• Registered: 09-12-2015
  • Posts: 54

Topic: Help! we have questions in adding forces.

Hi all, I use oofem to do the LinearStatic analysis. As case1.png shows, I use TrPlaneStress2d  as element,  fix the bottom, and add a 100N force in the top.  How  could I add the 100N force?

Now we are using the NodalLoad, fro example, if the top edge have 50 points, we set NodaLoad as 100N/50= 2N。Is this correct? I doubt because we have thickness, so the points number is not true, and the result is about 3 time less than the Abaqus software results both in displacement and stress.

Post's attachments

case1.png 284.41 kb, file has never been downloaded. 

You don't have the permssions to download the attachments of this post.
  • Registered: 09-12-2015
  • Posts: 54

Re: Help! we have questions in adding forces.

This is my oofem input file.

Post's attachments

case1_Holes_10_a3.in 233.07 kb, 5 downloads since 2017-04-04 

You don't have the permssions to download the attachments of this post.
  • Registered: 25-06-2013
  • Posts: 241

Re: Help! we have questions in adding forces.

You can simply check the applied force by summing the reactions which gave me in your case something about 300. Your approach would be almost correct in a case wth the same size of elements, but in your case, I would use element edge load instead.

  • Registered: 09-12-2015
  • Posts: 54

Re: Help! we have questions in adding forces.

Thank you for your good answer! Now I use your edge load method instead. The attachment is my current input file.

However, I still have a question is that the force size I should set in my oofem input file. Suppose I have 31 short edges in the top and I want to add an 100N force from the top. How should I set the force size? Is 100N or 100N/31=3.226N? And as the http://www.oofem.org/resources/doc/oofe … ode52.html says, I doubt which loadType I should set. Could you give me an advice?

Post's attachments

case1_Holes_10_a3.in 218.97 kb, 3 downloads since 2017-04-05 

You don't have the permssions to download the attachments of this post.
  • Registered: 09-12-2015
  • Posts: 54

Re: Help! we have questions in adding forces.

The physical force condition is as the attachment photo shows.

Post's attachments

physical.png 654.19 kb, file has never been downloaded. 

You don't have the permssions to download the attachments of this post.
  • Registered: 21-09-2017
  • Posts: 16

Re: Help! we have questions in adding forces.

Hello! I also have a question in load. I attach 2 point loads and  own weight in the plate thickness 25 cm.  after the calculation as a result, not all the points are marked and the value of -nan (ind) is not true. Help  me please!  My in file attached

Post's attachments

plita_OOFEM.in 138.67 kb, 3 downloads since 2017-10-05 

You don't have the permssions to download the attachments of this post.

7 Reply by kuzovleva (edited by kuzovleva 05-10-2017 07:16:24)

  • Registered: 21-09-2017
  • Posts: 16

Re: Help! we have questions in adding forces.

plate picture https://drive.google.com/drive/folders/ … WVRVDhYUW8

  • Registered: 27-09-2017
  • Posts: 14

Re: Help! we have questions in adding forces.

Edge loads are specified with units of force/length. If you want a force of 100N, and the contact length on the top edge is 25mm for example, you would specify 4 (N/mm) or 4000 (N/m) depending on your unit system.

9 Reply by bp

  • bp
  • Administrator
  • Offline
  • From: Prague, Czech Rep.
  • Registered: 02-03-2007
  • Posts: 1,026

Re: Help! we have questions in adding forces.

Hi Olga,
the solution fails ( I refer to your post from Oct 5th), as you have several nodes at the same position  (like nodes 53 and 518). Node 53 is not connected to any element, there is no stiffness and thus it can move arbitrarily. You have to merge duplicated nodes or support the free node.
Note that there are other duplicities (node 846 and 54) and (52 and 754) and perhaps some others.

You solve plane stress problem, this is 2D problem in xy plane, you could not apply load in z direction. To do this, you have to switch from plane stress to 3D shells,for example.

Borek

bp's Website

10 Reply by kuzovleva (edited by kuzovleva 10-10-2017 12:27:44)

  • Registered: 21-09-2017
  • Posts: 16

Re: Help! we have questions in adding forces.

I changed the grid and removed duplicate and free nodes. Now she looks like this. My Ctrl file:
plita3.out
This unv file to OOFEM input file.
LinearStatic nsteps 1 nmodules 1
vtkxml tstep_all domain_all primvars 2 1 4 vars 4 4 1 42 21  stype
domain 3dShell
OutputManager tstep_all dofman_all element_all
ncrosssect 1 nmat 1 nbc 3 nic 0 nltf 1
SimpleCS 1 thick 0.25 
isole 1 d 2.5 e 3059 n 0.25 tAlpha 0.00001
BoundaryCondition 1 loadTimeFunction 1 prescribedvalue 0.0
NodalLoad 2 loadTimeFunction 1  Components 6 0 0 -4 0 0 0
NodalLoad 3 loadTimeFunction 1  Components 6 0 0 -8 0 0 0
ConstantFunction 1 f(t) 1.0
group conc
elemprop mat 1 crosssect 1
etype[41] TrPlaneStress2D
etype[44] PlaneStress2D

group LC1
nodeprop bc 6 1 1 0 0 0 0 load 1 2

group LC2
nodeprop bc 6 1 1 0 0 0 0 load 1 3

group N1
nodeprop bc 6 1 1 1 0 0 0.
But the result is not true.
excerpt out file:
  GP  1.1  :  strains  -nan(ind) -nan(ind) 0.0000e+00 0.0000e+00 0.0000e+00 -nan(ind)
              stresses -nan(ind) -nan(ind) 0.0000e+00 0.0000e+00 0.0000e+00 -nan(ind)
I really need to figure this out!

11 Reply by bp

  • bp
  • Administrator
  • Offline
  • From: Prague, Czech Rep.
  • Registered: 02-03-2007
  • Posts: 1,026

Re: Help! we have questions in adding forces.

Hi, could you provide your input file?

bp's Website

12 Reply by kuzovleva (edited by kuzovleva 11-10-2017 06:55:46)

  • Registered: 21-09-2017
  • Posts: 16

Re: Help! we have questions in adding forces.

Hello! I put in file https://drive.google.com/drive/folders/ … WVRVDhYUW8
I understand, that my system geometrically variable now, but don't understand,what degrees of freedom  must be for geometrically invariability.

Olga

  • Registered: 25-06-2013
  • Posts: 241

Re: Help! we have questions in adding forces.

Hi,

I think the problem is that you are using 2d plane stress elements in x-y plane, but you are loading them in the z direction.
Can you explain what you want to simulate? A working example is attached, but it might be different from what you want.

Martin

Post's attachments

plita3.in 5.96 kb, 2 downloads since 2017-10-11 

You don't have the permssions to download the attachments of this post.

14 Reply by kuzovleva (edited by kuzovleva 12-10-2017 12:53:41)

  • Registered: 21-09-2017
  • Posts: 16

Re: Help! we have questions in adding forces.

Hi. Of course, this is my mistake: you need to use 3d elements (the bending task of the plate and the load in the z  axes). Then for triangles element I use cctplate3d? And what about quadrangles elements?
Now I have mesh  with  only triangles elements and make in file with cctplate3d, but not good result
the task  and in file this... https://drive.google.com/drive/folders/ … WVRVDhYUW8 (can't add file in attachment)where there could be another mistake?

Olga

15 Reply by bp

  • bp
  • Administrator
  • Offline
  • From: Prague, Czech Rep.
  • Registered: 02-03-2007
  • Posts: 1,026

Re: Help! we have questions in adding forces.

Hi,
the cct3d element is just a plate element, even transformed to 3D, so it defines only three DOFs (disp_z, rot_x, and rot_y in xy plane). So for example, you have not prevented rotational DOF around z axis in every node. Much better solution is to use full shell elements, that provide stiffness for all 6 DOFs - see modified input attached. I have made some additional changes in vtkexportmodule to export only quantities defined for shell element.

Post's attachments

plita3.in 153.76 kb, 2 downloads since 2017-10-12 

You don't have the permssions to download the attachments of this post.

bp's Website

  • Registered: 21-09-2017
  • Posts: 16

Re: Help! we have questions in adding forces.

Hi. thank you very much! YOU helped me a lot!