# Optimizing a spanner/wrench in hyper mesh-optistruct

## Recommended Posts

Thanks

##### Share on other sites

I tried applying force close to the edges as shown in the figure both the sides and got a result. This is the closest i got to. I am trying to get the x design in the middle.

##### Share on other sites

In the model you shared the tetramesh is too coarse in the interior of design component (see image below). Because topology optimization results are mesh dependant there is not enough mesh resolution available for truss-like structure. I have remeshed the model with hexa/penta mesh with uniform element size through the thickness.

To get truss-like structure minimum member size control (mindim) should be used. From Free eBook: Practical Aspects of Structural Optimization (A Study Guide):

Quote

Controls the smallest dimension to be retained in topology design, as well as minimizing the checker board effect caused by
the mesh and giving a more discrete design. Since the optimization is seeking a discrete value of 1 or 0 for the elements, this
constraint usually improves the clarity of the design, by penalizing intermediate elements that would otherwise form.
Although minimum member size (MINDIM) control penalizes the formation of small members, results that contain members
significantly under the prescribed minimum member size can still be obtained. This is because a small member in the structure
can be very important to the load transmission and may not be removed by penalization. Minimum member size control
functions more as a quality control than a quantity control.
It is recommended that MINDIM be at least 3 times, and no greater than 12 times, the average element size. 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

Because the model has uniform depth it can be simplified to 2D for learning purposes. Try out different optimization controls before moving to 3D.

Try the following options on topology optimization card (DTPL):

-parameters: mindim

-pattern grouping: one plane symmetry

-extrusion

-draw

Rahul R likes this

##### Share on other sites

Thanks

Just to get some point clear

1) For hexa meshing -> 3D -> Solid Map -> one volume -> source shel -> quads only -> elem size= 1. I have attached a snap shot below

2) 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).

3) when I increase my element size to 2 i get an error message saying

" Element # 17725, element type HEXA.
*** PROGRAM STOPPED: ERRORS DURING ELEMENT QUALITY CHECK."

##### Share on other sites

I usually first create the 2D mesh on surfaces, then use 3D>Solid Map>general. This procedure gives better control over mesh quality. Meshing complex geometry with quads only option might result in bad mesh quality.

The error you have is due to bad element quality. You should remesh or bypass element check (not recommended) with control cards> PARAM> CHECKEL>NO

iwinphilip likes this

##### Share on other sites

Can you help with this what this light blue color indicates and i get a mesh value of 0.01. i am using element optimize method.

##### Share on other sites

The blue elements in the Quality Index Panel indicates elements with borderline quality and the compound Q.I. is perfect at 0.01.

iwinphilip likes this

##### Share on other sites

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).

##### Share on other sites

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

##### Share on other sites
9 hours ago, iwinphilip 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.

8 hours ago, iwinphilip 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

iwinphilip likes this

##### Share on other sites

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

Mixed.hm

##### Share on other sites

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).

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.

iwinphilip likes this

##### Share on other sites

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

trial1.hm

##### Share on other sites

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):

49 minutes ago, iwinphilip 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.

iwinphilip likes this

##### Share on other sites

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.

##### Share on other sites

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).

The attached model has a structured mesh. Observe how the surfaces were partitioned.

##### Share on other sites

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

##### Share on other sites

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)

nil

##### Share on other sites

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

##### Share on other sites

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:

Quote

*** ERROR # 780 ***
DTPL card with simultaneous PATRN and EXTR is not supported yet.
violated DTPL id = 1

## Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

×   Pasted as rich text.   Paste as plain text instead

Only 75 emoji are allowed.