## LS Dyna

#### Force reaction decrease after decreasing mesh size

• Mansoureh
Subscriber

Dear all, I have a problem with mesh sensitivity analysis

I am doing a Quasi-static analysis for one unit cell of Gyroid. the size of the unit cell is 1*1*1 and i want to compress it up to 0.1 mm . bottom plate is fixed.

• peteroznewman
Subscriber
Dear For the issue of plotting a force vs displacement curve, if you plot the displacement of the plate, it doesn't matter that some parts of the sample lift off the plate, both the top and bottom plates have this effect. One approach for tracking the displacement of the part is to make a Named Selection of elements that are very close to the top plate. Then you can plot the Minimum Z Directional Deformation. That value would capture the elements that are still touching the plate. The elements in that Named Selection that lifted off the plate would be measured by the Maximum Z Directional Deformation.
The mesh sensitivity study shows a good trend. What is the thickness of the wall? How many elements are across the thickness at a mesh size of 0.01 mm? Linear Tet elements are known to be overly stiff in bending, so 1 element through the thickness must never be used, 2 elements through the thickness is unacceptable, 4 elements through the thickness is barely acceptable, 8 elements is great.
That guidance is for linear tet elements, and doesn't apply to quadratic tet elements, but those are not available in Explicit Dynamics.
Linear Hex elements perform better than linear Tet elements. If you could generate a gyroid surface, mesh that with quad elements, then extrude those into hex elements, like two layers on each side, that would be four hex elements through the thickness and would give you a better ability to increase the number of elements through the thickness without creating a huge number of nodes.
You will find that the Force-Displacement curve converges with element size faster than the Stress-Strain curve.
• Mansoureh
Subscriber
Dear Peter
Thank you very much for the answer. For the first paragraph, I should check your criteria. But I think the problem is very serious than that at first, I should bring my mesh from another program which means my mesh is not editable at all and I could not define to give me exactly 4 elements in the thickness I put the image below to show you how was the element for all 5 mesh sizes, at best, for mesh size of 0.012, you can find it in the below image:

thickness is 0.04 mm. and the whole dimension of unit cell is 1*1*1 mm

, for the final mesh size of 0.012, the simulation takes 4 days !!!! and I used mass scale as well but the performance of my PC does not work especially when I am using other programs during doing simulation. But the result of mesh sensitivity does not satisfy, How much should make the elements be smaller???? for example for one paper that I found, for a simple unit cell of Primitive they found the mesh sensitivity with 3 values: BUT for me, it does not work, I think something is wrong with my model, maybe I should change the unit cell to sth like this paper and try again with my own material
yes thank you for mentioning that to me I am aware that I should use linear elements. I did not try quad mesh and I do not know the software can create that type for this structure tr not, I can try it, but I do not think that it works.
and one important thing is time. I was waiting for the smallest mesh size for 4 days. at the beginning of the simulation, it shows me 20 hours but I do not know why but every time that I checked it it was very slow, for the last 5 hours that it showed me for the remaining time, it took 15 hours to complete!!

• peteroznewman
Subscriber
Dear I know you are using nTopology to create the gyroid solid body and export a solid element tet mesh directly from that. I don't know if nTopology can create a gyroid surface body and mesh that with linear quad elements. I don't know if nTopology can extrude quad elements normal to their face to create a thin hex solid element. ANSYS Mechanical meshing can extrude shell elements into solid elements.
The important feature of extruding shell elements is the tremendous reduction in node count vs tet meshing the thin walled solid. This will reduce the amount of memory and storage needed for the solution. Unfortunately, Explicit Dynamics codes compute the maximum time step from the characteristic length, and that is going down according to the minimum dimension of the element. As more elements go through the thickness, the maximum time step is reduced, no matter if it is a small tet element or a thin but long and wide hex element.
Here is a thread where I created a gyroid surface using matlab code, and exported the STL from matlab to use in ANSYS. This isn't great because STL files are triangles, which are not as good as quad elements. With a bit more work the triangles can be converted to quad elements in other software.
https://forum.ansys.com/discussion/32275/spaceclaim-surfaces-from-implicit-equations
Here is another thread where someone has exported an IGES file from software called MathMod.
https://forum.ansys.com/discussion/1035/issues-when-meshing-a-complex-gyroid-shape-heat-sink
• Mansoureh
Subscriber
Dear Peter, thank you for your reply, yes I could extract Quad mesh from nTop. and now I am working on simulation, I hope that I can get my result.
I will inform you if I could get results from mesh sensitivity.
Just two questions:
1.
I want to do a quasi-static simulation for the compression test.
In the " Analysis setting" there are several options like :
using " Custom " type and manually use a mass scale setting to speed up a simulation
or
"Quasi-static " type and use the mass scale?
What is the difference between these two option? Do they give us the same result under the same boundary conditions and end time value? I found this explanation in help ansys.

2.
and my other question is related to failure criteria:
If I want to use "strain limit" as failure criteria: ( we have tensile test data and we have failure 10% strain, which one would I define for my failure criteria?
should I define it in "analyst setting " as " geometric strain limit " parameter" OR in the "engineering data for material"?
What's the difference between them?
In ansys help, they wrote a recommendation for geometric strain limit. why do they recommend it as 0.75 to 3? I got confused !!
Thanks a lot for your help.
• Mansoureh
Subscriber
Dear Peter, thank you for your reply, yes I could extract Quad mesh from nTop. and now I am working on simulation, I hope that I can get my result.
I will inform you if I could get results from mesh sensitivity.
Just two questions:
1.
I want to do a quasi-static simulation for the compression test.
In the " Analysis setting" there are several options like :
using "Custom" type and manually use a mass scale setting to speed up a simulation
or
"Quasi-static" type and use the mass scale?
What is the difference between these two option?Do they give us the same result under the same boundary conditions and end time value?I found this explanation in help ansys.

2.
and my other question is related to failure criteria:
If I want to use "strain limit" as failure criteria: (we have tensile test data and we have failure 10% strain, which one would I define for my failure criteria?
should I define it in"analyst setting " as " geometric strainlimit " parameter" OR in the "engineering data for material"?
What's the difference between them?
In ansys help, they wrote a recommendation for geometric strain limit. why do they recommend it as 0.75 to 3? I got confused !! I mean if I want to use my data from tensile test at 10%strain, it would be under recommendation. Right?

Thanks a lot for your help.

• Mansoureh
Subscriber
thank you for your reply, yes I could extract Quad mesh from nTop. and now I am working on simulation, I hope that I can get my result.
I will inform you if I could get results from mesh sensitivity.
Just two questions:
1.
I want to do a quasi-static simulation for the compression test.
In the " Analysis setting" there are several options like :
using "Custom" type and manually use a mass scale setting to speed up a simulation
or
"Quasi-static" type and use the mass scale?
What is the difference between these two option?Do they give us the same result under the same boundary conditions and end time value?I found this explanation in help ansys.

2.
and my other question is related to failure criteria:
If I want to use "strain limit" as failure criteria: (we have tensile test data and we have failure 10% strain, which one would I define for my failure criteria?
should I define it in"analyst setting " as " geometric strainlimit " parameter" OR in the "engineering data for material"?
What's the difference between them?
In ansys help, they wrote a recommendation for geometric strain limit. why do they recommend it as 0.75 to 3? I got confused !! I mean if I want to use my data from tensile test at 10%strain, it would be under recommendation. Right?

Thanks a lot for your help.
• peteroznewman
Subscriber
Dear I expect the difference between Custom and Quasi-static settings in Explicit Dynamics is that the Quasi-static setting automatically chooses values for you, while for Custom you have to figure it out yourself. If you use the same values in Custom that were chosen in Quasi-static, then you will get the same result.
For Geometric Strain limit, there is no problem using 0.1 as the Geometric Strain limit. There is a default value of 1.5 so that solutions continue when no failure data has been entered by the analyst. I don't know why they have a lower limit on the recommended range. If the element gets too distorted, it can cause the solution to stop, so it makes sense to have an upper limit on this field.
In the Explicit Dynamics Theory Guide, the equation to calculate Geometric Strain is given as Equation 5-25. 5.3.4. Erosion Controls (ansys.com)
For On Material Failure feature of Erosion controls, see this page of the Autodyn User's Manual 22.6.3. Failure Models (ansys.com)
In section 22.6.3.1, it shows Material Stress and/or Strain Failure is created to handle composite materials that have a fiber direction 11, a matrix direction 22, an interlaminar direction 33 and a tensile failure limit in each of those directions is required along with other data.
So I would conclude that you would not get the identical result when using a strain value of 0.1 for the Geometric Strain Limit compared with using On Material Failure and using 0.1 for each of the three directions due to different equations being used.