpz project archive to your reply, I can take a closer look

  • Liked by
  • RosarioAnsys
RosarioAnsys posted this 27 March 2018


I thank you for your return, I made the changes and indeed the simulation works when I have a contact on each side of the material.

Unfortunately the results are not really realistic, but I applied the data to my material:

But here is the result:

I have the impression that HDPE is entering the lower and upper blocks when it should not.

I do not know where the problem can come from.

I have a duration of 1 second but I would like to do the same thing for 10 seconds, I have to use the transient structure module no?

I have attached the study as you requested.

I thank you again for your help


Attached Files

peteroznewman posted this 28 March 2018

Hello Rosario,

You must turn Large Deflection On. That is why it appears the material is entering the blocks. That change will make the solver take a lot more iterations, so you will wait longer.


That change will also make the solver want to take smaller steps, so you can change Auto Time Stepping to On and suggest Initial Substeps to 10.

You should change the Contact from Bonded to Frictional. You should add all the curved surfaces below the flat surface on the blocks. As the plastic is pushed down, it will eventually make contact with the curved surface, so you want that in the definition.

You want more elements through the thickness of the HDPE to let it easily conform to the shape without excessive element distortion.

Get ready for some difficulties getting the solver to converge. Here is an example with the changes I put in above.

The solver took 53 iterations before I hit Interrupt. The model converged 30% of the way to the full displacement of 0.3 mm so it only can show 0.09 mm of closure. Corrective action in the model is required to get it to go further. Why is the solver having difficulties finding the next equilibrium solution?  You need to look at the Newton-Raphson Residual plots to see where the largest force imbalance is in the model. Sometimes more elements near there can help. But to see the plots, you have to turn them on by typing how many you want saved. I typed 6.


After Interrupting Solution, you can look at a NR Residual plot. In this case, every one of the 6 plots had the Maximum Residual occur on either the top of bottom block, and since the mesh is so coarse, I expect a finer mesh is going to help the solver to converge.

Adding a lot of elements to the blocks is going to increase the wait time on the solver. One way to reduce that time is to change the blocks from flexible to rigid behavior. Then only the surfaces that push on the HDPE have to be meshed. If the deformation of the blocks is negligible, then this will save you a lot of time. 

After increasing the mesh density on the blocks and changing them to rigid bodies (a few other edits go along with that), the solver now converges to 50% of the displacement of 0.3 mm but fails to converge. The NR plots only show the Pad now since the Blocks don't need to converge. And so it goes. The gap between the blocks seems to be 1.3 mm, so was 0.3 mm just a trial?

Another way to reduce the time spent waiting for the solution to converge is to solve only a small piece of the whole assembly. Isn't the left side just a mirror image of the right side?  Why solve both?  Just cut the model in half and use a symmetry plane at the center.

The temperature condition causes the thermal expansion to grow the pad 14 mm longer, 4 mm wider and 0.4 mm thicker. If you want that, you should do that in step 1 before you close the blocks in step 2, but you have to leave 0.4 mm of space for it to grow in step 1.

Viscosity has no effect in the Static Structural model. Plasticity will allow the material take on a shape. Viscoelastic may be useful in a Transient model. 

  • Liked by
  • RosarioAnsys
peteroznewman posted this 28 March 2018

Below is the result of a half model, rigid blocks, Thermal Condition suppressed, Plasticity added to the material and a block displacement of 1.3 mm. It converged in 96 iterations.

  • Liked by
  • RosarioAnsys
RosarioAnsys posted this 28 March 2018

I'm working on the modification in the day, I'll let you know what I'm getting as a result today or tomorrow.

Thank you for the help

RosarioAnsys posted this 28 March 2018


I made various changes, changed the type of contact and used the large deflection function.

Unfortunately, after 1 hour of calculation without result I had to cut the simulation, I think that my computer is not powerful enough to manage this kind of simulation.

I still could get this chart using the coefficient of friction, the wide deflection and the auto time stepping:

and 2 errors:

"The solver engine was unable to converge on a solution for the nonlinear problem as constrained.  Please see the Troubleshooting section of the Help System for more information."



"The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose."


But, by removing only the thermal condition and restarting my computer I could get a new simulation:

But otherwise you're quite right when you say that the displacement is 1.3mm and it was possibly a source of problem during the simulation.

Would it be possible to have your data table, especially the value of your plasticity?

Would it be possible also to get your study attached so that I can simulate with correct values on my side but also with an easier understanding of your explanations on previous posts?

Thank you again for your time in solving my problem.

A last little thing like do you do to cut the model in half? I'm sorry I really beginner on Ansys?



peteroznewman posted this 28 March 2018

Hello Rosario,

You didn't say what version of ANSYS you are using. I used version 19.0 but if you are on 18.2 I can easily recreate this model in that version.

The Plasticity is the Bilinear Kinematic Hardening with a Yield Strength of 1 MPa and a Tangent Modulus of 0.

My model will run on your computer, it just may take longer, but it will take the same 96 iterations.

You can show your appreciation by clicking Like below the posts that are helpful.

Attached Files

  • Liked by
  • RosarioAnsys
RosarioAnsys posted this 28 March 2018

Hi, yes i used version 18.2.

How I have nothing to lose, I would try, it's more compared to what is problematic compared to my simulation and compare yours and mine.



peteroznewman posted this 28 March 2018

For the half model in version 18.2, the solver only needed 84 iterations, which took 9 minutes on my 8 core computer.


Attached Files

  • Liked by
  • RosarioAnsys
RosarioAnsys posted this 29 March 2018


I thank you for your speed and your file.

But I have a problem with generating the results:

I have erased the data generated before simulating as said in the window that I had when opening the file, but no change.

So, it's impossible for me to read the results or launch a resolution.

Thank you

Attached Files

peteroznewman posted this 29 March 2018


The error is in one of the result plots. Just delete the result plots, it will not delete the solution. Then make new result plots.


  • Liked by
  • RosarioAnsys
RosarioAnsys posted this 29 March 2018

Thank you, it's perfect, I'll be able to go on good bases with your model and mine

I thank you again for the help you have given me and thanks to you I understand better the software and the subtleties of it.

Good day to you and see you soon

RosarioAnsys posted this 6 days ago

Good morning,


I'm going to go back to the subject because I'd like to refine a detail in the simulation.

Indeed, I modified the material in order to correspond more to my need and I have some things which suit me perfectly thanks to you.

Now I would need to know the force needed for the upper block to come into contact with the lower block, so technically crush the material too.

I guess like you did on the simulation, putting a move doesn't take force into account.

To obtain the necessary force, I therefore decided to apply a downward force on the upper block (for the moment 1000N) like this:

My goal being to know the force necessary to the upper block to go up to the lower block, I decided to apply a force on the upper block and to modify the force until I obtain the desired result, that is to say: The two blocks are in contact and that the matter is crushed.

I think that my method is too long and that there are problems at the level of it since the simulation does not succeed on my side.


I also think that a distance limit condition is missing because indeed, by applying a force to it the upper block will tend to enter the lower block, right?

How to tell the software: as soon as the upper block comes into contact with the lower block the simulation must stop?


So is there a way to get an effective method to determine the force needed at my upper block to go to my lower block with a stop when they come into contact?

Edit: I also tried to put a free move on the upper block and put in solution "reaction force" but impossible to solve my simulation.

I don't know if it's possible to do what I want, I keep asking about youtube and the forum in the meantime


I have my Ansys file attached so you can see the problem.

Thank you all in advance



Attached Files

peteroznewman posted this 6 days ago

Hello again Rosario,

Suppress the force and unsuppress the Joint Displacement, which provides the correct motion to close the mold top to the bottom.

What you want to know is the force that is required to create this motion. That is being monitored during the solution and can be plotted using a Joint Probe.

I'm running your model now. I see it wasted 10 iterations at the beginning. Change the Initial Substeps from 10 to 20 to eliminate this first bisection when you run it.

After 191 iterations for me (181 for you), the solver finished. Here is the Force Probe result:

Warm regards,


Attached Files

  • Liked by
  • RosarioAnsys
RosarioAnsys posted this 2 days ago

Hello peter, 


This is exactly what I wanted and I didn't think it was so simple to get the desired result

I thank you very much for the help you give me.


I wanted to modify the dimensions of the material, that is to say to pass from 6mm to 7mm of height.

Unfortunately impossible to solve, I kept exactly the same settings not to distort the simulation, here is my mistake:

I put my archive in the subject.

I suppose it's something very simple to change but I really don't find, looking at the error, I wanted to change the substeps, but impossible to simulate without error.



Attached Files

peteroznewman posted this 2 days ago

Hello Rosario,

I see the distorted element error message in the image in your post. That can be very difficult to get past. Before I look at your archive, here is what you should try:

1) Take smaller time steps 
Break the analysis into 2 steps. Say the mold motion is 5 mm to close the mold fully in one step, but the error occurs at time 0.82 s, or in other words, 4.1 mm of motion. Change to a 2 step analysis where step 1 is 4 mm and step 2 increases that to 5 mm.  Now in the Initial and Minimum Substeps of step 2, type 100 to force the solver to take small time steps through the difficult portion. Insert your own numbers in this example. This alone may not be sufficient to resolve the problem, but might be required along with other changes.

2) Create better element shapes
Create a Named Selection for the element number in the error message to see where the problem is occurring. Look at the deformation at the last converged time step before the error. Can you see that the element is obviously distorted?  If so, add mesh controls, or slice the solid in Geometry in order to make an element that is pre-distorted in the opposite direction to the final distortion. As the solution proceeds, the element shape will get better, not worse. On some models I have got this error, but the element looks like an almost perfect cube, so there is nothing to improve.

3) Reduce the element size
Use smaller elements around the problem area, but not at the expense of ideal element shapes.

Please try those and let me know if you need additional help on how to do either of them. I don't have time to work on your model now, but I can answer questions.

Good luck,


  • Liked by
  • RosarioAnsys
RosarioAnsys posted this yesterday

Good morning, 

Your first solution works perfectly, no need to use the following methods, so thank you.