Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here


Analysis of a 3D Truss Structure

Analysis of a 3D Truss Structure

Analysis of a 3D Truss Structure


How to apply boundary conditions to a 3D truss structure?

As shown in the attached pictures, all the structural members are pinned- connected. CROD element is used to model the truss members. The pink elements in the pictures represent cables. I fixed six DOF of eight bottom nodes: Grid Point 1-5 and 9-13 and NASTRAN can generate result but it shows the singularity of other grid points. The failed directions are three rotational DOF.

I also tried the case that six DOF of all the grid points except 6 and 16 are restrained, NASTRAN still shows singularity of Grid Point 6 and 16. How to remove the singularity?

RE: Analysis of a 3D Truss Structure

The Crod could not constrain rotation. You should manually constrain the grid point rotational dof or, use CBeam.

Normally, to model this kind of structures you should use CBeam for truss and crod for cables. In this way you will not have singularity.
If the trusses are pinned @ end point you could "pin flag" the extremity. consulte the Nastran qrg to how to do.

Next time you post a picture, please, use a jpg format, is much faster to download.

RE: Analysis of a 3D Truss Structure


Thank you for the quick reply, Onda.

"Pin flag" is used for CBEAM elements. The truss members I analyzed can only stand tension/compression. If I use CBEAM, how do I remove bending of all members?

If I constrain all the rotational DOF of grid points, the structure with CROD doesn't generate singularity.

RE: Analysis of a 3D Truss Structure

If you use Cbeam, to remove bending You should pin flag both end of beam. Pay attention that on each knot of the structure almost one beam should not been pin flagged else you have again singularity on grid point.

You can use Cbar and constrain the 4th 5th and 6th DOF of each grid point.

RE: Analysis of a 3D Truss Structure

I analyze a structure which consist a beam on the ground. I would like to constrain the beam in that way that it can be movable in positive Z direction but immovable in negative Z direction. (Z is vertical to the ground) How do I do that?

From Patran displacment constraint, I can only make it zero.

Thanks for any input!


RE: Analysis of a 3D Truss Structure

When I used Cbar and constrain the 4th 5th and 6th DOF of each grid point, the model will be solved.

But my question is that the structure is a 3D truss, some grid points might be able to rotate with respect to the original coordinate system. Or I can make the assumption that the members can only stand axial loads, so the rotational dof are zero.    

RE: Analysis of a 3D Truss Structure

Because CBar have no stiffness for rotational DOF you need to constrain the grid points on 4-5-6 using CBAR.
If you use Cbeam you don't have this problem

RE: Analysis of a 3D Truss Structure

Onda, CBAR elements provide stiffness in all six degrees of freedom.


RE: Analysis of a 3D Truss Structure

Johnohors you right i've confused Cbar e Crod. sorry

RE: Analysis of a 3D Truss Structure

Onda, no problem, (in my opinion bar and rod are not particularly good descriptive names anyway, they don't imply their differences within nastran)


RE: Analysis of a 3D Truss Structure

Johnhors, Onda,

Thank you for the reply.

I used CROD element to model the truss because the truss members can only hold tension and compression load due to the joint design.

If I constrain 4,5,6 DOF of each grid point, there is no singularity. My question is that "Is this a correct way to model 3D truss structure?" I have seen a lot of examples of 2D truss analysis, and usually some DOF are removed since it is a 2D problem. I am not sure about 3D truss problem.

RE: Analysis of a 3D Truss Structure

Dear Alin09,
I see the picture of you truss latice structure, and I can tell you that meshing lines with CROD elements the model will fail for sure, you have a mechanism in some portions of your model, basically where you have four bars without any diagonal, please note that CROD elements do not have rotation degrees of freedrom, them the structure will collapse.
And yes, truss structures are meshed with CROD elements because members are bolted, then pin joint is the normal configuration, but you will have to assure to form triangles, not quadrilateral shapes, then the structure will be stable. A typical design is to mix beam & rod elements: the bottom chords of the structure are meshed with beam/bar elements with 6 DOF per node.
This is basic.
Best regards,

RE: Analysis of a 3D Truss Structure


Thanks for the reply.
IF I constrain all the rotational DOF of all truss nodes, the problem can be solved and there is no singularity.

In reality, I don't need to form triangles of beams/rods to make the truss structure stable, some pretension cables can be used to make the truss stable. For example, the PINK color members are cables in the attached figure.

My question is I don't know if I correctly use CROD element of NASTRAN by restraining all the rotational DOF. For ANSYS, if ROD elements are used, I don't need to constrain rotational DOF and the strcutre can be solved.


RE: Analysis of a 3D Truss Structure

Dear Alin09,
The CROD element is the simplest element of all the elements that have geometry associated with them. While you can use a CBAR or CBEAM element to represent a rod member, these elements are somewhat more difficult to define because you must explicitly specify an element coordinate system. The CROD element is ideal when you need an element with only tension-compression and torsion.
You must issue PARAM,AUTOSPC,YES to automatically constraint rotational RY & RZ (DOF 4&5) on CROD elements, but please note you have torsional rotational DOF, if you let alone CROD elements without constraining the torsinal DOF then you will receive error of the type "RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL".
Solutions: you must restraint rotations on your constraints or use permanent nodal constraints on constrained nodes.

When solving a problem with CROD elements you will see the following output (NX nastran 7.0) in the *.F06:        
                                           F O R C E S   I N   R O D   E L E M E N T S     ( C R O D )
       ELEMENT           AXIAL                                     ELEMENT           AXIAL
         ID.             FORCE          TORQUE                       ID.             FORCE          TORQUE
             1        3.726764E+03   0.0                                 2        3.726764E+03   0.0
             3       -7.453560E+03   0.0
1    NX NASTRAN STATIC ANALYSIS SET                                                                                             
                                     S T R E S S E S   I N   R O D   E L E M E N T S      ( C R O D )
         ID.        STRESS       MARGIN        STRESS      MARGIN         ID.        STRESS       MARGIN        STRESS      MARGIN
             1    4.658455E+02              0.0                               2    4.658455E+02              0.0           
             3   -9.316950E+02              0.0           

Best regards,

RE: Analysis of a 3D Truss Structure


Thank you, Blas!

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close