Smart questions
Smart answers
Smart people
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Member Login




Remember Me
Forgot Password?
Join Us!

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips now!
  • 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!

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

Donate Today!

Do you enjoy these
technical forums?
Donate Today! Click Here

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.
Jobs from Indeed

Link To This Forum!

Partner Button
Add Stickiness To Your Site By Linking To This Professionally Managed Technical Forum.
Just copy and paste the
code below into your site.

CommissarHolt (Aerospace) (OP)
7 Sep 09 16:32
Hello everyone,

I am trying to calculate the max deflection U2 of a 3D cantilever beam of square cross-section with a load at the free end.  I have completely constrained the fixed end and placed concentrated forces on the top nodes of the free end.  To keep the beam from bending along the z-axis, I constrained the element at the free end between the top nodes to deflect only in U1 and U2.  However, the deflection results in ABAQUS are over one order of magnitude less than those based on the cantilever beam deflection formula.  What is the reason behind this discrepancy?

-Tom      

corus (Mechanical)
8 Sep 09 3:22
Could be umpteen things. A common mistake I've seen is to apply a force in terms of Kg and not in Newtons. The difference is about 10 times.  

corus

CommissarHolt (Aerospace) (OP)
8 Sep 09 16:53
Sorry, there's a typo in my previous post.  The ABAQUS deflection results are over one order of magnitude greater than those based on beam deflection theory (I  must have been thinking I needed the ABAQUS results smaller as I was writing that statement).  

Corus: I don't think applying the force in kg instead of N is the reason for the discrepancy.  I used a 1000N force in my theoretical calculations.  When I performed the 2D deflection analysis in ABAQUS, I specified a -1000 load in U2 which gave me a result with a relative error of 1.5%.  I did the same thing for the concentrated forces in my 3D analysis.
Helpful Member!  DanStro (Mechanical)
8 Sep 09 17:22
Did you divide the load by the number of nodes you are applying it too?
CommissarHolt (Aerospace) (OP)
8 Sep 09 21:31
No.  I placed a 1000N load on each of the two nodes.
Helpful Member!(3)  johnhors (Aerospace)
9 Sep 09 2:34
Then you have applied 2000N load in total!


www.Roshaz.com

DanStro (Mechanical)
9 Sep 09 9:22
That has burned me a few times too. If you have N nodes then you need to apply a force of (total Force/N) to each.

Dan
johnhors (Aerospace)
9 Sep 09 9:49
Dan,

Be careful, very careful doing that! Spreading a load out over a number of nodes in this manner is not the same as applying a uniform pressure, regardless of whether you have a uniform mesh on a simple square or rectangular area or not. When available in either the pre-processor of your choice or the input deck itself, always apply a pressure instead.

Why? Because a uniform pressure will correctly honour the shape/displacement functions and geometry of each element face, whilst point loads at each node on the surface will not.

Think of it as the difference between lying on a water bed as opposed to lying on a bed of nails.


www.Roshaz.com

CommissarHolt (Aerospace) (OP)
9 Sep 09 13:04
By George, it worked!  I specified a 500N load for each node and got a result with only 0.25% error.

Quote:

Be careful, very careful doing that! Spreading a load out over a number of nodes in this manner is not the same as applying a uniform pressure, regardless of whether you have a uniform mesh on a simple square or rectangular area or not. When available in either the pre-processor of your choice or the input deck itself, always apply a pressure instead.

Why? Because a uniform pressure will correctly honour the shape/displacement functions and geometry of each element face, whilst point loads at each node on the surface will not.

I can see why applying a pressure load would lead to a more accurate analysis than a series of point loads.  However, selecting the Pressure load type in ABAQUS only lets me apply it to the surface and not a line of a 3D object.  Is there another load type I could use to achieve the desired effect?  I tried using a Line load but instead of selecting the top edge of the free end cross-section, ABAQUS selects all the edges in the beam.  
 
corus (Mechanical)
9 Sep 09 14:14
You should be able to select that individual line, but then again I think Abaqus simply applies the load equally to all nodes. If you're applying the load to an edge of linear brick elements then the load at the corner node should be half that of the adjacent internal node. So proportionately the loads should be in the ratio of 0.5, 1, 1, ... 1, 0.5
You can however partition the surface to leave only a small area in which to apply a pressure load. Bear in mind that the analysis is only accurate if it models accurately the real world situation. Loads are rarely applied as point loads in real life, other than perhaps by contact, and even then that is over a small area.
 

corus

DanStro (Mechanical)
9 Sep 09 14:28
johnhors, you're right. I very rarely use point loads, that is probably why I keep getting burned when I do, so I completely forgot about that.

Thanks.
johnhors (Aerospace)
9 Sep 09 14:45
CommissarHolt, with a 3D model of the cantilever it would be best to apply your load as a traction (in-plane) pressure smeared over the end face area.

Trying to apply loads spread over a line in 3D is no better than applying point loads, since the line has no physical width and hence no physical area. Thus rather than applying load at the point of a nail, you have merely transferred it to a knife edge.


www.Roshaz.com

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