Forum Jar
Forum Jar : Abaqus Forum : Inability to set SECTION=ELBOW for elbow elements in Abaqus CAE 6.11-3
See other topics in Abaqus Forum

Abaqus Forum
Important rules for using Abaqus Forum
• No offensive words are allowed in this forum.
• To prevent spams, you must not use the words "http" ".com" or "/"(slashes) in this forum.

Alert! Please do not buy anything or pay anyone on this forum. Scammers have been reported on our forum. Please also do not go to any links posted on here. We have been reported about links to websites that contain viruses. Thank you.

Topic: Inability to set SECTION=ELBOW for elbow elements in Abaqus CAE 6.11-3

I would like to model a simple pipe structure with any of the elbow elements available in Abaqus, for instance the beam element ELBOW31. In the Mesh module I successfully assign ELBOW31 as Element Type but it is also needed to assign an elbow section in the Property module. The problem is that when I create a Beam section in the list with the profiles I do not see "Elbow". In Abaqus Keywords Reference Manual for Beam Section it says "Set SECTION=ELBOW for elbow elements, which are available only in Abaqus Standard.". In my version Abaqus CAE 6.11-3, Abaqus Standard in the product employed in the simulation process so I don't understand why I can't see Elbow as an available cross section profile for beam elements?

Can you give me a clue how could I employ elbow elements in my analysis?

Thank you for the help in advance!

Yordan Venev

by Yordan Wed Aug 07 15:06:30 UTC 2013

Hello again,

I got to know the solution for the problem I had.
An Elbow section cannot be specified in CAE. That’s why do so: specify the beam as a pipe-section in CAE. Then you have to write out the inp-file from CAE using:
Job -> Write input
Then you get a inp-file that you can edit like:
** Two, or more, asterix give a comment line.
***Beam Section, elset=_PickedSet2, material=steel, temperature=GRADIENTS, section=PIPE
*Beam Section, elset=_PickedSet2, material=steel, temperature=GRADIENTS, section=elbow
Data line 1
Data line 2
Where according to the Abaqus 6.11 keyword manual *Beam section:
Data lines for ELBOW sections:
First line:
1. Outside radius of the pipe, r.
2. Pipe wall thickness, t.
3. Elbow torus radius, R, measured to the pipe axis. For a straight pipe, set .
This value is not written for the Pipe-section so it have to be added.
Second line:
Enter the coordinates of the point of intersection of the tangents to the straight pipe segments
adjoining the elbow, or, if this section is associated with straight pipes, the coordinates of a
point off the pipe axis. The second cross-sectional axis will lie in the plane thus defined, with
its positive direction pointing toward this off-axis point.
1. First coordinate of the point.
2. Second coordinate of the point.
3. Third coordinate of the point.
( Also use:
*Preprint, echo=NO, model=YES, history=YES, contact=NO
So that you can look in the dat-file that all detailed input that is written there is what you specified. )
After you have made these change save the inp-file under a new name and then run Abaqus using:
abaqus job=new_name
abq6113 job=new_name

Best regards,
Yordan Venev

by guest Thu Aug 15 11:34:05 UTC 2013

by Tue Nov 28 03:51:47 UTC 2017
Post a new comment

Name (optional):

By posting a comment, you indicate that you have agreed to our terms of use.

Feel adventurous? Check out random forums on Forum Jar!
Related Forums
Commercial software Forum
Finite element analysis Forum
Dassault Systemes S.A. Forum
Open-source Forum
Python (programming language) Forum
Fox-toolkit Forum
GUI Forum
Automotive industry Forum
Aerospace Forum
Industrial product Forum
Multiphysics Forum
Piezoelectric Forum
Elastomer Forum
ABAQUS, Inc Forum

sponsored links: free polls | free chat rooms (weirdtown chat) | widgets for myspace | make chat room | free chat room list | review websites | snowboard or ski | chat vocab

terms of use | privacy policy
©2018 All rights reserved.