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


4 Point Bend on an L Shaped Specimen

4 Point Bend on an L Shaped Specimen

4 Point Bend on an L Shaped Specimen

Hi Everyone,

My final year project involves modeling a 4 point bending on an L shaped specimen (only elastic). I am new to Abaqus, I have only used Solidworks simulation before. I am using Abaqus 6.14.
I used the instructions provided in this video to set up my FE model:
I had to tweak it a little bit as this video is for 3 point bending test. I also used a rotated CSYS for all of my boundary conditions. I am not really sure where I went wrong. Can someone give me directions or tips?
You can download the model using this link:


After submitting my simulation, I received these warning messages:

A transformed coordinate system has been used for node 1 (assembly) which is included in an *equation. However, no active dofs were detected at this node, possibly because the node is not connected to any element. If this situation occurs in an implicit dynamic procedure (*dynamic), it may lead to an inconsitent number of dofs between the fe mesh and the solver and the analysis being terminated. To avoid this situation, please make sure that a point mass and rotary inertia are defined at this node for activating needed translational and rotational dofs.


Boundary conditions are specified on inactive dof of 675 nodes. The nodes have been identified in node set WarnNodeBCInactiveDof.

There are 2 unconnected regions in the model.

Your help is much appreciated.

RE: 4 Point Bend on an L Shaped Specimen

In Abaqus warnings do not always mean something worrying. Pretty much every complex simulation generates them and most of them can be ignored. But of course it's always recommended to read and understand all warning messages. In your case I think that they don't indicate any serious problem unless the results look incorrect.

RE: 4 Point Bend on an L Shaped Specimen

Could you also attach .inp file ? RF output variable means reaction forces in Abaqus. It will only appear in the regions of the model where boundary conditions are specified. There might be an error in your BCs definition. Personally I would use different approach than shown in the video in this case - try modeling all rollers (including bottom ones) as rigid bodies, assigning all BCs to them and defining contact (pairs or general contact - both should work fine).

RE: 4 Point Bend on an L Shaped Specimen

Thank you for your advice, I followed it. I also moved the top two pins down using a boundary condition instead of the reference point method. It seems to work. Although, there is an interesting phenomenon that I don't understand what's causing it. As you can see on this picture, the bottom pin penetrates the specimen but I don't really know why. I used the same interaction settings & properties for all the pins. Any tips on what is causing this penetration? or is this just an incorrect plotting?

RE: 4 Point Bend on an L Shaped Specimen

In the meantime I checked your CAE model. There was an error in the definition of BC driving reference point. It was specified in wrong direction. But after fixing this another problem appeared - pins were penetrating the specimen. I tried various improvements of contact definition and what finally helped was applying small overclosure between each pin and beam and then turning on „Adjust only to remove initial overclosure” option. That’s because the angle between pin and beam was such that it was hard for Abaqus to establish contact. I think that you should try it with your model too. It should work but if the problem still exists try changing contact behavior, adding whole surface of the pin to contact pair definition and changing your model to meet requirements for master and slave surface. Also consider assigning rigid body constraint to the pins.

RE: 4 Point Bend on an L Shaped Specimen

Thank you for your guidance. It is much appreciated. I tried to follow your advice and I couldn't make it work. I used a different approach which seems to give me a better result than I got yesterday. However, the penetration at the lower pins are still present. I tried to assign rigid body constraint on the bottom pins but the simulation got aborted.
I attached my latest setup.
Can someone have a look at my setup and give me advice on this penetration issue?


RE: 4 Point Bend on an L Shaped Specimen

If you use this trick with strain-free ajustment that I described before on your previous model (the one with two pins) and make the pins rigid (using Rigid body constraint) then it should work fine. I did this and got good results. Apart from that I think that it’s better to apply BCs to pins through points like you did before instead assigning them to whole part.

RE: 4 Point Bend on an L Shaped Specimen

Thank you for help. It works fine now :)
I have another question...
How can I export the principal stresses which occurs at each node on the top surface of the specimen?

RE: 4 Point Bend on an L Shaped Specimen

Abaqus calculates stresses at integration points (there they are the most accurate) so you can’t request nodal stresses as history output but they can be interpolated from integration points in postprocessing. There’s more than one way to extract nodal stress values. First create a display group containing only these nodes that you want to evaluate for principal stresses - use Create Display Group, select Nodes as Item and Pick from viewport as Method. Choose by angle and click on the top surface of the beam. Click Done and in the Create Display Group window choose Save Selection As... Then specify a name for this group and confirm. Close the display group creation window. Switch to Plot Undeformed Shape, find Display Groups container in the Results tree on the left, expand it and double click on the name of previously created display group. Use Common Plot Options —> Labels —> Show node symbols to visualize nodes in the selected display group. Now there are two ways to extract stresses from these nodes:
1) use Report —> Field Output, select Unique Nodal, check boxes next to proper principal stress variables and click OK to write them to file
2) use Query —> Probe Values, switch to Nodes, choose Select a display group and pick the one previously created (before doing this you have to select one of the four principal stress variables (max, max(abs), mid or min) so that the probe values tool extracts proper output variable), wait until it collects the data and click Write to File...

The second method is much longer since not only it collects the data slowly node by node but you also have to pick principal stresses one by one. Thus I recommend the first approach.

Apart from this you could also use scripting but in this case it’s not necessary.

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! Already a Member? Login


eBook - Rethink Your PLM
A lot has changed since the 90s. You don't surf the Web using dial-up anymore, so why are you still using a legacy PLM solution that's blocking your ability to innovate? To develop and launch products today, you need a flexible, cloud-based PLM, not a solution that's stuck in the past. Download Now
White Paper - Using Virtualization for IVI and AUTOSAR Consolidation on an ECU
Current approaches used to tackle the complexities of a vehicle’s electrical and electronics (E/E) architecture are both cost prohibitive and lacking in performance. Utilizing virtualization in automotive software architecture provides a better approach. This can be achieved by encapsulating different heterogeneous automotive platforms inside virtual machines running on the same hardware. Download Now

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