# Optimizing a spanner/wrench in hyper mesh-optistruct

## Recommended Posts

Hi,

I am a new user to Hypermesh, I am wondering if it is possible to optimize a spanner/wrench in hypermesh software (optistruct) and what would the constraints look like or how to apply one (normally there are no constraints acting on a spanner). I have attached the file along with this post.

Any valuable feedback would be welcome.

thanks

spanner1.hm

##### Share on other sites

It depends on the type of optimization you need to perform. For optimization you need to organize the geometry in to design and non-design space. The non-design space resembles the constraining area where no design changes takes place.

Have a look at the e-book about Optimization in which it is explained in detail. ( https://altairuniversity.com/free-ebooks-2/free-ebook-practical-aspects-of-structural-optimization-a-study-guide/)

Also refer OptiStruct online help where you will get tutorials on optimization.

##### Share on other sites

Hi,

I tried optimizing but i am getting an error

*** ERROR # 2150 ***
Invalid Volume or Mass Constraint.
The response type is the total VOLUME.
the upper bound value = 2.6100e+006
the total volume = 8.7003e+006
the design volume = 5.1900e+006
the total mass = 6.5252e-002
the design mass = 3.8925e-002
The design material fraction (percent) should be at least 3 times
the DOPTPRM MINDENS (default 0.01).

Could someone help me solve this error.

##### Share on other sites

Hi,

this error is due to an invalid total volume constraint.

Quote

the upper bound value = 2.6100e+006
the total volume = 8.7003e+006
the design volume = 5.1900e+006

The non-design volume is 3.513e+006, which is more than the upper bound value of 2.6100e+006, resulting in a negative volume of -0.903e+006 available for optimization.

Using mass or volume fraction will ensure valid positive mass/volume formulation.

The model you have shared had some issues. I have remeshed the part and scaled it to 1/10th the size, which I think is more consistent with the loading and material units.

spanner2_edit.hm

iwinphilip likes this

##### Share on other sites

Hi Ivan

Thanks for the help. Would it be possible if you can share the steps you used for future reference.

kind Regards

##### Share on other sites

Hi Ivan

I guess the file "spanner2_edit.hm" file has not been attached since i cant download it.

##### Share on other sites

Hi,

glad to help. The steps are:

Geometry:

• Geom>autocleanup
• F11 (quick edit geometry) for manual defeaturing used toggle edge, replace point and add/remove point
• Geom>solid edit>trim with lines>with bounding lines for partitioning
• Tools>scale>uniform

Meshing:

• F12 (automesh)>QI  optimize>trias + meshing criteria
• 3D>tetramesh>Tetra mesh>Float trias/quads to tetra mesh
• F2 delete the shell elements on solid faces (use mask panel or browser to isolate only 2D elements)
• F10 check elements>3D
• inspect how the mesh conforms to geometry. Use shift+F7 to project nodes to geometry
• shift+F11 to organize elements into design/non-design components
• 1D>rigids to create rigid spiders

• constrain master node of a rigid spider on one end with Analysis>constraints
• define load on master node of a rigid spider on the other end with Analysis>forces in a separate load collector
iwinphilip likes this

##### Share on other sites

Hi Ivan

Is there any other way i could contact you directly if I need any help

Kind regards Iwin

##### Share on other sites

I prefer the open forum so others can benefit from it.

But if there is something that can only be discussed privately you can contact me through email

iwinphilip likes this

##### Share on other sites

Thanks, I am completely new to this software and probably may need a lot of guidance from you.

Simon Križnik likes this

##### Share on other sites

You're welcome. There are some great learning materials from Altair university- Practical Aspects of Finite Element Simulation is a good starting point.

Altair University

Altair India Student Contest

ELEATION By Apoorv Bapat

iwinphilip likes this

##### Share on other sites

how did you edit the volume of the model by using scale (1/10th) depending on load and force.

Could you provide the steps and whether this has to be done at the very beginning or later stage.

Thanks

##### Share on other sites

by using Tool>Scale>uniform

Tips:

• you can find various functionalities with ctrl+f then type in the keyword(upper right corner)
• F1 or H for help while working in any panel

1/10th scale was arbitrarily chosen. Make sure to scale according to your data. Note the model units consistency is N, mm, tonne, MPa.

Scaling can be done at any stages, but it is a good practice to get the geometry right from the start to avoid confusion.

##### Share on other sites

Hi Ivan

I created another model and tried to run  but when i run i still get the same error. (all units are in  N, mm, tonne, MPa﻿.)

*** ERROR # 2150 ***
Invalid Volume or Mass Constraint.
The response type is the total VOLUME.
the upper bound value = 3.6295e+004
the total volume = 1.2098e+005
the design volume = 8.6894e+004
the total mass = 9.0737e-004
the design mass = 6.5171e-004
The design material fraction (percent) should be at least 3 times
the DOPTPRM MINDENS (default 0.01).

So I did calculate manually Non-Design Value =  the total volume -  the design volume

=   1.2098e+005 - 8.6894e+004 = 34086 which is less than the the upper bound value = 3.6295e+004.

Formulation for volume fraction:

Volume fraction = (total volume at current iteration – initial non-design volume)/initial design volume

I took 30% of volume as upper bound

Volume fraction = (3.6295e+004 - 34086)/1.2098e+005 = 0.01825

Could you correct me if i am wrong in my calculation with an example and point out where I had made the mistake and if such mistake occurs in the future how to resolve the issue.

I have attached the model  along with this file. Kindly let me know if I have done any other mistakes.

please note this is what I considered

moment = 50000n/mm

length = 240mm

force = moment/length

force = 208N

Kind Iwin Philip

##### Share on other sites

Even though the volume available for optimization is positive, it is still below

Quote

The design material fraction (percent) should be at least 3 times the DOPTPRM MINDENS (default 0.01).﻿

MINDENS= Sets a lower limit on the amount of material that can be assigned to any design element. Extremely low values for this parameter can result in an ill-conditioned stiffness matrix.

(upper bound volume - non-design volume) / design volume > 3 x MINDENS

(3.6﻿295e+004 - 34086﻿) / 8.6894e﻿﻿+00﻿﻿4 0.025 < 0.03

Slightly increasing the upper bound volume or decreasing the MINDENS parameter (analysis>optimization>opticontrol) should work.

iwin_edit.fem

iwinphilip likes this

##### Share on other sites

Hi Ivan

Thanks I will try it out and let you know and any other error in the model and optimization you found out. Plus does the .fem file open in hyper works.

##### Share on other sites

Solver deck (.fem file) can be imported by File>import>solver deck

##### Share on other sites

Hi Ivan,

Thanks, Now I understood how the volume optimization works. I tried out and i get the result all the parameters have been satisfied but when I look at the iterations its all the same. I have attached a photo of it and also the file named "spanner1". Could you let me know why i don't get an optimized model.

spanner1.hm

##### Share on other sites

Hi,

here is how to post-process topology optimization results:

##### Share on other sites

Hi,

I do have a doubt why does it show  " No closed volume found " even though i checked everything and all lines are intact.

Iwin2.iges

##### Share on other sites

Solid>Bounding Surfaces cannot be executed, because the solid is already created.

Verify by going to Geom>solid edit panel and picking the solid. Also when in edit geometry mode (for example in the F11 quick edit panel) surface edges of solid objects are slightly thicker than surface edges not enclosing solid objects.

##### Share on other sites

Hi,

Thanks for that. Could you please help me out with how to do FEM analysis for this model. (the steps involved in this process)

Kind Regards

Iwin Philip

##### Share on other sites

Like mentioned before, I suggest you start with Free eBook: Practical Aspects of Finite Element Simulation (a Study Guide)

Altair University

Altair India Student Contest

ELEATION By Apoorv Bapat﻿

These tutorials might help:

First try to do it yourself and ask for help if you fail.

iwinphilip likes this

##### Share on other sites

Thanks a lot . I will have a look. But i did try out many forces and other possibilities but still not getting a model like what i wanted to as shown in the picture. the only result i am getting is the model without the red lines which i think is wrong. any valuable feedback/suggestions appreciated.

Kind Regards

sample.hm

##### Share on other sites

I am not at my HyperWorkstation so I will look into your model later in the weekend.

## 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.