General Mechanical

General Mechanical

Problem with bolt pretension

    • sh ga
      Subscriber

      Dear all,


      I have a support structure upon which there is a steel plate. This plate is connected to another plate. Between these two plates,  i have used beam connection from body-body connection and there is frictional contact between the two plates.



       


       


      I am applying the bolt pretension on these beam connections.



      I am expecting that the bolt pretension force will act in compression but when i run the simulation, bolt pretension is acting in the opposite direction. The below screen shot shows the deformation after 2 sub steps but it is clearly seen that the two plates are separated because of the bolt pretension.



      Can anybody help me here? I don't know what i am doing wrong here.

    • argenisbnl
      Subscriber

      Hello, I was working with a bolted flat cover of a cylindrical pressure vessel, and i had the very same problem, and if my memory don't fail, what i had to do was creating a new coordinate system on the bolt, and select that coordinate system at the Bolt Pretension manager. 


      Worth noting that I simulated just a part of the solid, and use cyclic region symmetry. 


      Good luck.


    • sh ga
      Subscriber

      Hi Argenisbnl,


      Thank you for your quick response. In your screen shot i see that you have solid body of a fastener. But in my case i am using body-body beam connection and when i apply bolt pretension on beam connection, it is not possible to choose the coordinate system as far as i know. Do you know how to select coordinate system for the beam connection?


       


       

    • argenisbnl
      Subscriber

      Hello, i don't know much about beam connection, that's why I have solid body of a fastener, but this video may help you.


    • peteroznewman
      Subscriber

      Hello sh ga,


      If you still have a problem, I am willing to look at your model to see if I can find the mistake.  Please Attach a Workbench Project Archive .wbpz file after you reply.


      If there was a contact offset defined between the plates, that would explain it, but by default, that would be set to 0.


      Regards,


      Peter

    • sh ga
      Subscriber

      Hi Peter,


       


      I can not share the modal because of confidentiality. There is a frictional contact between the plates and offset is set to default. I used line bodies for the bolt shank and used joints to connect line bodies to the plates. Now it is working as expected. Still i don't know why it was not working with body-body beam connection. 


       


      I have one question though. If there is an offset value applied in the contact between the plates, then will it affect the bolt pretension?

    • sh ga
      Subscriber

      Hi Argenisbnl,


       


      Thank you for sharing this video. I use the method explained in the video and it is working as expected now.

    • peteroznewman
      Subscriber

      Hi sh ga,


      If you apply an offset to the contact definition, that will be applied in step 1 at the same time the pretension load is ramping up, so they will both be present at the end of step 1.


      If you need help while working on this confidential model, and cannot get it resolved through posts alone, you might consider making a generic version of the model that has no confidential features, but has the same problem you are trying to resolve so you can share the generic model.


      Regards,
      Peter

    • sh ga
      Subscriber

      Hi Peter,


       


      Thank you for your help. So if there are mid surfaces connected by the bolts in the assembly and in the contact generated between the mid-surfaces, offset value is applied then body-body beam connection won't work. Is this true?


       


      I will try to solve it first by myself and if problem still exists then i will make one generic case and share it with you. 

    • peteroznewman
      Subscriber

      Hi sh ga,


      Yes, if you have two midsurfaces, the contact has a Shell Thickness property that can be set to Yes so that it put the offset in for you automatically.


      If the plates become midsurfaces, you do the same with the line body. Make a fixed joint between the vertex of the line body and the circle in the midsurface, and repeat for the other midsurface and the other end of the line body. The pretension can be applied to the line body the same as you have already done.


      Regards,


      Peter

    • sh ga
      Subscriber

      Hi Peter,


       


      Thank you for this information. I have two more questions. Can you please help me with them?



      • I am getting a warning message that the intersection is not found between element 330030 and element 330482. But in the mesh i have only 201244 elements. How to find the problematic region?

      • Second warning message is Contact element 377580 (real ID 204) status changes abruptly from no-contact -> contact (with target element 384863). I have more than 30 contacts in the assembly. How to recognize the warning message is for which contact?


      I am trying to locate the problematic region but i couldn't find. Can you please tell me a way to locate the region for respective warning messages?

    • Sandeep Medikonda
      Ansys Employee

      Sh ga,


        Those other elements could correspond to the Contact/Target elements.


        If you right-click on the Error/Warning message and select Go to Object, it should take point you to the offending contact.


        Hope this helps.


      Regards,


      Sandeep

    • sh ga
      Subscriber

      Hi Sandeep,


       


      The first warning message which says intersection not found doesn't appear in the message window but it is in the output file. Do you know any other way to locate the region?

    • Sandeep Medikonda
      Ansys Employee

      Sh ga,


        Create a named selection of the offending elements since you know their IDs and they should help you identify which contact is creating this problem in the model.


        If you are using v19 or above, you can just hit 'M' on your keyboard and this will bring up a dialog box to enter a node/element number.


      Regards,


      Sandeep

    • sh ga
      Subscriber

      Hi Sandeep,


       


      I am getting a warning message that the intersection is not found between element 330030 and element 330482. But in the mesh i have only 201244 elements. So when i use named selection, it can not select the element as these are the contact elements. Do you know any other way to identify the region?


       

    • Sandeep Medikonda
      Ansys Employee

      Hi Sh ga,


        Use the worksheet and manually enter these values.

    • sh ga
      Subscriber

      Hi Sandeep,


      Do you have any tutorial or screen shot of using worksheet? It would be a great help if you can share some tutorials or screen shots. Thank you.

    • Sandeep Medikonda
      Ansys Employee

      It's usually us asking for images :-). Here you go, please see these articles from the manual:


      Help Page 1


      Help Page 2


      Help Page 3


      Article


      Regards,


      Sandeep

    • sh ga
      Subscriber

       Hi Sandeep,


      Thank you for sending these articles. Since you were asking for images, i am attaching them here. In the finite element model, i have 107517 elements. See the screen shot below.


      Num. of nodes and elements


      Now, in the output file, i am getting a warning message which is in the screen shot below. By the way this warning message does not appear in the message box. So can not right click on it to identify the problematic region.


      warning message


      Now, you told me to use the named selection to identify the problematic region. So i created the named selection, and enter the element id to identify the region. But named selection is not selecting anything. Please see the screen shot below.


       


      named selection


      So, i still don't know how to identify the the problematic region. Can you please tell me how to identify this region?


       


      Thank you.


       


       

    • Sandeep Medikonda
      Ansys Employee

      Sh ga,


         I might have misspoken here, I apologize. I vaguely remember doing something like this in a model a while ago but looks like you are only able to query solid elements here. But, I am sure that there is a different way to identify real ids even if this needs a command object. Let me find out and get back to you.


      Regards,


      Sandeep

    • sh ga
      Subscriber

      Hi Sandeep,


      Please let me know if you find out a way to locate them. Thank you.

    • Sandeep Medikonda
      Ansys Employee

      Sh ga,


      Can you put a small command snippet in your solution as shown:


      /show,png
      ESEL,S,ELEM,,525
      nsle,s,1
      /auto /view,1,1,1,1
      eplot

      This should plot the element of interest:



      Now, if you have the real id from your initial contact, you can use the following commands to plot these as well (say for a real ID of 4 in this case and CONTA174 elements)


      /show,png
      set,2,last
      esel,s,real,,4
      esel,r,ename,,CONTA174
      nsle,s,1
      esln,s,1
      /auto /view,1,1,1,1
      eplot

      If none of this helps, see if you are able to take the results to MAPDL and plot them using the commands discussed above:



       


      Hope this helps!


      Regards,


      Sandeep

Viewing 21 reply threads
  • You must be logged in to reply to this topic.