April 9, 2020 at 3:50 pmCADuserSubscriber
I have the following question: It is about pressing a plate (1mm thickness) into a certain shape. The mould has an organic shape. With the result it should be shown if or if not the thickness of the plate is sufficient. The plate (plastic) is heated and shaped accordingly by a mould (with upper and lower part).
So far I have tried out different variants and have made progress with the static-mechanical analysis. Explicit dynamics was also tried out. Do any of you have experience in this field or a suggestion how to proceed?
I would be happy about an answer. Thanks a lot.
April 9, 2020 at 6:19 pmWenlongAnsys Employee
Since the plate needs to be heated and deform correspondingly, I would recommend a coupled thermal-structural analysis.
You can find more information in this link:https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/wb_sim/ds_coupled_field_static.html
- How to access Ansys Online Help Document
- How to show full resolution image
- How to use Google to search within Ansys Student Community
April 9, 2020 at 6:26 pmCADuserSubscriber
Dear Mr. Wenlong,
Thank you very much for your answer. Unfortunately the link you have provided seems to me only accessible to companies. Is there another one that I can access as a student? Thank you very much.
April 10, 2020 at 8:27 pmWenlongAnsys Employee
Can the temperature be considered as boundary conditions?
> If yes. Is dynamic effect dominant?
----> If yes, then choose transient structural or Explicit dynamics
----> If no, then do a Static structural.
> If no, is the plate heated first, and loaded after the temperature gets stable?
> If yes, then do a steady-state thermal analysis, then transfer the temperature distribution result to a static structure analysis or transient structural analysis.
> If no, which also means if the plate is loaded while being heated up (heat has not become steady while loading), then a coupled thermal-structural analysis may be necessary. I think alternatively, you can do a transient thermal analysis, then transfer the result data to a static or transient analysis, providing that your structural deformation won't influence the heat transfer speed.
April 11, 2020 at 12:04 amCADuserSubscriber
Dear Mr. Wenlong,
thank you very much for your help. The temperature can be considered as boundary conditions.
I am currently not sure if the dynamic effect is so dominant. The plastic is heated and then shaped by two moulds (see picture). The force to be applied should be kept constant. Which method do you think would be better for this purpose?
Furthermore, the problem of body penetration has occurred despite weak springs and the use of the pinball region. Unfortunately the target body does not deform as desired. Do you have a suggestion for possible adjustments?
Thank you very much.
April 11, 2020 at 12:18 ampeteroznewmanSubscriber
I am sure that the inertial forces are insignificant in this process.
April 11, 2020 at 8:54 amCADuserSubscriber
Thank you for your answer. What type of analysis do you think would be best?
I also don't think inertial forces play a significant role here. Furthermore, the plastic plate has a maximum size of 70x70mm.
April 11, 2020 at 10:17 ampeteroznewmanSubscriber
Wenlong outlined a very nice decision tree. The process you describe sounds like Thermoforming. I understand the plastic sheet will be heated in an oven to a uniform temperature, then placed in a mould and pressed into shape and allowed to cool so that it keeps the shape when removed from the mould.
The heat flow between the plastic and the mould can affect the thickness distribution as the pressing occurs. If the mould is wood, then the heat transfer to the mould while pressing is slow, but if the mould is aluminum, then the heat transfer during pressing could be large, reducing the temperature of the plastic in the contact area and affecting where the thinning occurs.
- What material is the mould made out of?
- What is the temperature of the mould when the plastic is inserted?
- What is the temperature of the plastic when inserted?
- What is the air temperature around the mould?
- How many seconds does it take to move the plastic from the oven to the mould?
- How many seconds does it take the mould to close and press the shape (not counting the cooling time)?
The type of analysis depends on the answers to these questions.
I have the free Student license of ANSYS 2020 R1 and the Coupled Field Statics is the first analysis in the Toolbox.
A Statics model can have a large amount of deformation in the parts which is enabled under Analysis Settings by turning on Large Deflection.
Looking at your image, I see a single layer of elements through the thickness of the plate. I can't tell if you modeled the plastic sheet as a surface in CAD and meshed it with shell elements and assigned a thickness, or if you modeled the plastic sheet as a solid in CAD. If you have solid elements, you will require around 8 elements through the thickness of the sheet. This will require a lot of nodes and you might exceed the Student node limit of 32,000. I recommend you create a surface in CAD and mesh with shell elements. The thickness of the shell can be tracked during the solution and the thickness distribution easily shown in the results. This model will also take less time to solve.
April 11, 2020 at 10:54 amCADuserSubscriber
Thank you for your detailed answer. I have already asked myself similar questions. I also consider the use of shell elements to be useful.
Unfortunately I haven't done too many analyses yet and I'm not familiar with all functions in Ansys. Personally, I think a coupled field statistics analysis makes sense. Since the mould will not be made of metal but comparable to wood and the times used are negligible (less than 10s for removing and closing the mould), I think this type of analysis should be sufficient, don't you?
What advantages could transient structural or explicit dynamics bring?
April 11, 2020 at 11:38 ampeteroznewmanSubscriber
Wenlong provided the following directions for how to access the Help system to open a URL link...
A transient solution would allow the cooling over time to be included in the simulation. There could be a significant change in the surface temperature of the plastic in even 10 s.
If the mould required punching a hole in the sheet, that would be simpler to model in explicit dynamics.
April 11, 2020 at 1:04 pmCADuserSubscriber
Okay, thank you both for the great help! Happy Easter!
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
© 2022 Copyright ANSYS, Inc. All rights reserved.