Optimizing a spanner/wrench in hyper mesh-optistruct
Answers
-
The blue elements in the Quality Index Panel indicates elements with borderline quality and the compound Q.I. is perfect at 0.01.
0 -
as you mentioned 'recommended that MINDIM be at least 3 times, and no greater than 12 times, the average element size' so if element size is 1 then for 3D models should it be 3 (MINDIM).
0 -
Hi
can you check the model which i uploaded whether the meshing is correct.
Initially I started with meshing in 2d and got a value of 0.02.
Then I converted to 3d model.
Element density =2
0 -
Altair Forum User said:
so if element size is 1 then for 3D models should it be 3 (MINDIM).
mindim is based on the average element size. For 2D elements is calculated as the average of the square root of the area of the elements and for 3D elements,
as the average of the cubic root of the volume of the elements.Altair Forum User said:can you check the model which i uploaded whether the meshing is correct.
There are some issues:
- the elements in the Design component are duplicated 4 times
- there are 4 holes because not all 2D elements were dragged in the X direction
- meshing with quads only results in lots of elements failing jacobian (F10: check elements>3D>jacobian). Try meshing with quads, which allows some triangular elements for better mesh quality
- after 2D elements are used for solid map they should be deleted
- some nodes of 2D elements at the vertical line (design and non-design space split) were moved which might not be desired
0 -
Hi
I have tried to include most of the suggestion you have mentioned. I have tried it with both quads and mixed meshing with meshing size of 2. I still wasn't able to get a good result like yours. I have uploaded both the files and photos of the 2 meshes. Any valuable feedback is appreciated. I also took the MINDIM to be 2.(if its wrong kindly help how to calculate this value with an example).
Thanks
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
0 -
Hi,
try meshing with QI optimize using criteria from the image below. If you want structured mesh then partition the surfaces before meshing (F11: quick geometry edit>split surf-node/line).
<?xml version="1.0" encoding="UTF-8"?>
Given the average mesh size of 2 the mindim should be 2*3=6. If the defined MINDIM is less, it will be reset to a default value equal to 3 times the average element size.
0 -
Hi, i have meshed it as per the above info. Have a look and let me know for any errors.
can you have a look. I have used the partition like always to separate the two parts front and end.
You mentioned ' I have re meshed the model with hexa/penta mesh with uniform element size through the thickness.'. Is the thickness mentioned here about the mesh size.
Kind
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
0 -
The element check is OK, but there is always room for improvement :
- Back to back triangles should be avoided
- Avoid triangular elements on outer edges or holes
- structured or smooth mesh is recommended
Use drag tria element, combine tria element and smooth in QI panel.
The two parts (front and end) could be further subdivided to allow better control of the mesh flow.
Check how not to mesh (from page 20):
https://altairuniversity.com/wp-content/uploads/2014/02/2Dmeshing.pdf
Altair Forum User said:Is the thickness mentioned here about the mesh size.
Yes, I meant mesh size in the X direction, which should be equal to mesh size in YZ plane.
0 -
Hi,
I did try out most of the functions in QI panel except drag tria element and when I tried using smooth function it does not give any result back it still remains the same. I used the QI optimize function for my previous models except I didn't make any changes to the Jacobean value.
'Yes, I meant mesh size in the X direction, which should be equal to mesh size in YZ plane.' Reagrding this, is there any way I can check it out or understanding from the figure.
Currently I am not in front of the system. I will try these out and let you know. Once again big thanks for guiding me with your feedback.
0 -
Try smoothing using 2D>smooth panel.
I was referring to the element size or density (number of elements along the depth of the mapping) to be defined in the along direction. Increasing the element size in the depth direction (in this case x-axis) will increase 3D element aspect ratio, which is undesirable (default element check limit is 5).
<?xml version="1.0" encoding="UTF-8"?>
The attached model has a structured mesh. Observe how the surfaces were partitioned.
0 -
Hi
Thanks for your tips. I do have a small doubt the result u obtained previously, is it all dependent on the meshing or any other factors have to be considered.
Thanks
<?xml version="1.0" encoding="UTF-8"?>
0 -
Hi,
in addition to mesh dependency, topology optimization results will be influenced by these factors:
- volume fraction constraint
- manufacturing constraints (minimum/maximum member size, draw direction, extrusion, pattern grouping-symmetry,...)
- design optimization parameters (DOPTPRM)
<?xml version="1.0" encoding="UTF-8"?>
0 -
nil
0 -
Hi
Thanks, I did get a better result but I have a doubt are there any preconditions required to place the node for these functions 'draw direction, extrusion, pattern grouping' ( I even tried it with my model using diff samples). I did got through the tutorials and the videos which were available and is it possible to use all the above 3 at once.
Thanks
0 -
Please refer to Optistruct help (User Guide>Design Optimization>Manufacturing Constraints>Topology Optimization Manufacturability) for more details.
It is perfectly acceptable (and general practice) to combine multiple manufacturing constraints, though the user should be careful not to over constrain the problem and be aware of the reduction in design freedom that the manufacturing constraints bring.
Combining pattern grouping (symmetry) with extrusion constraint is currently not supported:
*** ERROR # 780 ***
DTPL card with simultaneous PATRN and EXTR is not supported yet.
violated DTPL id = 10
Altair Employee
