The interaction between two parts

  • 85 Views
  • Last Post 5 weeks ago
Aaron posted this 17 January 2019

I would like to simulate the following process:

fist to bend the hinge, which has a cavity inside. After the bending arrived to its limits(the two oblique surface coincides), I try to stuck a part inside. The connecting faces between two parts are bonded. Afterwards, release the load to see the interaction between the two parts.  I have tried several ways, but fianlly failed.

Does anyone have suggestions? thanks.

The parts is sort of as following.

Order By: Standard | Newest | Votes
peteroznewman posted this 18 January 2019

Relevant post. I can imagine a cavity added to this post.

If you have folded the hinge until the cavity has collapsed, how to you stick a part inside the cavity?

Please sketch out (with a pencil) a more detailed sequence of events you want to simulate and post those images.

When does the bonding occur and which faces are bonded?

Aaron posted this 18 January 2019

  • I did it twice to get the configration, and fabricate the cavity, after that I place the fabricated part inside.
  • as shown int the schematic, faces 1,2,3,4 are bonded to the outer part. But for the two end faces, it is open, which means the hyperelastics material could deform in the width direction
  • the schematic is shown as follows. the shady is the fabricated part. afterwards, due to the stress of the outer part, it would try to restore to be flat, while the inner part would prevent that movement. I would like to get the equillibrate state.
  • Thanks a lot.

jj77 posted this 18 January 2019

This looks to me like a staged analysis. Use perhaps birth and death to activate part in the cavity, once you have bent the part. See this video for more details

https://www.simutechgroup.com/tips-and-tricks/fea-videos/348-ansys-workbench-tips-tricks-element-birth-death

Hope it helps

  • Liked by
  • peteroznewman
Aaron posted this 18 January 2019

thank you for your advice.

I did it in your way. But problem is still there.  Want to share my file, but the .wbpz file is too large,about 350M. is any other way to share with you?

Thank you so much.

peteroznewman posted this 19 January 2019

RMB on Mesh (in Mechanical) or on Model (in Workbench) and Clear Generated Data, then save the project and create the archive. It will be much smaller.

  • Liked by
  • jj77
Aaron posted this 20 January 2019

ok. I clear up all those results as follow. thank you, peter.

Attached Files

peteroznewman posted this 21 January 2019

Hi Aaron,

This is a very interesting problem. I took your model and sliced it through the center to use half symmetry and make the model solve faster. I also improved the mesh and added a frictional contact so the part did not self-intersect. Here is the result with a section view that cut out the back face to make it easier to see the issue: how to fill a body into the deformed shape, then release the stress in the part.

Unstressed shape with an empty cavity:

Stressed shape that wants an unstressed insert molded into the cavity.

Attached is an ANSYS 19.2 archive.

I look forward to members answering the question of how to accomplish this task.

Attached Files

Aaron posted this 21 January 2019

Thank you so much for your patience and help. Let us wait.

By the way,I have tried some other ways. The method here I wanna use is a sort of pre-force. So I exported the results out and then map the field to the new model as preloading. Afterwards,assembly the two parts.Finally.remove the preload.It is just my plan.I don not know whether can realize it or not. I see some clips on line,and they took force as preloads. But here I should map stress or strain. After I imported the data,it reported the data is invalid.I am trying to fix it.

 

Thank you again.

jj77 posted this 21 January 2019

 I have never done staged analysis in ansys, but it looks like the only options is that there are stresses to fit the space thus one would end up with stresses and not a stress free state. In other software that are used in civil and say for staged analysis, one has the option of adding the structure in a stage in a stress free state (e.g., in Strand7). This is called there the morphed option. So one for morphing one would export the deformed mesh and then mesh the cavity, making sure that there is compatibility at the boundaries, at the same time keeping the stress state in the deformed part constant.

 

So I see it as a two step restart problem, so export deformed part or mesh/geom., generate the cavity mesh/geom., and then bring it and add it in to the deformed and stressed part, and continue loading.

I tried also to be clever by deleting the stresses say after the first step when the part gets inserted (step two) via the inistate,dele, command, but that does not work when one has multiple steps. It would work though if we had one step and managed to get the run time live actual time of the current iteration so one can then set that after say 1 s (if statement) one does an alive on the cavity part + inistate,dele, that should in theory work, but I guess it has to be a subroutine and I do not have much experience with that in ansys (just abaqus and strand7 api)

jj77 posted this 21 January 2019

Actually it might be when they are reactivated that they are stress free, ansys help manual seems to indicate that they do not have any strain history, and the results I am seeing are very low strains compared to the model I deform, and quite small stresses compared to the rest of the model.

 

I think Peter you have had this discussions before, but I do not know if the conclusion is that they become alive stress free. Seems so to be.

peteroznewman posted this 21 January 2019

Yes jj77, the elements come alive stress and strain free.

I thought about having elements inside the cavity that are killed. I imagine this would work if the cavity was flat and the elements in the cavity were only 1 element thick. That way, the shape of the cavity elements are controlled by the shared nodes on the rubber hinge, and when they are made alive, their proper shape is present.

The problem in this situation is that a single element won't span the gap. I wonder what would happen to the nodes in the center of the cavity. There is nothing moving them to be between their neighboring shared nodes that are moving a very large distance, probably turning the killed element inside-out in the process.

What if an extremely low stiffness material was assigned to a body that was in the cavity at the start? The nodes inside this body move as the walls of the rubber hinge move to complete Step 1.  Then in Step 2, the elements in the cavity are assigned zero stress in the INISTATE command, and the material is changed to the material of interest, then the solution continues with the proper stress in the rubber hinge and a zero stress part in the cavity. I don't know if this is possible or how to do it, but that is along the lines of a two-step process.

Regards, Peter

Aaron posted this 22 January 2019

Thank you so much. 

I used to utilise ABACUS before. So, is it possible to realize it in ABACUS, based on your experience?

Thanks.

peteroznewman posted this 22 January 2019

Hi Aaron,

Discussion of how to do this in ABAQUS would be appropriate on the SIMULA User Community website.

This site is for ANSYS discussions.

Regards, Peter

Aaron posted this 22 January 2019

OK. Thank you. I will try.

jj77 posted this 5 weeks ago

Many software vendors (at least from my working exp., I have done this many times for users, called a demo capability report), can do a benchmark should you want to buy the software or extend/upgrade it (e.g., subscr.), so it might be worthwhile contacting your software vendor/re-seller and discuss, mentioning that you need to do this and if not possible you might need to change software (to one that can analyse this), of course this needs to be true, so that would be the case, e.g., if this type of analysis is what your company need to do, in order to manufacture this part, so you need to do this on a regular basis, and hence need a method of doing this.

 

 

Aaron posted this 5 weeks ago

Thank you my friend. I wil try to ask their technician to see.

If further information, I will share with your guys.

Thanks  a lot.

  • Liked by
  • jj77
Close