Bolted connection

Dear Folks

I’m working on an assembly with many bolted connections, it is easily performed using NX, NX enables me to easily specify the bold-head and nut diameters, and adjust the mesh to have notes along the bolt-head and nut circles.

I want to model bolted connections using the “beam” connection in Ansys Mechanical 2019R3. When I set the “Behavior” to “Deformable”, the following fields appear for each end of the beam connection: “Pinball Region”, “Material”, “Diameter”. So my questions are:

image(1) Is the beam connection in Ansys 2019R3 a correct means of modeling bolts?

(2) Assuming the answer is yes, What are the “Pinball Region”? Should I set them to the diameters of bolt-head and nut?

(3) There are 3 beam materials and diameters! One for the beam connection, and one for both ends! Is this a bug in Ansys?


  • peteroznewmanpeteroznewman Member
    edited February 9

    I am familiar with NX11 Pre/Post Bolted Connection, which I agree is quite easy to use.

    In ANSYS, if you right click on the Connections folder and insert a Beam Connection, that is similar to what NX does. The Radius is the radius of the bolt shank and the material is the material of the bolt shank. I don't see three materials.

    Leave the Pinball Region set to All.  I expect you have made a face with the diameter of the washer or nut or bolt head, so all the nodes on that face will get a spider of Connection Elements like an NX spider of RBE elements.

    You get to choose in ANSYS if you want Deformable or Rigid behavior of the Connection Elements to those nodes. Rigid is the default Behavior.

    You can add a Bolt Pretension load to this Bolted Connection.

    NOTE: Ansys also has Bonded Contact. There are many formulations for this and one of them is Beam. This seems to be similar to the Beam Connection, but you can't add Bolt Pretension loads.

  • GeorgeAerospaceGeorgeAerospace EgyptMember
    edited February 9
    How to simulate the washer and nut??
    What is the meaning of pinball and behavior??
  • peteroznewmanpeteroznewman Member
    edited February 9

    Instead of using a Beam Connection, you can have an actual solid body bolt and solid body nut. The bolt head can be at the diameter of the washer. It can have either Bonded Contact to the flange it is clamping, or it can have Frictional Contact to the flange.  The bolt shank can have a Bolt Pretension load.

    Pinball is a search radius from one node to decide if another node should be included in the contact definition or not.

    Behavior is how the Connection Elements behave. They can be Rigid or Deformable. That is like RBE2 and RBE3 in NX NASTRAN.


  • GeorgeAerospaceGeorgeAerospace EgyptMember
    edited February 11

    Dear sir

    Sorry if I was not clear. Please allow me to clarify.

    As you can see in the screenshot, for the Reference body, when I set the "Behavior" to "Beam", a new "Material" and "Radius" appear. The same thing occurs for the "Mobile" body. So I end up with 3 materials and 3 radii.

    So my questions are as follows:

    1) What is the difference between the three materials and radii? Or this is a bug in Ansys?

  • peteroznewmanpeteroznewman Member
    edited February 11

    When you have a Beam Connection, a beam element is created from an end point on one side at the center of the selected geometry, to an end point on the other side. This is like the shaft of an actual bolt where you can specify the radius and material.

    ANSYS gives you the option to run beam elements from the end point of the bolt shaft to the nodes on the surrounding geometry. It is not a bug, but I don't use that feature. I use Rigid or Deformable for Behavior to get RBE3 or RBE2 type MPC connection equations from those end points out to the nodes on the selected geometry (face or edge).

  • GeorgeAerospaceGeorgeAerospace EgyptMember
    edited February 15

    Thank you for your response, but forgive me I didn't understand it fully;

    You said that when I set the "Behavior" to "Beam", ANSYS runs beam elements from the bolt end point of to the the surrounding nodes. Then you said that you use "Rigid" or "Deformable" behaviors to get MPC connection from the bolt end points to the surrounding nodes.

    That is, all the "Beam", "Rigid" and "Deformable" behaviors do the same thing. Did I understand you correctly? You didn't explain the difference!

    I'm so sorry, but I still cannot understand what is the difference between the three materials and radii? Can the bolt be steel on one end, and aluminum at the other end and in the same time it is brass???

  • peteroznewmanpeteroznewman Member
    edited February 16

    Do you recognize the Swiss knife gadget in the image below?
    It has many useful tools if you use them one at a time.
    But if you pull them all out at once, it is absurd to try to use it.

    ANSYS is like that Swiss knife gadget.
    It has many useful tools, but you can make an absurd model if you pull out too many tools, as you have suggested above.

    Here is a tutorial showing a Solid Body representation of a bolted joint. This is the most detailed and accurate method of representing a nut and bolt connection, but it is also the most time consuming to build and solve.

    A simpler representation is to delete the Nut and Head and just keep the shank of the bolt, but represent the shank with beam elements.

    In older releases of ANSYS, you had to go back to CAD and draw a line at the center of the bolt so there was a line body to mesh with beam elements.


    In newer releases of ANSYS, they have automated away the task of drawing the line body. Now it is as simple as choosing Beam Connection, and picking an edge or face for the head end and an edge or face for the nut end of the bolt shank.


    A common modeling situation is to have two thin plates come together and be welded. A simple representation is a midsurface shell model. In older releases of ANSYS, you could use Bonded Contact and set the Behavior to MPC so you could see the connection elements of the Bonded Contact. This works great for transferring a load from one end of a part to the other, but if it is a long weld seam, you don't get a local measure of the force going through each connection element.

    In a newer release of ANSYS, they added the ability to replace the MPC connection elements with Beam elements. Now you can extract the axial and shear force from each individual beam element along the weld seam. This makes evaluation of weld strength much easier.

    The user interface for Bonded Contact got a new capability to select a behavior of Beams instead of an MPC type of connection.


    Back to the Beam Connection capability, the default behavior is the MPC end condition of Rigid. It never occurs to me to change the behavior to Beam. Just like the Swiss knife, while I'm using the scissors, I don't pull out the bottle opener, it would only be in the way.

    You might suggest that the developers hide the ability to set the behavior to Beams when doing a Beam Connection. In the meantime, you can just ignore that capability.

    ANSYS offers AIM, which has a simpler user interface with a limited selection of options as an alternative to Workbench.

  • GeorgeAerospaceGeorgeAerospace EgyptMember
    edited February 16

    Dear peteroznewman

    I thought I can model the bolt accurately and efficiently using Ansys beam connection. To do so, instead of the 3D model in your video tutorial, it is enough to just:

    1) Spider MPC from the upper-hole-edge-center to all nodes within a circle offset from upper hole edge, to have the diameter of the bolt head

    2) similar spider MPC from the upper-hole-edge-center to all nodes within a circle offset from lower hole edge, to have the diameter of the bolt head

    3) 1-D beam element connecting the centers of the above two spider elements

    This is what exactly done using NX "Bolted connection".

    I wished Ansys can do the same using Ansys beam connection. I thought that the "Radius" or "Pinball region" properties can do the same as NX bolted connection. To confirm this, I have created the shown test problem. I tested all the behaviors of the beam connections ("Beam", "Rigid" and "Deformable"). To be sure, I exported the fem model from "Mechanical" to an ANSYS input file and opened it and confirmed that Ansys just creates a spider element and connects it only to nodes on the edge nodes. That is, Ansys beam connection cannot model the bolt nut nor head using any of the "Radius" or "Pinball region" properties. I began to believe these properties are buggy and has no effect at all.


    If I'm wrong, please correct me.

    Otherwise, do you know how can I submit this bug or suggestion to Ansys programmers?




  • peteroznewmanpeteroznewman Member
    edited February 18

    Dear George,

    You've got it wrong.

    I understand the NX way of doing bolt connections. In fact, I have a video on that topic that I just uploaded to my YouTube channel, but this is not an appropriate place to show NX videos!  I understand it's frustrating when ANSYS does things differently to NX.

    You don't understand what Pinball does. To have the effect you want, you must pick the face, not the edge. I demonstrate this in a followup video to my original solid body fastener tutorial.

    The default Behavior when a Beam Connection is made is Rigid. Why do you insist on changing it to Beam? That is not useful. Stop doing that. If you want, you can put in an enhancement request to ANSYS that when a Beam Connection is being defined, the Behavior list is only the two MPC types of Rigid and Deformable. I would support that.

    I'm not ANSYS staff, but they do read these posts and maybe one of them can submit this as an enhancement request for you. Over the years, I have submitted a few enhancement requests to ANSYS through my ANSYS Elite Partner, Simutech Group, and one of them was implemented!

  • GeorgeAerospaceGeorgeAerospace EgyptMember
    edited February 18

    Thanks a lot for your useful help...

  • peteroznewmanpeteroznewman Member
    edited February 18

    You're welcome. Please mark a post with Is Solution (when you are logged in) so that the Discussion is marked as Solved.

Sign In or Register to comment.