how to apply displacements as BCs?

Rahul_P1

Hello,

I am simulating a three point bending test, and want to apply a displacement of 20 milimeters in the z direction to two nodes in the probe's central line as initial condition.

The goal is to check the force needed to obtain such strain.

I have tried using SPC and SPCD cards, but all I obtain is an undeformed shape after the simulation. When I use an arbitrary force instead of a displacement, the results come as expected, though.

I uploaded the .hm file with BCs and forces and the .hm file with displacement.

Thank you in advance

Gustavo Blazek

Rahul_P1

Hi Gustavo,

Irrespective of the use case, I am just wondering about the way you have defined the enforced displacement.

Note that the degree of freedom referenced on SPCD must also be referenced on a SPC or SPC1 bulk data entry and selected by the SPC subcase information command,
So you need to create a SPC load collector and constrain the DOFs specified in SPCD in this SPC collector,
Then Reference SPCD card in LOAD subcase, and SPCs in SPC subcase.

See comment 1 in the help document - Altair OptiStruct > Reference Guide > Input Data > Bulk Data Section:
SPCD
The degree-of-freedom (G and C) referenced on this entry must also be referenced on an SPC or SPC1 bulk data entry and selected by the SPC subcase information command in the same subcase.

Rahul_P1

Hi Rahul,

thank you very much for your prompt reply and valuable help. Earlier I had set the displacement only as SPCD and referenced it in a LOAD subcase.

It works as wished now, thank you very much again.

Regards,

Gustavo Blazek

Altair Forum User

I am having similar issue and I have not been able to resolve it. Please, find my attached hm file. I want to apply x displacement of 1 and y displacement of 1 to the left bottom node of the model. I got this error:

 

*** ERROR # 186 ***
 An SPCD component must be constrained by an SPC or SPC1 data.
      GRID ID = 22
    component = 1
  LOAD set ID = 3
   SPC set ID = 1
   subcase ID = 1

 

Rahul Ponginan

 

Maybe I don't understand this:

Note that the degree of freedom referenced on SPCD must also be referenced on a SPC or SPC1 bulk data entry and selected by the SPC subcase information command,
So you need to create a SPC load collector and constrain the DOFs specified in SPCD in this SPC collector,
Then Reference SPCD card in LOAD subcase, and SPCs in SPC subcase.
See comment 1 in the help document - Altair OptiStruct > Reference Guide > Input Data > Bulk Data Section:
SPCD
The degree-of-freedom (G and C) referenced on this entry must also be referenced on an SPC or SPC1 bulk data entry and selected by the SPC subcase information command in the same subcase.

 

Also, where can I access Altair Opstistruct Reference guide? Thank you.

 

Unable to find an attachment - read this blog

Altair Forum User

Everybody,

there is no need to use SPCD at all for enforced displacement.

It is sufficient to use SPC only and enter the requested displacement directly there.

 

samuel88:

You can find the Reference Guide in the Online Help.

Hypermesh > Help > HyperWorks Help Home > (See Welcome Page down below) Reference Guides > OptiStruct

 

Regards Juergen

 

Altair Forum User

Juergen Kranzeder

Prakash Pagadala

@tinh

Rahul Ponginan

 

 

See the figures below:

 

I applied three different displacement boundary conditions, one at each node on my model. When I ran the analysis, I realized that the result is not giving the aggregate effect of all the displacements. Rather, it gives the analysis for each displacement boundary condition as each subcase. Kindly help me check the attached model (hm file) and indicate what I am doing wrong. My goal is to see the overall effect of applying three displacement boundary conditions and a fixed boundary condition, as shown on the model. Thank you.

 

<?xml version="1.0" encoding="UTF-8"?>

 

<?xml version="1.0" encoding="UTF-8"?>

 

Unable to find an attachment - read this blog

Altair Forum User

I got it. Thank you.

 

 

Altair Forum User

Prakash Pagadala

 

I have 2D model in hypermesh and hyperwork. I need to obtain the perimeter of the geometry and the coordinates which I can use to create the same geometry in MATLAB.
 
Kindly advice me on how to:
1. Obtain the perimeter of a 2D geometry in  hyperwork and hypermesh
2. Extract the coordinates that create the 2D geometry in hyperwork and hypermesh.
 
Thank you.

Altair Forum User

Hi @samuel88

 

You can select the elements on the perimeter and use Tools page>> Masscalc>> Area to calculate area

jsk459

Hi @Prakash Pagadala  

 

If i want to apply the velocity to the body, how can i use SPCD load collector, since it is only defining enforced displacement ?

Altair Forum User

Hi,

 

What type of analysis are you trying to work on?

 

Velocity and acceleration are dynamic loads and it is not possible to apply in a linear static subcase. 

 

 

jsk459

Is it possible to do the LsDyna - Explicit dynamics analysis into the optistrct module ?

Altair Forum User

Hi,

 

Instead, use RADIOSS.