I am testing auxetic lattices of mult-metamaterials, however I have some problem with penetration during compression anyone had this problem before?
As it goes past 20mm stroke that's when it starts to penetrate, with other materials this problem did not occur.
Did you define contact between the faces that are penetrating?
yes, do you think setting a pinball radius could fix the problem?
Yes, you want a big pinball radius that covers both faces.
Also, you want a mesh that has more than one element through the thickness.
ok, atm I have set the pinball radius around 2-3mm, problem did not solve so i set it to 15mm
Pin ball radius of 15mm
update: tried pin ball radius, tried changing formulations such as using augmented lagrange and pure penalty but still same problem, any other suggestions?
If you attach your model here then perhaps someone can have a look
Delete that post above.
And see this link on how to attach a file
I'm currently running the solver I will upload the model once its finished thanks
I've cleared generated data for mesh and results, so if anyone wants to have a look just generate mesh with fine, It would be good to have this solved by friday thanks.
I have a few comments.
There are many small sliver faces. What CAD tool are you in? Those defects in the geometry should be removed before you start meshing. There are tools in Mechanical to repair these faces and careful use of Mesh Defeaturing can overcome these defects but it's better if they are cleaned up in CAD. Once you do this, the bodies will be sweepable and you can use fewer elements along the extrusion direction.
The best practice is to have at least two elements through the thickness of the part. There is a global mesh setting, Proximity, that can put 2 elements through the thickness of thin walled parts.
Rather than using Bonded Contact to connect the parts, the mesh would be simpler if you united all the bodies so it could mesh two element through the combined thickness, instead of each half of the wall thickness.
A few small changes like flipping the Target/Contact sides of the Frictional contact and you can save on the number of nodes in the model. The Frictional Contact is not closed. I used Adjust to Touch to get it to be touching.
Use Auto Time Stepping On. When you turn this Off, you don't get the benefit of allowing each load increment to achieve equilibrium, so the shapes you end up with may be wrong and not in equilibrium. I realize that with the two elements through the thickness and the auto time stepping on will greatly increase the solution time. This is the price you have to pay to get an accurate result.
In 2 hours, the solver made 80 iterations and advanced to a time of 0.0675 sec into the 30 mm displacement or 2 mm. So in 30 hours, it might get to 30 mm, but probably not. It would take less time if fewer elements were used along the extrusion direction. If I was you, I would reformulate this as a 2D Plane Strain model, then it will solve in minutes instead of hours.
I haven't done this yet, but that is the next step.
Attached is the ANSYS 2019 R2 archive.
I am using autodesk fusion 360, I will try the 2D plane strain
Do I change target contact sides for all layers and indenter?
Some feedback with regards to your initial problem (parts going through each other).
In your model you have not defined contacts between the structure that is getting compressed. That is there is no self contact, so parts will go through each other. The bonded contact you have is to keep these part bonded, but that will not account for the self contact between different parts when they are being squashed together and different faces make Contact with themselves or with adjacent faces.
To define this type of "self" contact see the example below (you need to do this for all self contacts (for every faces that might come into contact), so there will be quite a few for your case. This is a part that is being pressed on the top thus the internal hole faces will start contacting each other.
I am going to try this right now I will update once finished.
Thank you jj77 it worked
Ansys customers with active commercial software licenses can access the
customer portal and submit support questions. You will need your active account number to register.