Selecting faces of a line body mesh

Hi

I have extracted a beam profile from a model in spaceclaim. In design modeler, I want to apply a remote force on the face of the beam, but I am unable to select the face of the beam (mesh) as beams are represented as line bodies. I am trying to obtain the bending moment results from a remote force that acts on the width of a beam and the bending moment results from a remote force that acts on the length of a beam. Is there any way around this?

Comments

  • peteroznewmanpeteroznewman Member
    edited January 25

    What do you mean "remote force"?  How remote are you talking about?

    Once you abstract a solid body to a line body, you have to apply all the forces to the line body. There are no faces anymore. Mechanical can display the cross section but that is for display only. It is a line body.

  • usernameeeeeeusernameeeeee Member
    edited January 25

    The model is essentially an L that is fixed at one end and has a force applied on the other. There are two beams welded together to create the L geometry and I want to get the bending moment results of the beam that is fixed at one end. Basically my problem is that if I create the entire geometry (i.e. both beams)  it will be a solid model, and I am unable to obtain beam results since its a solid model. As a resut, I found out about remote forces and simplified my geometry to one beam and tried to apply one where the force would act on the model.

     

    So if I have to use the line bodies, how would I connect them to simulate the welded connection between the beams. This may sound really simple, but I am pretty much a novice when it comes to ansys.

     

    **** This is the last edit I will make to this reply. Apologies.

  • peteroznewmanpeteroznewman Member
    edited January 25
    In SpaceClaim you Merge the two rectangular sections into a single solid body that has an L-shaped cross-section. Then when you extract the beam, SpaceClaim will create the section properties for the L beam and create a line body. You apply loads to that.
  • usernameeeeeeusernameeeeee Member
    edited January 25

    I see "Merge Faces"' underneath the repair tab in the adjust subsection and "Connect" underneath the prepare tab in the beam subsection. So I should use the "Merge Faces" option ? And would it make a difference if I selected "maintain tangency" or not ?

     

    I'm actually getting an error when I'm trying to merge the faces. "Could not replace faces with a single face"

     

    Edit: Never mind I think I found it in the "Design" tab in the intersect subsection. The tool was called "Combine" and the description says "Merge or split objects..."

     

     

  • usernameeeeeeusernameeeeee Member
    edited January 25

    Now when I try to extract the beams I get an error "Failed to extract 3 beams"

    The beams are hollow. Would that affect anything ?

     

     

  • peteroznewmanpeteroznewman Member
    edited January 26

    Yes, Combine is the name in SpaceClaim. I was going from memory and have too many programs that all use different names for the same thing!

    SpaceClaim can handle hollow beams. If you attach the .scdoc file to your reply, I will take a look, but say what version of ANSYS you are using.

    Or you can insert some images in your reply. 

  • usernameeeeeeusernameeeeee Member
    edited January 26

    I can't really post the file/images on this forum since it would public. However, are there certain conditions that would cause this error to occur?

  • peteroznewmanpeteroznewman Member
    edited January 26

    You could create some shapes that are not proprietary but exhibit the same error for public display.

    One condition that will cause the extraction of a beam to fail is if the body is not a pure extrusion of the end face. For example if there is a cross-drilled hole, or if the beam is tapered.

  • usernameeeeeeusernameeeeee Member
    edited January 26

    I am using Ansys 2019 R2

     

    Thank you for the suggestion. I created another L beam with different dimensions and noticed something. I made the cross sectional area the same for both beams at first and I was able to successfully extract the beams. I then made the cross sectional area of one beam slightly larger, which is actually representative of my model, and again I was met with the same "failed to extract 2 beams" error. Also notable, now its "failed to extract 2 beams" rather than "failed to extract 3 beams" as the error appeared in my model.

    I attached the L beam which is showing the error.

  • peteroznewmanpeteroznewman Member
    edited January 26

    This solid body breaks the rule I described above. Each beam must be a pure extrusion of one end face.  Look at the orange face. I created a plane on the underside of the top tube and used Split Body to create two separate bodies. Now you can extract two beam. However, since the beams are welded together, I would pull the vertical tube end face up 6 mm to the midpoint of the top tube and pull the top tube back 5 mm as shown in the third image. Now the end points of the two beams meet at the same coordinates and will be easy to "weld" together by using the Share button on the Workbench tab (last image).

  • usernameeeeeeusernameeeeee Member
    edited January 26

    Thank you. Where do you go in spaceclaim to create a plane? Additionally what method did you use to pull/move the beams in such a way?

  • peteroznewmanpeteroznewman Member
    edited January 26

    On the Design tab, you can see the Plane button the Split Body button, and the Pull tool.

  • usernameeeeeeusernameeeeee Member
    edited January 26

    OK, I figured out how to split and pull.

    Also, to clarify, even though we pulled the beams in such a manner, the actual welded setup of the beams is still simulated. Is that correct ?

     

    Edit: There was a failed to attach geometry error, but I somehow got around it.

     

    Thank you

  • usernameeeeeeusernameeeeee Member
    edited January 26

    In mechanical, are the meshes for both beams supposed to combine to effectively create an L shaped mesh? Because it looks like a mesh was just created for each beam separately and not combined. The meshes do instersect each other, but they seem to be seperate; for example, each mesh also has different colors.

     

    Also, mechanical is acting weird. I applied a fixed support and force to the line bodies and tried to solve, but got a solver error: general error. Then I retried and eventually mechanical closed. Now when I re open mechanical, the configuration of the line bodies as shown below are not connected as they appear in space claim. I have opened the geometry in spaceclaim and the line bodies are still connected. I'm going to try closing and opening workbench.

     

  • peteroznewmanpeteroznewman Member
    edited January 26

    The welding occurred when you clicked the Share button on the Workbench tab in SpaceClaim.

    The Fixed Support goes on a Vertex, the force can go on a vertex for a tip load or a line body for a distributed load.

  • usernameeeeeeusernameeeeee Member
    edited January 26

     Yes, I understand. However, my geometry is not appearing as connected when I open mechanical.

  • peteroznewmanpeteroznewman Member
    edited January 26

    In Workbench, File Archive and create a .wbpz file that you can attach after you post your reply and I will take a look.

  • usernameeeeeeusernameeeeee Member
    edited January 26

    I recreated the geometry in spaceclaim and obtained success. Thank you !

  • peteroznewmanpeteroznewman Member
    edited January 27

    Great!  Please choose a post to mark with Is Solution to mark the Discussion as Solved.

Sign In or Register to comment.